Manual En

User Manual: Pdf

Open the PDF directly: View PDF .
Page Count: 348 [warning: Documents this large are best viewed by clicking the View PDF Link!]

Chapter 1 Introduction
Chapter 2 Installation
Chapter 3 EAGLE Modules and Editions
- 3.1 EAGLE Modules
- 3.2 Different Editions
Chapter 4 A First Look at EAGLE
Chapter 5 Principles for Working with EAGLE
Chapter 6 From Schematic to Finished Board
Chapter 7 The Autorouter
Chapter 8 Component Design Explained through Examples
Chapter 9 Preparing Manufacturing Data
Chapter 10 Appendix

EASILY APPLICABLE GRAPHICAL LAYOUT EDITOR

Version 8.4

Manual

71023841

This software and documentation are copyrighted by Autodesk, doing business under

the trade name EAGLE. The software and documentation are licensed, not sold, and

may be used or copied only in accordance with the EAGLE License Agreement

accompanying the software and/or reprinted in this document. This software

embodies valuable trade secrets proprietary to Autodesk.

Specifications subject to change without notice.

No part of this publication may be reproduced, stored in a retrieval system, or

transmitted, in any form or by any means, electronic, mechanical, photocopying,

recording, scanning, digitizing, or otherwise, without the prior consent of Autodesk.

Printing this manual for your personal use is allowed.

Windows is a registered trademark of Microsoft Corporation.

Linux is a registered trademark of Linus Torvalds.

Mac is a registered trademark of Apple Computer, Inc.

Table of Contents
Chapter 1   Introduction...................................................19
1.1  What is in this Manual?................................................................19
1.2  Important Changes......................................................................20
 SPICE Simulation..........................................................................20
 Live Design Rule Check.................................................................20
 WINDOW Command – Flip Board View......................................20
 Routing Direction..........................................................................20
 SLICE Command............................................................................21
 User Language................................................................................21
 FUSIONSYNC Command...............................................................21
 Managed Libraries..........................................................................21
 Board Contour Detection...............................................................21
 New EAGLE Internal Vector Font.................................................21
 ROUTE Command..........................................................................21
 Managed Libraries.........................................................................22
 Design Blocks.................................................................................22
 ROUTE command..........................................................................22
 Copy/Paste.....................................................................................22
 Design Rule Check.........................................................................22
 ALIGN command...........................................................................22
 ROUTE command..........................................................................22
 BGA Router....................................................................................23
 New Installer Routines and Subscription Licenses......................23
 Flexible Board size in Free and Standard Edition........................23
 Reworked Icons..............................................................................23
 Pin Snapping in the Schematic......................................................23
 Renamed WIRE Command to LINE.............................................23
 New SLICE command....................................................................23
 ROUTE Command Improvements................................................23
 Route Start Selection...................................................................23
 Undo Mouse Clicks......................................................................24
 Electrical Snap Indicator.............................................................24
 Loop Remove...............................................................................24
 Via Placement and Change of Routing Layers............................25
 BGA Autorouter..............................................................................25
 Design Blocks.................................................................................25
1.3  General Comments About EAGLE Component Libraries...........26
1.4  Technical Terms...........................................................................26
Chapter 2   Installation....................................................29
2.1  System Requirements..................................................................29
2.2  Installation of the EAGLE package.............................................29
3

Table of Contents
2.3  Updating an Older Version..........................................................29
 First Back up, Then Install............................................................29
 Notes on Library Files....................................................................30
 In Case of Changes in the File Data Structure..............................30
2.4  First Start of EAGLE...................................................................30
2.5  Language Settings........................................................................31
 Windows.........................................................................................31
 Linux and Mac OS X.......................................................................31
Chapter 3   EAGLE Modules and Editions.........................33
3.1  EAGLE Modules...........................................................................33
 The Layout Editor..........................................................................33
 Schematic Editor............................................................................33
 Autorouter......................................................................................33
3.2  Different Editions........................................................................34
 Premium Edition............................................................................34
 General.........................................................................................34
 Schematic Editor..........................................................................35
 Layout Editor...............................................................................35
 Autorouter Module......................................................................36
 Standard Edition............................................................................36
 Free Edition....................................................................................36
Chapter 4   A First Look at EAGLE...................................39
4.1  The Control Panel........................................................................39
 Documentation..............................................................................40
 Libraries Summary........................................................................40
 Design Blocks.................................................................................42
 Design Rules...................................................................................42
 User Language Programs, Scripts, CAM Jobs..............................43
 Projects...........................................................................................43
 Menu Bar........................................................................................44
 File Menu.....................................................................................44
 View Menu...................................................................................45
 Options Menu..............................................................................46
 Window Menu..............................................................................49
 Help Menu...................................................................................50
4.2  The Schematic Editor Window....................................................50
 How You Obtain Detailed Information About a Command..........51
 User Guidance..............................................................................51
  Help Function..............................................................................51
 Command Parameters...................................................................52
  GRID............................................................................................53
 The Action Toolbar.........................................................................53
  USE..............................................................................................53
4

Table of Contents
  SCRIPT........................................................................................53
  RUN.............................................................................................53
  WINDOW....................................................................................53
  UNDO/REDO.............................................................................54
  Stop Icon.....................................................................................54
  Go Icon........................................................................................55
 The Command Toolbar of The Schematic Editor.........................55
  INFO............................................................................................55
  SHOW..........................................................................................55
  DISPLAY......................................................................................55
  MARK..........................................................................................55
  MOVE..........................................................................................56
  COPY...........................................................................................56
  MIRROR.....................................................................................56
  ROTATE......................................................................................56
  GROUP........................................................................................56
  CHANGE.....................................................................................57
  PASTE..........................................................................................57
  DELETE.......................................................................................57
  ADD.............................................................................................57
  PASTE DBL.................................................................................58
  PINSWAP....................................................................................58
  GATESWAP................................................................................58
  REPLACE....................................................................................58
  NAME..........................................................................................58
  VALUE........................................................................................58
  SMASH........................................................................................58
  MITER.........................................................................................59
  SPLIT...........................................................................................59
  SLICE..........................................................................................59
  INVOKE......................................................................................59
  LINE (was WIRE).......................................................................59
  TEXT...........................................................................................60
  CIRCLE.......................................................................................60
  ARC.............................................................................................60
  RECT...........................................................................................60
  POLYGON...................................................................................60
  BUS.............................................................................................60
  NET.............................................................................................60
  JUNCTION..................................................................................61
  LABEL..........................................................................................61
  ATTRIBUTE................................................................................61
  DIMENSION...............................................................................61
  MODULE.....................................................................................61
  PORT...........................................................................................62
5

Table of Contents
  ERC..............................................................................................62
 Commands Not Available in the Command Toolbar....................62
 ASSIGN........................................................................................62
 CLASS...........................................................................................62
 CLOSE..........................................................................................62
 CUT..............................................................................................62
 EDIT.............................................................................................62
 FRAME.........................................................................................63
 EXPORT.......................................................................................63
 LAYER..........................................................................................63
 MENU..........................................................................................63
 OPEN............................................................................................63
 PACKAGE.....................................................................................63
 PRINT..........................................................................................64
 QUIT.............................................................................................64
 REMOVE......................................................................................64
 SET...............................................................................................64
 TECHNOLOGY............................................................................64
 UPDATE.......................................................................................64
 VARIANT.....................................................................................64
 WRITE..........................................................................................65
 Mouse Keys.....................................................................................65
 Selecting Neighbouring Objects..................................................65
4.3  The Layout Editor Window.........................................................65
 The Commands on the Layout Command Toolbar.......................66
  INFO............................................................................................66
  SHOW.........................................................................................66
  DISPLAY......................................................................................67
  MARK..........................................................................................68
  GROUP........................................................................................68
  MOVE..........................................................................................68
  MIRROR.....................................................................................68
  ROTATE......................................................................................69
  ALIGN.........................................................................................69
  COPY...........................................................................................69
  PASTE.........................................................................................69
  DELETE......................................................................................69
  CHANGE.....................................................................................70
  PASTE DBL.................................................................................70
  ADD.............................................................................................70
  PINSWAP....................................................................................70
  REPLACE....................................................................................70
  LOCK............................................................................................71
  NAME..........................................................................................71
  VALUE.........................................................................................71
6

Table of Contents
  SMASH........................................................................................71
  MITER.........................................................................................71
  SPLIT...........................................................................................72
  OPTIMIZE...................................................................................72
  MEANDER..................................................................................72
  SLICE...........................................................................................72
  ROUTE........................................................................................72
  RIPUP..........................................................................................73
  LINE............................................................................................73
  TEXT............................................................................................73
  CIRCLE........................................................................................74
  ARC..............................................................................................74
  RECT...........................................................................................74
  POLYGON...................................................................................74
  VIA...............................................................................................75
  SIGNAL.......................................................................................75
  HOLE...........................................................................................75
  ATTRIBUTE................................................................................75
  DIMENSION...............................................................................75
  RATSNEST..................................................................................76
  AUTO...........................................................................................76
  AUTO BGA..................................................................................76
  ERC..............................................................................................76
  DRC.............................................................................................76
  ERRORS......................................................................................77
4.4  The Library Editor Window.........................................................77
 Table Of Contents...........................................................................77
 Important Icons in the Library Editor..........................................79
 The Package Editing Mode............................................................79
 Design New Package...................................................................80
  PAD.............................................................................................80
  SMD............................................................................................80
 The Symbol Editing Mode.............................................................80
 Design a New Symbol..................................................................81
  PIN...............................................................................................81
 The Device Editing mode...............................................................81
 Create Actual Components from Symbols and Packages...........82
  ADD.............................................................................................82
  NAME..........................................................................................82
  CHANGE.....................................................................................83
 PACKAGE....................................................................................83
 CONNECT....................................................................................83
 PREFIX........................................................................................83
 VALUE.........................................................................................83
 TECHNOLOGY............................................................................83
7

Table of Contents
  ATTRIBUTE................................................................................83
 DESCRIPTION............................................................................83
4.5  The CAM Processor.....................................................................84
 Generate Data................................................................................84
 Starting the CAM Processor........................................................84
 Load Job File................................................................................85
 Load Board...................................................................................85
 Set Output Parameters................................................................85
 Start Output.................................................................................85
 Define New Job............................................................................85
4.6  The Text Editor Window.............................................................86
Chapter 5   Principles for Working with EAGLE...............87
5.1  Command Input Possibilities.......................................................87
 Activate Command and Select Object...........................................87
 Command Line...............................................................................87
 History Function............................................................................88
 The Context Menu.........................................................................88
 Function Keys................................................................................89
 Script Files.....................................................................................90
 Mixed Input....................................................................................91
5.2  The EAGLE Command Language................................................91
 Typographical Conventions...........................................................91
 Enter key and Semicolon.............................................................91
 Bold Type or Upper Case.............................................................92
 Lower Case...................................................................................92
 Underscore...................................................................................92
 Spaces...........................................................................................92
 Alternative Parameters................................................................92
 Repetition Points.........................................................................93
 Mouse Click..................................................................................93
 Entering Coordinates as Text........................................................93
 Relative values:............................................................................94
 Polar values:.................................................................................94
 Right Mouse Click:.......................................................................94
 Modifier:......................................................................................94
5.3  Grids and the Current Units........................................................95
5.4  Aliases for DISPLAY, GRID, and WINDOW...............................97
 Example: DISPLAY Alias...............................................................97
 Example: GRID Alias.....................................................................97
 Example: WINDOW Alias.............................................................98
 Editing, Renaming, Deleting of an Alias.......................................98
5.5  Names and Automatic Naming...................................................99
8

Table of Contents
 Length.............................................................................................99
 Forbidden and Special Characters................................................99
 Automatic Naming.........................................................................99
5.6  Import and Export of Data..........................................................99
 Script Files and Data Import.......................................................100
 File Export Using the EXPORT Command.................................100
 DIRECTORY..............................................................................100
 NETLIST.....................................................................................101
 NETSCRIPT................................................................................101
 PARTLIST...................................................................................101
 PINLIST......................................................................................101
 SCRIPT.......................................................................................101
 IMAGE........................................................................................101
 LIBRARIES................................................................................102
5.7  The EAGLE User Language.......................................................103
5.8  Forward&Back Annotation........................................................104
5.9  Configuring EAGLE Individually...............................................104
 Configuration Commands............................................................104
 The Menu Options/Set (SET Command)....................................105
 Display Certain Layers Only......................................................105
 Context Menu Entries................................................................105
 Contents of The Parameter Menus............................................106
 ROUTE Command Settings.......................................................106
 Confirm Message Dialogs Automatically..................................107
 Color Settings...............................................................................107
 Miscellaneous SET Options.........................................................109
 The eagle.scr File...........................................................................111
 The eaglerc File.............................................................................113
 EAGLE Project File.......................................................................113
Chapter 6   From Schematic to Finished Board...............115
6.1  Creating the Schematic Diagram................................................115
 Open the Schematic Diagram.......................................................115
 Set the Grid...................................................................................116
 Place Symbols................................................................................116
 Load Drawing Frame..................................................................116
 Place Circuit Symbols (Gates)....................................................118
 Hidden Supply Gates..................................................................118
 Devices with Several Gates.........................................................119
 Designlink – Access to Farnell's Online Product Database......119
 Wiring the Schematic Diagram...................................................120
 Draw Nets (NET).......................................................................120
 Defining Cross-References for Nets...........................................121
 Cross-References for Contacts...................................................122
9

Table of Contents
 Specifying Net Classes................................................................123
 Drawing a bus (BUS).................................................................124
 Pinswap and Gateswap.................................................................125
 Power Supply................................................................................126
 Define Attributes..........................................................................127
 Global Attributes........................................................................127
 Attributes for Elements..............................................................127
 ERC – Check and Correct Schematic..........................................130
 Organize Schematic Sheets..........................................................132
 Points to Note for the Schematic Editor......................................132
 Superimposed Pins....................................................................132
 Open Pins when MOVEing........................................................132
 Duplicating a Section of the Schematic.......................................132
 With Consistent Layout.............................................................133
 Merge Different Schematic Files..................................................133
 With Consistent Layout.............................................................134
 Multi-Channel Devices...............................................................134
 Design Blocks................................................................................134
 Adding Design Blocks into Your Current Design......................135
 Save a Drawing as a Design Block.............................................135
 Save a Selection of the Drawing as a Design Block...................136
 Selection criteria.........................................................................137
6.2  The Hierarchical Schematic.......................................................137
 Creating a Module........................................................................137
 Define Ports..................................................................................140
 Using Module Instances...............................................................141
 Resulting Component Names in the Layout................................142
 ModulInstanceName:PartName...............................................142
 Offset..........................................................................................142
 Assembly Variants for Modules...................................................142
 Special Features between Schematic and Layout........................143
 SHOW command.......................................................................143
 Consistency.................................................................................143
6.3  Considerations Prior to Creating a Board..................................143
 Checking the Component Libraries.............................................143
 Agreement with the Board Manufacturer...................................144
 Specifying the Design Rules.........................................................144
 General Principles......................................................................145
 Layers.........................................................................................146
 Minimum Clearance and Distance............................................147
 Sizes............................................................................................147
 Restring (Pad and Via Diameter)..............................................148
 Shapes........................................................................................150
 Supply.........................................................................................151
10

Table of Contents
 Masks..........................................................................................152
 Misc.............................................................................................153
6.4  Create Board..............................................................................153
 Without the Schematic.................................................................154
 Specify the Board Outline............................................................154
 Arrange Components....................................................................156
 Attributes for Components and Global Attributes......................158
 Boards with Components on Both Sides.....................................158
 Exchanging Packages...................................................................159
 PACKAGE Command.................................................................159
 REPLACE command..................................................................160
 Changing the Technology.............................................................161
 Define Forbidden Areas................................................................161
 Routing – Placing Tracks Manually.............................................161
 Walkaround Obstacles................................................................161
 Ignore Obstacles.........................................................................161
 How to route...............................................................................161
 Un-route traces..........................................................................163
 Traces with arcs..........................................................................163
 Defining a Copper Plane with POLYGON...................................164
6.5     FUSIONSYNC   –   Synchronise   EAGLE   Board   and   Fusion   3D
Board Model.....................................................................................167
 How does this work?.....................................................................167
 Synchronise with Fusion............................................................167
 What if There Need to be Changes in the Board’s Geometry?. 167
 How to Synchronise...................................................................167
 View on Web...............................................................................170
 Pull from Fusion.........................................................................170
 Push to Fusion............................................................................171
6.6  DRC – Checking the Layout and Correcting Errors...................173
 The DRC Errors Window.............................................................174
 Error Messages and their Meaning..............................................175
6.7  Multilayer Boards.......................................................................178
 Inner Layer...................................................................................178
 Supply Layers with Polygons and More than One Signal.........178
 Resticted Areas For Polygons....................................................179
 Multilayer Boards with Through Vias..........................................179
 Layer Setup.................................................................................179
 Multilayer with Blind and Buried Vias........................................180
 Disambiguation..........................................................................180
 Displaying Vias...........................................................................181
 Layer Setup.................................................................................181
 Hints For Working With Blind, Buried, and Micro Vias..........186
11

Table of Contents
 Micro Via − A Special Case of Blind Via......................................187
6.8  Editing and Updating Components...........................................187
 Open Device/Symbol/Package....................................................187
 Updating Project (Library Update).............................................188
6.9  Differential Pairs And Meanders...............................................189
 Routing Differential Pairs............................................................189
 Meanders......................................................................................190
 Length Balance for a Differential Pair......................................190
 Specifying a Certain Length.......................................................191
 Symmetric and Asymmetric Meanders.....................................191
 Length Tolerance Display...........................................................191
6.10  Assembly Variants....................................................................192
 Creating Assembly Variants.........................................................192
 Assembly Variants and CAM Processor......................................194
6.11  Print Out Schematic and Layout...............................................195
 Settings of the Print Dialog..........................................................195
6.12  Combining Small Circuit Boards on a Common Panel............197
6.13  Consistency Lost between Schematic and Layout....................198
 Criteria For Consistency..............................................................200
 Consistency Indicator..................................................................201
Chapter 7   The Autorouter............................................203
7.1  Basic Features............................................................................203
7.2  What Can be Expected from the Autorouter.............................204
7.3  Controlling the Autorouter........................................................204
 Bus Router....................................................................................205
 Routing Pass................................................................................205
 TopRouter....................................................................................205
 Optimization................................................................................205
7.4  What Has to be Defined Before Autorouting.............................206
 Design Rules................................................................................206
 Track Width and Net Classes......................................................206
 Grid..............................................................................................206
 Placement Grid..........................................................................206
 Routing Grid..............................................................................207
 Memory Requirement.................................................................208
 Layer............................................................................................208
 Preferred Directions....................................................................209
 Restricted Areas for the Autorouter............................................209
 Cost Factors and Other Control Parameters...............................210
7.5  The Autorouter Menu................................................................210
 Autorouter Main Setup................................................................210
 Routing Variants Dialog...............................................................211
7.6  How the Cost Factors Influence the Routing Process................213
12

Table of Contents
 Layer Costs....................................................................................214
 cfBase.xx: 0..20..........................................................................214
 Costs..............................................................................................214
 cfVia: 0..99.................................................................................214
 cfNonPref: 0..10.........................................................................214
 cfChangeDir: 0..25.....................................................................214
 cfOrthStep, cfDiagStep..............................................................215
 cfExtdStep: 0..30........................................................................215
 cfBonusStep, cfMalusStep: 1..3..................................................215
 cfPadImpact, cfSmdImpact: 0..10.............................................215
 cfBusImpact: 0..10.....................................................................215
 cfHugging: 0..5...........................................................................216
 cfAvoid 0..10...............................................................................216
 cfPolygon 0..30...........................................................................216
 Maximum......................................................................................216
 mnVia 0..30................................................................................216
 mnSegments 0..9999.................................................................216
 mnExtdSteps 0..9999................................................................216
7.7  Number of Ripup/Retry Attempts.............................................216
7.8  Routing Multi-Layer Boards with Polygons...............................217
7.9  Backup and Interruption of Routing..........................................218
7.10  Information for the User..........................................................218
 Status Display...............................................................................218
 Log file..........................................................................................220
7.11  Evaluate the Results.................................................................220
7.12  Parameters of a Control File.....................................................221
7.13  Practical Hints..........................................................................222
 General.........................................................................................222
 Single-Sided Boards.....................................................................222
 SMD Boards With Supply Layers................................................222
 What can be done if not all signals are routed?..........................223
7.14  The Follow-me Router.............................................................223
 Partial and Full Mode..................................................................223
 Configuration...............................................................................224
 Routing Parameters.....................................................................225
 Notes.............................................................................................225
7.15  BGA Routing............................................................................226
Chapter 8   Component Design Explained through 
Examples.......................................................................229
8.1  Managed Libraries.....................................................................229
13

Table of Contents
 Migration to Managed Libraries.................................................230
 Library Manager...........................................................................231
 Make Your Libraries Managed....................................................233
8.2  Definition of a Simple Resistor.................................................234
 Resistor Package..........................................................................234
 Define a New Package...............................................................234
 Set the Grid................................................................................234
 Solder Pads................................................................................235
 Pad Name...................................................................................236
 Silkscreen and Documentation Print........................................236
 Labeling......................................................................................236
 Restricted area for components................................................237
 Description.................................................................................237
 Note............................................................................................237
 Resistor Symbol...........................................................................238
 Define a New Symbol................................................................238
 Set the Grid................................................................................238
 Place the Pins.............................................................................238
 Pin Names..................................................................................240
 Schematic Symbol.....................................................................240
 Description.................................................................................241
 Resistor Device.............................................................................241
 Define a New Device..................................................................241
 Selecting, Naming and Configuring Symbols............................241
 Selecting the Package................................................................242
 Connections Between Pins and Pads........................................242
 Define Prefix..............................................................................243
 Value..........................................................................................243
 Description.................................................................................244
 Save............................................................................................244
 Library Description......................................................................245
 Use Library...................................................................................245
8.3  Defining a Complex Device.......................................................245
 Creating a New Library................................................................247
 Drawing the Pin-Leaded Package................................................247
 Set the Grid................................................................................248
 Place Pads..................................................................................248
 Pad Name...................................................................................249
 Draw the Silk Screen Symbol....................................................249
 Package Name and Package Value............................................249
 Areas Forbidden to Components..............................................250
 Description................................................................................250
 Save.............................................................................................251
14

Table of Contents
 Defining the SMD Package...........................................................251
 Set the Grid................................................................................252
 Placing SMD Solder Pads..........................................................253
 SMD Names...............................................................................254
 Draw the Silk Screen..................................................................255
 Package Name and Package Value............................................255
 Area Forbidden to Components................................................255
 Locating Point (Origin)..............................................................255
 Description.................................................................................256
 Save............................................................................................256
 Defining the Logic Symbol for the Schematic Diagram..............257
 Check the Grid...........................................................................257
 Place the Pins.............................................................................257
 Pin Name...................................................................................258
 Draw the Symbol.......................................................................258
 Placeholders for NAME and VALUE........................................258
 Description................................................................................258
 Save............................................................................................258
 Defining a Power Supply Symbol................................................259
 Check the Grid...........................................................................259
 Place the Pins.............................................................................259
 Pin Name...................................................................................260
 Placeholders for NAME and VALUE........................................260
 Associating the Packages and Symbols to Form a Device Set....260
 Select Symbols............................................................................261
 Naming the Gates.......................................................................261
 Specify Addlevel and Swaplevel.................................................261
 Choosing the Package Variants.................................................262
 The Connect Command.............................................................263
 Defining Technologies...............................................................264
 Specifying the Prefix..................................................................265
 Value...........................................................................................265
 Description.................................................................................265
 Save............................................................................................266
8.4  Supply Voltages.........................................................................266
 Component Power Supply Pins...................................................266
 Invisible Supply Pins.................................................................266
 Pins with the Same Names..........................................................268
8.5  One Pin – Multiple Pads Connections......................................268
8.6  Supply Symbols.........................................................................269
8.7  Attributes....................................................................................271
 Define Attributes..........................................................................271
 Display Attributes........................................................................273
 Placeholders in Symbol and Package........................................273
15

Table of Contents
8.8  External Devices without Packages...........................................274
8.9  Labeling of Schematic Symbols.................................................274
8.10  More about the Addlevel Parameter........................................275
 Summary......................................................................................275
 Relay: Coil and First Contact must be Placed.............................276
 Connector: Some Connection Pins can be Omitted....................276
 Connector with Fixing Hole and Restricted Area.......................277
8.11  Defining Components with Contact Cross-References............278
 Define Symbol..............................................................................278
 Define Device................................................................................279
 Define Package.............................................................................279
8.12  Drawing Frames.......................................................................279
8.13  Components on the Solder Side...............................................281
8.14  Components with Oblong Holes..............................................281
8.15  Arbitrary Pad Shapes...............................................................282
8.16  Creating New Package Variants...............................................283
 Package from Another Library....................................................283
 Defining the Package Variant...................................................283
 Connect Command....................................................................285
 Defining Technologies...............................................................285
 Save............................................................................................285
 Using a Modified Package from Another Library.......................285
 Import the Package...................................................................285
 Defining the Variant..................................................................286
8.17  Defining Packages in Any Rotation.........................................286
 Rotating a Package as a Whole....................................................287
 Packages with Radial Pad Arrangement.....................................287
8.18  Library and Part Management................................................288
 Copying of Library Elements.......................................................288
 Within a Library........................................................................288
 From One Library into Another................................................289
 Composition of Your own Libraries..........................................291
 Removing and Renaming Library Elements...............................291
 Update Packages in Libraries......................................................292
Chapter 9   Preparing Manufacturing Data.....................295
9.1  Which Data do we Need for Board Manufacture?.....................295
 Gerber Plot Data..........................................................................296
 GERBER_RS274X.....................................................................296
 GERBERAUTO and GERBER...................................................296
 Drill Data......................................................................................297
 EXCELLON................................................................................297
 EXCELLON_RACK...................................................................297
 SM1000 and SM3000...............................................................298
16

Table of Contents
 Further Drill Data Devices........................................................298
 Prototype Manufacture With a Milling Machine.......................298
 outlines.ulp................................................................................298
 mill-outlines.ulp........................................................................298
 Film Generation Using PostScript Files......................................298
 Printing on a Film........................................................................299
 Data for Pick-and-place Machines and In-circuit Testers..........299
 Documentation............................................................................300
 Parts List....................................................................................300
 Drill Plan....................................................................................301
 Drill Legend...............................................................................302
 Assembly Variants.......................................................................302
9.2  Rules that Save Time and Money..............................................302
9.3  Quick Guide for Data Output....................................................303
 Job gerb274x.cam........................................................................304
 Job excellon.cam..........................................................................305
 Job gerber.cam............................................................................306
9.4  Which Files do I Need for my Board?.......................................307
 Files List.......................................................................................307
 Placeholders for Output File Name Generation.......................310
 Hints Concerning File Extensions:............................................310
9.5  Peculiarities of Multilayer Boards..............................................310
 Inner Layers.................................................................................310
 Drill Data for Multilayer Boards With Blind and Buried Vias....311
9.6  Set Output Parameters...............................................................311
9.7  Automating the Output with CAM Processor Jobs....................314
 Defining a New CAM Job.............................................................314
 Extending gerber.cam Job for Multilayer Boards.......................315
 Error Message: Apertures Missing..............................................316
 Gerber Info Files...........................................................................317
 Drill Data Generation with Separate Rack File...........................317
 Define a Drill Configuration (Rack) File...................................317
 Define Job for Drill Data Output...............................................318
 Drill Info File..............................................................................318
9.8  Device Driver Definition in eagle.def.........................................318
 Creating Your Own Device Driver................................................319
 Example 1: Gerber(auto) device, Millimetre.............................319
 Example 2: EXCELLON Device, Output with Leading Zeros. .319
 Units in the Aperture and Drill Table.........................................320
9.9  Gerber Files for Photoplotters with Fixed Aperture Wheels.....320
17

Table of Contents
 Defining the Aperture Table (Wheel)..........................................321
 Aperture Emulation......................................................................321
Chapter 10   Appendix....................................................323
10.1  Layers and their Usage.............................................................323
 In Layout and Package Editor.....................................................323
 In Schematic, Symbol, and Device Editor...................................324
10.2  EAGLE Files.............................................................................324
10.3  EAGLE Options at a Glance.....................................................325
10.4  Configuration of the Text Menu..............................................328
10.5  Text Variables..........................................................................329
10.6  Options for Experts in eaglerc.................................................329
 CAM Processor – Suppress Drills/Holes Warning..................330
 Change Component Value Warning.........................................330
 Consistency Check.....................................................................330
 Delete Wire Joints.....................................................................330
 Device Name as Value for all Components...............................330
 Disable Ctrl for Radius Mode....................................................330
 Group Selection..........................................................................331
 Load Matching File Automatically............................................331
 Name of Net, Busses, Signals and Polygons..............................331
 Open Project...............................................................................331
 Panning Drawing Window.........................................................331
 Polygon Edges as Continuous Lines..........................................331
 Reposition of the Mouse Cursor................................................332
 Units in Dialogs.........................................................................332
10.7  Error Messages........................................................................332
 When Loading a File....................................................................332
 Restring smaller than in older version......................................332
 Library objects with the same names.......................................332
 Pad, Via Replaced with a Hole..................................................333
 Skipped unsuitable objects........................................................334
 Can't Update File.......................................................................334
 In a Library...................................................................................335
 Package/Symbol is in use..........................................................335
 In the CAM Processor..................................................................335
 Polygon may cause extremely large plot data...........................335
 In the Free or Standard Edition..................................................336
 Can't perform the requested action..........................................336
 Index............................................................................337
18

Chapter 1

Introduction

This manual describes the use of the EAGLE software and its basic

principles. The order of chapters follows the typical process from drawing a

schematic to a ready-to-use layout.

1.1 What is in this Manual?

A chapter's main heading is intended to tell you briefly what the contents of

that chapter are. Here in the first chapter we want to give a quick overview

what you can expect from this manual.

Chapter 1 – Introduction

Contains a preview of the manual and informs you about the most

important changes compared to the previous version.

Chapter 2 – Installation

Deals with the program's installation.

Chapter 3 – EAGLE Modules and Editions

Explains the various program variants.

Chapter 4 – A First Look at EAGLE

Gives a preview of the program's structure and describes the

editor windows and their commands.

Chapter 5 – Principles for Working with EAGLE

Examines the basic ways of using and configuring EAGLE.

Chapter 6 – From Schematic to Finished Layout

Follows the route from schematic to layout.

Chapter 7 – The Autorouter

Dedicated to the Autorouter module and its configuration.

Chapter 8 – Component Design Explained through Examples

Explains the definition of library components through examples and

informs about library and component management.

Chapter 9 – Preparing the Manufacturing Data

Everything you need to know about generating manufacturing data.

Chapter 10 – Appendix

Lists useful additional information and explains some error messages

EAGLE prompts in certain situations.

1 Introduction

1.2 Important Changes

Anybody who has already been working with a prior version of EAGLE is

advised to read the file UPDATE_en.txt. It contains a description of all the

differences from earlier versions. This file is located in the eagle/doc

directory. Please read it before you start working with the new EAGLE.

Information that was not available or that has been changed since finishing

this manual is also described in UPDATE_en.txt.

Detailed information, especially about the EAGLE command language and

the EAGLE User Language, is available on the help pages.

The most important changes are listed here:

SPICE Simulation

V8.4.0 – Integrated open-source ngspice simulator with examples.

The new ngspice-simulation library contains pre-configured parts. Spice

model cards and subcircuit models, as well as native parts are supported, and

an interface is provided to map gate pins to model inputs. Valid spice-

compatible netlists are created and can optionally be manually edited before

simulation. User interface supports making spice-compatible library parts,

and for converting existing parts.

Results are given in text form and plotted where applicable. OP analysis

results are shown in schematic and can be toggled on/off.

Simulation types supported: AC, DC, Transient, and Operating Point.

Simulation related commands in EAGLE: SIM, SIMOPTOGGLE,

SOURCESETUP, MAKESPICE, MAPTOMODEL, IPROBE, VPROBE,

VPPROBE

See help for SIM command to begin.

Live Design Rule Check

V8.4.0 – After a change in the Layout, like moving a component or while

you are routing, the Design Rule Check will be executed automatically. The

errors list will be updated and the DRC error polygons will be drawn. So you

immediately will recognize any Design Rule violations. Live DRC can be

turned on or off through the Live DRC checkbox in the Set/DRC menu or

with the command SET LIVE_DRC ON | OFF.

WINDOW Command – Flip Board View

V8.4.0 – WINDOW FLIP allows for viewing and editing the board from the

perspective of the bottom side. There is also an icon available in the Action

toolbar.

Routing Direction

V8.3.2 – While the ROUTE command is active, you can use the Arrow-right

key to change the routing direction. The starting point jumps from the one

end of the airwire to the other. This can be done at any time as often as you

want.

1.2 Important Changes

SLICE Command

V8.3.2 – SLICE offers options to automatically ripup traces left or right of

the slice line. These options are available through icons in the parameter

toolbar.

User Language

V8.3.2 – The User Language supports 3D Packages and URNs

(UL_PACKAGE3D).

FUSIONSYNC Command

V8.3.0 – Data exchange between the mechanical CAD system Fusion 360

and EAGLE. This command is used to have the EAGLE board represented as

a 3D object in Fusion. During the whole design process you can push the

EAGLE Layout into Fusion or pull it from there into EAGLE. See page 167

for details.

Managed Libraries

V8.3.0 – 3D Packages support: All packages in Managed Libraries will be

assigned simple 3D boxes by default. These can be replaced with 3D STEP

file models using a web-based editor. References to these 3D packages are

retained by components added to schematics and boards and can be updated

using the UPDATE command.

Added support for user creation and editing of Managed Libraries (private-

only for now).

Board Contour Detection

V8.3.0 – Added detection of board shape based on information in layer 20

(Dimension) and layer 46 (Milling). If a single, non-self-intersecting and

closed outline is detected, this will become filled depending on the user's

color profile. Holes will be shown in background color.

Since V8.3.1 it can be switched on or off in the Options/Set/User Interface

menu.

New EAGLE Internal Vector Font

V8.3.0 – EAGLE now uses a new internal vector font which is very similar

to OSIFONT, a common font implementation in the CAD industry. It covers

a bigger set of characters, in particular common Western European, Greek,

Cyrillic, other Eastern European characters and many special symbols. The

new font does not become active unless the option Keep old vector font in

this drawing in Options/User interface is unchecked.

For new designs, the new implementation is taken by default.

ROUTE Command

V8.3.0 – The new Single Layer mode greys out all layers except the one on

which you are routing. Can be enabled/disabled with the command SET

SINGLE_LAYER_MODE On | Off.

1 Introduction

The Avoid Obstacles mode now allows routed wires to connect to same-signal

arbitrary pad shapes.

Managed Libraries

V8.2.0 – Support for easily downloading updates to the built-in libraries and

installing new libraries from our Online Library index. When placing

components from these libraries, the ID and version of the libraries will be

stored in Schematic and Board files.

Design Blocks

V8.2.0 – Now it is possible to edit and create new Design Blocks from the

Control Panel’s tree view.

When a Design Block with a single sheet schematic is pasted into schematic

and board, it is possible to select the location where to be placed by a mouse

click in both editors, schematic and layout.

ROUTE command

V8.2.0 – Improved the ROUTE command's loop handling by making the

removal of a loop interactive when it occurs with a mouse move and not

requiring a mouse click to see the result.

Copy/Paste

V8.1.1 – The shortcuts Ctrl+C and Ctrl+V are now assigned to COPY and

PASTE by default.

Design Rule Check

V8.1.1 – The Airwires branch in the Design Rule Check’s Error window lists

remaining signal wires in the layout. Clicking on an entry in the list invokes a

pointer to the Airwire.

ALIGN command

V8.1.1 – The ALIGN command operates on a set of selected objects and

aligns them in different modes. The following are supported:

Align Top | Bottom | Left | Right edges, align Vertical | Horizontal centers,

Distribute Vertically | Horizontally and Align Components to Grid. The Align

Components to Grid mode uses the origin of the objects for alignment, all

other modes operate using axis aligned bounding boxes of objects to be

aligned.

ROUTE command

V8.1 – The ROUTE command has the capability to automatically detect

obstacles along the path of the routed wire and contouring around them.

Walkaround Obstacles mode is operational when you are routing using

straight segment wire bend styles, with no mitering!

If you switch from routing mode Walkaround Obstacles to routing mode

Ignore obstacles, you will find the routing behaviour as it was in previous

EAGLE versions.

1.2 Important Changes

The ROUTE command option Loop removal is now set to on by default.

BGA Router

The BGA Router now supports non-square BGA components.

New Installer Routines and Subscription Licenses

V8.0 – EAGLE uses new installer routines for Windows, Linux and Mac

versions. EAGLE offers subscription licenses now. Details can be found on

the Autodesk web sites.

Flexible Board size in Free and Standard Edition

V8.0 – The Free and Standard Edition of EAGLE are no longer limited to a

fixed board size, but to the area of 80 cm² for Free and 160 cm² for

Standard.

Reworked Icons

V8.0 – The command and action icons which were introduces in EAGLE V7

are reworked for better visibility and recognition.

This first edition of the V8 manual does not yet show all icons in the

new V8 style. This will be updated as soon as possible.

Pin Snapping in the Schematic

V8.0 – When drawing a net in the Schematic Editor, the net always jumps to

the pin connection point which is located on one end of the pin and can be

made visible if displaying layer 93, Pins.

Renamed WIRE Command to LINE

V8.0 – The WIRE command has been renamed to LINE. For compatibility

reasons WIRE is still allowed.

New SLICE command

V8.0 – The SLICE command is used to cut nets and board traces in two with

a gap specified by the current line width. Schematic wires that are sliced

become separate nets, similar to deleting a middle wire segment. Board

traces that are sliced maintain net connectivity with the new trace gap

containing an airwire (similar to ripup command).

ROUTE Command Improvements

Route Start Selection

V8.0 – The process of picking the object to start routing has changed so that

the result is more predictable and flexible. Now, you can start routing from

any copper object (pad, via, wire), in addition to airwires, without needed to

press the Ctrl key.

1 Introduction

When the left mouse button is pressed to start a route, a specific search order

is used to find the route start object. That search order is:

•Through-hole pads and SMDs/vias defined on current route layer

•Wires on current route layer

•Airwires

•SMDs and vias, not defined on current-layer

•Wires not defined on current layer

For example, picking a Top SMD with the current route layer as Top is

straightforward when many airwires cross over the SMD because of this

search order. Conversely, if the current route layer is Bottom, for example,

airwires and other current layer wires would have precedent over this Top

SMD when the objects are co-located.

Undo Mouse Clicks

V8.0 – Now while routing if you make a mistake with a mouse click (or you

find a better route path) and want to change it, you can press the backspace

<BS> key (DEL on Macs) to "undo" the prior mouse click. You can "Undo"

the prior mouse clicks all the way back to the route start object. When

undoing through via placements, the layer will automatically switch to the

prior routing layer.

If something is typed into the command line, the <BS> key will erase

the last typed character in the command line, as normal. In this case,

the <BS> key will have no effect on the route command. The

command line needs to be empty of characters before the <BS> key

works on the ROUTE command.

Electrical Snap Indicator

V8.0 – The ROUTE command has always had the snapping to nearby

electrical objects, but now an indicator (X) is displayed when a snap occurs to

the nearby electrical object's center point. As in the past, the Snap Length

parameter controls how close you can get to a nearby electrical object before

the mouse is snapped to it's center point.

Loop Remove

V8.0 – The Loop Remove feature, which defaults to off, allows you to re-

route any portion of a path between two pads and automatically remove the

redundant (loop) wires and possibly via.

The re-route can start at a pad, in the middle of a wire, or a via, and end in

the same fashion – on a pad, in the middle of a wire, or a via. The Loop

Remove will not work if the loop to remove goes through a pad or if a T

connection exists – for the loop to be removed it has to go between two pads

(or sub-section of those pads) and no have T connections in that path.

1.2 Important Changes

Via Placement and Change of Routing Layers

V8.0 – When a layer change is requested, the via is now immediately placed

at the end of the route and can be dragged around before committing it by

left-clicking.

A new keyboard shortcut has been added to change routing layers. The Space

key changes the routing layer to the next routing layer. The next routing layer

is displayed in the status line as Next Layer: Bottom for example.

You can continue to press the Space to cycle forward through the available

routing layers. If you cycle back to the current routing layer, the via at the

end of the route disappears. Pressing Shift + Space works in a similar

manner, but cycles backwards through the routing layers.

The condition holds here as with "Undo Mouse Clicks": the command

line must be empty for the Space key to work with the route

command.

To place a via and continue routing on the same (current) routing layer, press

Shift+Left button click.

If the route start object, or the object at the last mouse click, is a through-

hole pad or via, then you can press Shift + middle button click to change the

routing layer without adding a via. This could be useful, for example, if you

started routing from a through-hole pad on the top layer, but then decide it

may be better to route from this pad on the Bottom layer.

BGA Autorouter

V8.0 – The BGA router is a special kind of Autorouter which is designed to

route the connections out of Ball Grid Array (BGA) with a minimal number of

layers. The BGA router allows to route selected or all signals and supports

micro vias, if enabled. It is started with the BGA icon or with AUTO BGA in

the command line. After BGA routing you can continue with manual or

automated routing.

Design Blocks

V8.0 – A Design Block is technically spoken a combination of a Schematic

and a (consistent) Board. It is intended to represent a kind of designed

module which can be easily reused in EAGLE.

It’s possible to select objects in schematic and board which are consistent

and save them as a Design Block. The Design Block can be given a

Description and can have attributes. Once saved it can be re-used at any time

in a project.

1 Introduction

1.3 General Comments About EAGLE

Component Libraries

The component libraries supplied with EAGLE have been compiled with

great care as an additional service to you, our customer. However, the large

number of available components and suppliers of these components means

that the occasional discrepancy is unavoidable. Please note, therefore, that

Autodesk takes no responsibility for the complete accuracy of information

included in library files.

Please note that libraries are not necessarily identical to former libraries with

the same name. Therefore, it is advisable to back up your old libraries before

installing the new ones.

1.4 Technical Terms

In this manual, in the help function, and in EAGLE itself we frequently use

some technical terms that should be explained here in a few words.

Airwire:

Unrouted connection on a board, displayed in the unrouted layer (= rubber

band).

BGA:

Ball Grid Array – a surface mount device with round soldering pads beneath

the case.

Blind Via:

A plated-through hole for changing the layer of a track which has not been

drilled through all layers in the production process of a multilayer board.

Buried Via:

A plated-trough hole, which has been drilled through the current layer stack

in the production process like a normal (through) via, but does not connect

all layers of the whole board.

Core:

Two copper layers applied to a solid substrate.

Design Rule Check (DRC):

EAGLE can identify the violation of certain Design Rules (e.g. if two different

tracks overlap or are too close) with the DRC.

Device:

A fully defined element in a library. Consists of at least one Package and one

Symbol.

Device Set:

Consists of Devices that use the same Symbols for the Schematic but have

different Package variants or technologies.

Drill:

Plated-through drilling in the layout (in pads and vias)

Electrical Rule Check (ERC):

EAGLE can identify the violation of certain electrical rules (e.g. if two outputs

are connected) with the ERC. It also checks the consistency of the schematic

and the layout.

1.4 Technical Terms

Follow-me Router:

The manual ROUTE command offers an operating mode that calculates and

displays the connection of a selected signal automatically. The current

position of the mouse cursor determines the trace of the connection. Only

available with the Autorouter module.

Forward&Back Annotation:

Transforms all the actions one makes in a schematic online into the layout

(and with limitations from layout into schematic). Both files are consistent all

the time.

Gate:

The term Gate is used in this manual for a part of a component which can be

individually placed on a schematic. This can be one Gate of a TTL

component, one contact pair in a relay, or an individual resistor from a

resistor array.

Hole:

Non plated-through drilling in the layout (e.g. a mounting hole).

Layer Stack:

Current number and order of copper and isolation layers which are used to

build up a printed circuit board.

Micro via:

A plated-through hole (like Blind via) with a relatively small drill diameter

which connects an outer layer with the next reachable inner layer.

Module:

A subunit of the hierarchical schematic that contains a smaller part of the

schematic

Module instance:

A simple symbol in a superior level in the hierarchical schematic that

represents the usage of a module.

Net:

Electrical connection in a schematic.

Obstacle Avoidance:

A manual routing mode that takes care on Design Rule settings. In this mode

you can be sure that all Design Rules and Net Class settings will be taken into

consideration.

Package:

Component footprint stored in a library.

Pad:

Through-hole pad associated with a Package.

Pin:

Connection point on a Schematic Symbol.

Port:

Similar to a pin, the port connects module instances in the hierarchical

diagram with nets.

Prepreg:

Used in a compound of inner and outer layers for multilayer boards.

1 Introduction

Rack:

Configuration table for a drilling machine. Needed for generating drill data.

Ratsnest:

Command for calculating the shortest airwires and for hiding or displaying

certain airwires for a better overview.

Restring:

Pronunciation: rest-ring. Setting that determines the width of the copper

ring around a plated-through hole of a pad or via.

Signal:

Electrical connection in a board.

Supply Symbol:

Represents a supply signal in the schematic. Causes the ERC to run special

checks.

Symbol:

Schematic representation of a component, stored in a Library.

User Language:

Freely programmable, C-like language for data import and export.

Via:

Plated-through hole for changing the layer of a track. See also Micro via,

Blind via, and Buried via.

Wheel:

Aperture configuration file. Generated with Gerber data for board

manufacturing.

Wire:

Electrical connection in a board, or a line (since lines are drawn with the

LINE command).

Chapter 2

Installation

2.1 System Requirements

Detailed system requirement are mentioned on the Autodesk EAGLE product

website. EAGLE is available in 64bit versions only. Choose the appropriate

installation package according the architecture of your operating system. In

order to run EAGLE the following is required:

a minimum of 3 MB of memory,

about 700 MB free disk space,

a minimum graphics resolution of 1024 x 768 pixels,

preferably a 3-button wheel mouse.

2.2 Installation of the EAGLE package

On the Autodesk product website you will always find the newest installation

files. First download the current EAGLE package according your operating

system from the web site. EAGLE is available for Windows, Linux and Mac

OS-X in 64bit packages.

http://www.autodesk.com/products/EAGLE/Overview

For the Windows and Mac installation simply double-click the downloaded

archive. Then follow the setup routine. The Linux package has to extracted

into a folder of your choice.

2.3 Updating an Older Version

First Back up, Then Install

For reasons of safety it is good practice to create a backup of your previous

data before proceeding!

After starting EAGLE for the first time, please check the path settings in the

Control Panel's Options/Directories.. menu.

The path settings are taken from the EAGLE configuration file eaglerc(.usr),

if existing, from a previous EAGLE version installed. Modify the settings if

necessary. The variable $EAGLEDIR stands for the current EAGLE

installation directory.

2 Installation

Please read the file update.txt in the EAGLE/doc directory, in order to

familiarize yourself with the changes in the new version of the program.

Notes on Library Files

All files from previous versions can be used with the new EAGLE version.

Please check which library files are in use, and available for the ADD

command. To make sure that you are working with those of the new EAGLE

version you should, for example in the Schematic Editor, type the following

command in the command line



This removes all libraries from the buffer. Then type



to load all libraries of the currently given directory or other directories.

The information about libraries in use is stored in the eagle.epf file of the

currently active project.

If you have added new Devices to existing libraries, you should re-name and

copy these libraries to a separate folder to avoid over writing, muddling up

files with newer or older ones, and in the worst case loosing your work prior

to updating. This same rule holds true for ULPs and Script files as well.

In Case of Changes in the File Data Structure

In case of an update where it was necessary to change the file data structure,

it may be wise to save your own library files from the earlier version in the

new EAGLE. Expanding the tree view's library preview or showing all

libraries by the first ADD command cause additional time in screen update

viewing, depending on your computer speed. EAGLE has to update the files

temporarily to the new file format before showing the libraries' contents.

In case you have a lot of files, there is a quick and comfortable way to solve

this issue. You need two tools to achieve this:

The User Language Program run-loop-all-lbr-script.ulp and a Script file that

contains one line:



Edit one of the library files that shall be updated and start the ULP. You will

be asked for the Script file to be executed, then all libraries which are in the

same directory will be updated.

The data structure of the library files remains unchanged in the

transition from version 7 to version 8.0!

2.4 First Start of EAGLE

If you start EAGLE you are asked to sign in into your personal Autodesk

account. The account is assigned with your email address you registered and

ordered your EAGLE subscription. After logging in, EAGLE will start

according the entitlement (Standard or Premium Edition, expiration date of

subscription) you are eligible for.

2.4 First Start of EAGLE

You do not necessarily need an internet connection for working with EAGLE.

It’s also possible to work in OFFLINE mode for 14 days. After this period you

are asked to sign in again in order to check the validity of the entitlement. If

you do not have internet access, EAGLE will fall back into free mode until

you can log in again.

The free Edition asks for a login only once at the first start. From then on,

you don’t have to connect to the internet anymore.

2.5 Language Settings

EAGLE decides due to the operating systems' language which language to

use. If the systems' language, for example, is set to German, EAGLE will use

German language. In case you don't like the automatically selected language,

you have the following possibilities to change it.

Windows

EAGLE takes care on a variable named LANG. For changing it go to the

Windows Control Panel where you can define environment variables. Set up

a variable named LANG. For english language the value is typically set to

en_US or en_GB. For german language the value should be set to de_DE,

de_CH, or de_AT. In case you would like to use a batch file to start EAGLE, it

could look like this:



 !"!#$%$%

"&&!$%

This is of use, if there are other applications that react on the LANG variable.

The batch affects EAGLE only.

Linux and Mac OS X

The same as described for the Windows EAGLE can be done for Linux and

Mac OS-X. There you have to define the variable with the systems' EXPORT

command.

You could also use a script file in order to start EAGLE:



'(')"'!#$%$%'!

2 Installation

This

page

has been

left free

intentionally.

Chapter 3

EAGLE Modules and Editions

3.1 EAGLE Modules

The Layout Editor

The Layout Editor, which allows you to design Printed Circuit Boards (PCBs)

comes with the Library Editor, the Computer Aided Manufacturing (CAM)

Processor, and the Text Editor. With the Library Editor you can already

design Packages (footprints), Symbols and Devices (for a schematic). The

CAM Processor is the program which generates the output data for the

production of the PCB (e.g. Gerber or drill files). It is also possible to use

User Language programs and Script files.

Schematic Editor

If you want to draw Schematic diagrams for electronic systems you should

have Schematic and Layout Editor. You can generate the associated circuit

board at any time with a mouse-click. EAGLE then changes to the Layout

Editor, where the packages are placed next to an empty board – connected

via airwires (rubber bands). From here you can go on designing with the

Layout Editor as usual. Schematic and layout are automatically kept

consistent by EAGLE (Forward&Back Annotation). Schematic diagrams can

consist of a maximum of 999 sheets in the Professional Edition (99 sheets in

the Standard Edition). On the left side of the Schematic Editor window the

preview of the sheets is displayed.

The Schematic Editor is also applicable for drawing simple electrical wiring

diagrams (connection scheme, contact plans...).

Autorouter

You can have airwires routed automatically if EAGLE has the Autorouter

module. You can choose single nets, groups of nets or all nets for the

automatic routing pass. The program will handle various network classes

having different track widths and minimum clearances.

The Autorouter also serves as basic engine of the Follow-me router. This is

an advanced operating mode of the ROUTE command for manual routing,

which calculates and displays the trace of a selected signal automatically.

The Autorouter has a special function to route BGA connections (AUTO

BGA).

3 EAGLE Modules and Editions

3.2 Different Editions

EAGLE offers various performance/price categories (editions) called Free

Standard, and Premium. The facilities mentioned in this manual always refer

to the Professional edition.

Premium Edition

General

maximum drawing area 150 x 150 inches

resolution 0.003125 µm

mm or inch grid

up to 255 drawing layers

command (Script) files

C-like User Language for data export and import and the

realization of self-defined commands

Fully documented, readable XML data structure

easy library editing

composition of self-defined libraries with already existing

elements by Drag&Drop

easy generation of new Package variants from other libraries by

Drag&Drop

free rotation of package variants (0.1-degree steps)

arbitrary pad shapes in the Package Editor

library browser and powerful component search function

technology support (e. g. 74L00, 74LS00..)

easy definition of labelled drawing frames

free definable attributes, applicable for Devices in the Library

and in Schematic or Layout

support of assembly variants

easy-to-use dimensioning tool

merging of different projects with maintaining consistency

(Design Reuse)

Design Blocks as Schematic and Layout

Save Schematic and Board (or parts of them) in a common Design

Block for design re-use in other projects

Design Blocks as templates for Schematic and Layouts

integrated PDF data export function

export function for graphic files (BMP, TIF, PNG...)

printouts via the OS's printer drivers with print preview

partlist generation with database support (bom.ulp)

Drag&Drop in the Control Panel

3.2 Different Editions

user-definable context menu with object-specific commands for all

objects, available through a right mouse click

properties of objects can be accessed and edited via context menu

automatic backup function

Schematic Editor

Schematics can be designed in a hierarchical structure: modules are

represented by module instances and connected through ports in the

top level of the schematic.

the hierarchy can reach any depth

up to 999 sheets per schematic

icon preview for schematic and module sheets

sorting sheets of modules and schematic with Drag&Drop

cross references for nets

automatic generation of contact cross references

simple copying of parts

replace function for parts without loss of consistency between

schematic and layout

Online-Forward&Back Annotation between schematic and board

automatic board generation

automatic generation of supply signals

Electrical Rule Check (error check in the Schematic and consistency

check between Schematic and Layout)

Layout Editor

full SMD support

support of Blind and Buried vias

rotation of objects in arbitrary angles (0.1-degree steps)

components can be locked against moving

texts can be placed in any orientation

dynamic calculation of signal lines while routing the layout

magnetic-pads function

tracks can be layed out with rounded corners in any radius

mitering to smooth wire joints

Loop remove function for re-routing any portion of a path between

two pads with automatic removal of the previous redundant trace

Design Rule Check for board layouts (checks e.g. overlaps,

measures of pads or tracks)

copper pouring (ground plains)

Package variants support

Differential Pair routing

automatic creation of meanders for length compensation of signals

3 EAGLE Modules and Editions

user-definable, free programmable User Language to generate data

for mounting machines, test equipments, milling machines or any

other data format

output of manufacturing data for pen plotters, photo plotters and

drilling machines with the CAM Processor

Creation of 3D data (e.g. STEP or STL) for mechanical CAD systems

via a web service

Autorouter Module

fully integrated into basic program

TopRouter with gridless routing algorithm, which can be preceded by

the Autorouter

optional automatic selection of routing grid and preferred directions

in the signal layers

Special BGA Autorouter BGA escape routing

support for multi-core processors to process multiple routing jobs

simultaneously

uses the set of Design Rules you defined for the layout

change between manual and automatic routing at any time

basic engine for the Follow-me router, a tool that supports

you in manual routing; the trace of a selected signal will be

calculated automatically

ripup&retry algorithm

user-definable strategy (by cost factors)

routing grid down to 0.8 mil (0.02 mm)

no placement restrictions

up to 16 signal layers (with user definable preferred directions)

full support of Blind and Buried vias

takes into consideration various net classes

Standard Edition

Compared to the Premium Edition the following restrictions apply to the

Standard Edition:

The layout area is restricted to 16000 mm². The board dimensions

are flexible. A typical size could be 160 x 100 mm (about 6.3 x 3.9

inches). Outside this area it is not possible to place Packages and draw

signals.

A maximum number of 4 signal layers is allowed.

A schematic can consist of a maximum of 99 sheets.

Free Edition

The following restrictions apply to the Standard (former Light) Edition:

3.2 Different Editions

The board area is flexible and restricted to 8000 mm². Typical board

size can be 80mm x 100mm (about 3.9 x 3.2 inches). Outside this area

it is not possible to place Packages and draw signals.

Only two signal layers can be used (no inner layers).

A schematic can consist of two sheets.

Larger layouts and schematics can be printed with the smaller editions. The

CAM processor can generate manufacturing data as well.

3 EAGLE Modules and Editions

This

page

has been

left free

intentionally.

Chapter 4

A First Look at EAGLE

4.1 The Control Panel

The Control Panel normally appears after starting EAGLE, and this is the

program's control center. All the files specific to EAGLE are managed here,

and some basic settings can be made. It is similar to the familiar file

managers used by a wide variety of applications and operating systems. Each

EAGLE file is displayed in the tree view by means of a small symbol.

A context menu is opened by clicking with the mouse on an entry in the tree

view. This allows you, depending on the object, to carry out a variety of

actions, like rename, copy, print, open, create new etc. Graphics or PDF files,

for example, will be opened with the default application.

The Control Panel supports Drag&Drop. This can also be done between

different programs. You can, for instance, copy files, move them, or create

links on the desktop. User Language programs or script files that are pulled

with the aid of the mouse out of the Control Panel and into an editor window

are started automatically. If, for instance, you pull a board file with the

mouse into the Layout Editor, the file is opened.

The tree structure provides a quick overview of the Libraries, Design Blocks,

Documentation, Design Rules, User Language programs, script files, CAM

jobs and projects. Special libraries, text, manufacturing and documentation

files can belong to a project as well as schematic diagrams and layouts.

The first time it is called, the Control Panel will appear very much as shown

in the following diagram. If an object is selected in the tree view, further

relevant information or a preview is displayed in the right hand part of the

window.

Simply click onto various folders and files in order to experiment with the

Control Panel's facilities.

4 A First Look at EAGLE

On the top right corner the current ONLINE/OFFLINE status is shown. The

following image shows that EAGLE is currently OFFLINE. On the right, click

onto the user name and select one of the options there. Here you can Go

online again, let display the License information and Sign out from your

account.

Documentation

The Documentation branch allows direct access to the EAGLE tutorial and

manual available in different languages. Additionally, there can be found the

UPDATE.txt file and documentation files of some of the User Language

programs. Double-click opens the file with the default PDF reader or text

editor.

Libraries Summary

The possibility of displaying the contents of the libraries is particularly

interesting. It provides a very rapid overview of the available Devices.

➢

Control Panel: On the right, the preview of a Design Block

➢

Control Panel: License/Status Information

4.1 The Control Panel

Expand the Libraries entry, and you can see the available libraries. We

distinguish between Managed Libraries and “normal” libraries. Managed

libraries come with the EAGLE installation and are kept up-to-date and in

sync with our online EAGLE Managed Libraries repository. If there are

newer versions of Managed Libraries available, you can decide to download

and use them.

Besides the Managed Libraries folder you see a lbr folder which is supposed

to be the folder for all of your own and self-made libraries.

In the Description field you can see a brief description of the contents. If a

library is selected, you will see more extensive information about the library

in the right hand part of the Control Panel. If you then expand a library

entry, the contents will be displayed together with a short description of each

element. Devices and Packages are marked with a small icon.

Now select, for example, a Device:

The description of the Device and a graphical representation of it appear on

the right. The available Package and technology variants are listed. If you

click onto one of the Package versions, the Package preview shown above will

change.

If a Schematic Editor window is open, the entry ADD will be shown right of

the variant name. Click it and the Device is attached to the mouse cursor as

soon as it is over the Schematic Editor window. Now you can drop it in the

schematic.

If you are only working with the Layout Editor, this will of course also

operate with Packages. It is, additionally, possible to drag a Device from the

tree view into a schematic diagram and to place it there by means of

Drag&Drop. If it has more than one Package version, the ADD dialog opens

automatically, so that the desired Package can be selected.

The green marker behind the library entry indicates that this library is in use.

This means that it can be used in the current project. Devices in this library

will be examined by the search function in the ADD dialog of the schematic

diagram or of the layout. This makes them available for the project. The

library will not be examined if the marking is gray.

If starting EAGLE without a project (no eagle.epf file is read, the project has

been closed before exiting EAGLE last time) and creating a new project

(⇒ File/New/Project) all libraries will be in use automatically. However,

opening an already existing project, where only certain libraries are in use

before creating the new project, will adopt this selection.

4 A First Look at EAGLE

If the Library Editor window is open, you can Drag&Drop a complete Device

set or Package definition from the Control Panel into the library window.

This way you can copy it from one library into another. If the target library

already contains an element with the same name, it will be updated

automatically.

Design Blocks

Design Blocks (dbl) ideally contain a consistent Schematic and Layout pair

that can be easily (re-)used in any project. Design Blocks can have a

Description and Attributes for getting information about the intent of the

Design Block.

A right mouse click onto a Design Block entry opens a context menu that

allows to Open, Rename, Copy, Delete a Design Block or directly Add it to a

Schematic.

Design Rules

Special Design Rules can be specified in EAGLE to govern the board design.

These can be saved as data sets in special files (*.dru).

The parameter set that is to govern the current project is specified in the

Design Rules branch of the tree view. If no data has been provided for the

Design Rules (DRC command), EAGLE will itself provide parameters. The

marking to the right of the file entry specifies the default parameter set for

the current project. The layout will be checked by the DRC in accordance

with these criteria. Further information about the DRC and the Design Rules

is found starting on page 144.

➢

Control Panel: Library summary with Device view

4.1 The Control Panel

User Language Programs, Scripts, CAM Jobs

These entries show the contents of the ulp, scr and cam directories. They

contain various User Language programs (*.ulp), script files (*.scr) and CAM

jobs (*.cam) for the output of data using the CAM Processor. If one of these

files is selected in the Control Panel, you will see a full description of the file.

The paths can be set by means of the Options/Directories menu. This is

discussed in more detail later in this chapter.

Projects

The various projects are managed from the Control Panel. A click onto the

Projects entry displays various folders. These are located under the path set

under Options/Directories/Projects. It is allowed to define more than one

path there.

A project usually consists of a folder which represents the project by its name

and the project's configuration file eagle.epf. The folder usually contains all

files that belong to your project, for example, schematic and board file,

special library files, script files and so on.

Project directories that contain the project file eagle.epf will be marked with

a special folder icon .

The project to be edited is selected in the Projects branch. On the right of the

project's name you will find a marker which is either gray or green. With the

help of this marker one can open or close projects. Clicking onto a gray

marker, loads the project. The marker appears green now. Clicking onto the

green marker again or clicking onto another gray marker closes the current

project respectively opens another project after closing the current one. This

way one can switch easily from one project to another.

As an alternative you can open or close a project by double-clicking onto the

entry in the tree view or by pressing the Space or Enter key.

While closing a project the settings of the currently opened Editor windows

will be stored in the corresponding project file eagle.epf, provided that the

option Automatically save project file is set in the Options/Backup menu.

If the project file was generated by another EAGLE version than currently

used, you will be asked, if it is allowed to overwrite the file.

New projects are created by clicking the right mouse button onto a folder

entry in this branch. A context menu opens which permits new files and

directories to be created and the individual projects to be managed.

Selecting the option New/Project invokes a new folder which has to be given

the project's title. The project file eagle.epf will be created automatically.

You can also use the File/Open/Project or the File/New/Project menu to

open or create a new project.

The context menu contains the Edit Description item. A description of the

project can be entered here, and this is then displayed in the Description box.

4 A First Look at EAGLE

It is possible to create a description for schematic and board files. It has to be

defined in the editor windows. See help function for the DESCRIPTION

command for more information.

Menu Bar

The Control Panel allows various actions to be executed and settings made

through pull-down menus that are explained below.

File Menu

The File menu contains the following items:

New

Creates a new Layout (board), Schematic, Design Block, Library, CAM job,

ULP, script or text file. The Project option creates a new project. This initially

consists simply of a new directory in which the files for a new project are

handled. These will consist as a rule of the schematic diagram and layout,

possibly of special libraries, script files, User Language programs,

documentation files etc. and of the file eagle.epf, in which project-specific

settings are stored.

The default directories for the various file types are defined in the

Options/Directories menu.

CAM jobs are definitions for generating output data with the CAM Processor.

Script and ULP files are text files containing command sequences in the

EAGLE command language or the EAGLE User Language. They can be

created and edited with the EAGLE Text Editor or with an external text

editor.

➢

Context menu for project management

4.1 The Control Panel

Open

Opens an existing file of the types mentioned above.

Open recent projects

Lists recently used projects.

Save all

All changed files are saved. The current settings for the project are saved in

the file eagle.epf, even if the option Automatically save project file in the

menu Options/Backup... is switched off. User-specific settings are stored in

the file eaglerc.usr (Windows) or .eaglerc (Linux/Mac).

Close project

The project will be closed. Project-specific settings are saved in the

eagle.epf file of the current project directory.

Once you have overwritten a project file from an older version (before 6.0)

the dimension values will be stored in a different format. If you then load

such a file with an old version of EAGLE, all menu entries (like wire widths or

drill diameters) will fall back to their default values.

License information

Shows the entitlements of your license.

Sign out

Here you can sign out from your Autodesk account. Now another user could

EAGLE again, you will be asked for your EAGLE/Autodesk login data.

Exit

The program is terminated. When EAGLE is started again, the last program

status is restored, i.e. the windows and other working environment

parameters appear unchanged. If there was no project loaded only the

Control Panel will be opened next time.

The current status is also saved when you leave EAGLE with Alt-X from any

program part.

If you have deactivated the Pull-down menu of the Editor windows

with the Options/User interface menu, Alt+X won't work. Use the

QUIT command instead. You could even assign the QUIT command

to Alt+X with the help of the ASSIGN command.

View Menu

Extended mode

The Documentation and the Project branch of the tree view show all files by

default. Image and other binary files can be opened directly with the

appropriate default application. If this mode is switched off, only EAGLE

related files will be shown.

4 A First Look at EAGLE

Refresh

The contents of the tree view are updated.

Search in tree

The tree view of the Control Panel is searchable. This menu entry invokes a

Search line which is located above the Control Panel's status bar. The search

function looks exactly for the given search pattern. If you are using more

search patterns, all of them must occur in order to get a match.

The search function has access to all objects that can be displayed in the tree

view, like file names, Device and Package names in libraries, and for example

the short description shown in the Descritpion column. In order to make the

search more flexbile wildcards are allowed. ? stands for any character, * for

any number of any character.

In case you want to search for a name that contains a *, you have to escape it

with a backslash: 40\*14, for example, searches for 40*14.

Sort

The contents of the tree view will be sorted by name or by type.

Options Menu

Directories

The default directories for particular EAGLE files are entered in the

directories dialog box.

More than one path may be entered for each of these. In the Windows

version the entries are separated by semicolons, while a colon is used in the

Linux and Mac version. The Projects directory is also the default directory for

the Text Editor.

The Projects directory contains subdirectories, each of which represents a

particular project. Each of the project directories contains an EAGLE project

file (eagle.epf). A project directory and its subdirectories usually contain all

the files that are associated with one particular project, such as the schematic

diagram and the layout, text files, manufacturing data, documentation files

and so on.

Type the path directly into the corresponding box, or select the desired

directory by clicking the Browse button.

➢

The directories dialog in the Options menu

4.1 The Control Panel

The default settings can be seen in the diagram above. $EAGLEDIR stands

for the installation's EAGLE directory.

You may also use $HOME for your home directory under Linux. Under

Windows it is possible to define this environment variable in the Windows

Control Panel, System settings. If a HOME variable has not been set within

the Environment variable, then under Windows EAGLE will suggest the

directory Application Data.

This directory is defined in the Windows registry in:

HKEY_CURRENT_USER\Software\Microsoft\Windows\CurrentVers

ion\Explorer\Shell Folders\AppData

In this folder you can also find the user-specific configuration file

eaglerc.usr. Under Windows 7/8/10 this is typically

C:\Users\your_account_name\AppData\Roaming\CadSoft\EAGLE

It is of course also possible to specify paths with an absolute format.

The HOME variable must not point to the root directory of a drive!

Backup/Locking

When files are saved, EAGLE creates backup copies of the previous files. The

maximum backup level field allows you to enter the maximum number of

backup copies (default: 9). Backup files have different file extensions,

enumerated sequentially. Schematic files receive the ending s#x, board files

b#x, and library files l#x. x can run from 1 to 9. The file with x = 1 is the

newest one.

The automatic backup function also permits the backup to be scheduled. The

time-interval can be between 1 and 60 minutes (default: 5 minutes). The

backup files have the endings b##, s## and l## respectively.

All these backup files can be further processed in EAGLE if they are renamed

and given the usual file endings (brd, sch, lbr).

If the option to Automatically save project file is chosen, your project is

automatically saved when you close the current project or leave the program.

Enable file locking is set off by default. For each file edited in one of the

EAGLE editor windows, EAGLE creates a lock file name.lck. If another

EAGLE user tries to open one of the already locked files, a dialog window

that offers various options pops up.

➢

Backup dialog

4 A First Look at EAGLE

User Interface

The User Interface dialog allows the appearance of the editor windows for

the layout, schematic diagram and library to be adjusted to your preferences.

You can also access this menu from the Editor windows.

In the Controls box you specify which objects are to be displayed in the editor

window. If you deactivate all the Controls, only the command line will

remain for entry. This maximizes the free area available for the drawing.

The option Always vector font shows and prints texts with the built-in vector

font, independently from the originally used font. Using the Vector font

guarantees that the output with a printer or the CAM Processor is exactly the

same as shown in the editor window. Fonts other than vector font depend on

the systems' settings and cannot be controlled by EAGLE. The output of non-

vector fonts may differ from the editor's view.

Opening the User Interface dialog from one of the Editor windows (for

example, the Layout Editor) the Always vector font option offers an

additional item Persistent in this drawing. Setting this option causes EAGLE

to save the Always vector font setting in the current drawing file. So you can

be quite sure that the layout will be shown with vector font at another's

person computer (for example, at a board house).

Please see the help function for details (TEXT command).

Since EAGLE 8.3.0 EAGLE comes with a new internal vector font. It is very

similar to OSIFONT which is commonly used in the CAD world. In order to

maintain all your projects with previous versions, the option Keep legacy

vector font in this drawing is selected with each project. In case you create a

new project EAGLE will automatically use the new vector font.

➢

Settings for the User Interface

4.1 The Control Panel

Limit zoom factor limits the maximum zoom factor in an editor window. At

maximum zoom level the width of the drawing is about one Millimetre

(approx. 40 mil). Switching off this option allows you to zoom until the

0.003125 Micron grid will become visible.

If you are working with a wheel mouse, you can zoom in and out by turning

the mouse wheel. Mouse wheel zoom determines the zoom factor. The value

0 switches this function off. The wheel is used for scrolling then.

EAGLE also supports the use of two-finger-pan gestures on track pads for

navigating and zooming. If you activate the Legacy mouse wheel mode

option, the gestures are no longer supported.

The field External text editor allows you to specify an alternative for the

built-in EAGLE text editor. Further details on this can be found in the help

function in the section Editor windows/Text editor.

The background color and the appearance of the drawing cursor can be

separately adjusted for the layout and the schematic diagram editors. The

background may be black, white or shown in any other color (Colored). The

background color definition is described on page 107.

The cursor can be displayed optionally as small cross or as large cross-hairs.

The section Vertical text lets you decide whether text should be readable

from the right hand side upwards (Up) or from the left hand side downwards

(Down) in your drawings.

Icon size can be used for scaling the icons. The value is in pixels.

Selecting the User guidance check box displays additional information about

the selected object, like the net or signal name, the net class, or the part's

name and value (with NET, MOVE, ROUTE, SHOW...), instructions about

the possible mouse actions in the status bar of the editor window.

Window Positions

Here you can store the positions and the sizes of the currently open Editor

windows. Each file that will be opened from now on appears in its Editor

window at the given position and size parameters that were stored.

If you delete the stored positions again, EAGLE determines the location of an

Editor window and uses a fixed size for it, which is the default setting.

Window Menu

From the Window menu you can choose the window (schematic, board, etc.)

to be displayed in the foreground. The number on the left is the window

number. It allows you to choose a window when combined with the Alt key

(e.g. Alt+1 selects window 1).

The combination Alt+0 can be used anywhere in the program to bring the

Control Panel into the foreground.

The functionality of Alt+window_number is supported in the

Windows and in the Linux version only.

4 A First Look at EAGLE

Help Menu

The Help menu contains an item for calling the help function.

4.2 The Schematic Editor Window

The Schematic Editor window opens when you load an existing schematic or

create a new one. There are several ways of opening files in EAGLE.

You can, for instance, load a schematic diagram by means of the

File/Open/Schematic menu in the Control Panel. Alternatively double-click

onto a schematic diagram file in the tree view.

If you want to create a new schematic, select the menu File/New/Schematic.

This will open a schematic with the name untitled.sch in the current project

directory.

➢

The Schematic Editor

If you want to create a schematic diagram straight away in a new project, you

may for example click with the right mouse button onto a project in the

Projects entry of the tree view, and select the New project option from the

context menu. The new project receives a name. Then click onto this entry

with the right mouse button. Now select New/Schematic from the context

menu.

A new schematic opens in this project directory.

On top you will see the title bar, which contains the file name, and then the

menu bar, and the action toolbar.

Below the action toolbar there is the parameter toolbar, which contains

different icons, depending on the active command.

4.2 The Schematic Editor Window

Above the working area you will find the coordinate display on the left,

with the command line, where commands can be entered in text format, to

the right of it.

EAGLE accepts commands in different but equivalent ways: as mouse clicks,

text via keyboard, or from command (script) files.

On the left of the work space you find the command toolbar, which

contains most of the Schematic Editor's commands.

In the status line, at the bottom of the screen, instructions for the user

appear, if a command is active.

On the left you you can see the preview of the schematic sheets. You can sort

the sheets via Drag&Drop.

Each of the toolbars can be displayed or hidden using Options/User

Interface. It is also possible to rearrange the toolbars within certain limits

with the aid of the mouse. The command toolbar, for instance, can also be

placed on the right, or the action and parameter toolbars can be placed

together on one line.

How You Obtain Detailed Information About a

Command

User Guidance

If the mouse cursor remains above an icon for longer than a certain time, the

name of the EAGLE command appears. You also see a short explanation

below in the status line.

For example, move the cursor over the LINE icon. Bubble help with the word

Wire appears directly by the cursor. The short description, Draw lines,

appears in the status line.

If you select the command, a short note appears below in the status line,

indicating what would normally be expected as the next action. For instance,

if you click onto the LINE icon, the status line will display the instruction:

Left-click to start wire .

These functions can be activated or cancelled in the Control Panel by means

of the Options/User Interface menu.

Help Function

If you want to learn more about a command, e.g. the LINE command, click

its icon in the command toolbar, then click the help icon.

As an alternative you can type

*←

in the command line. The ← character symbolizes the Enter key.

The contents of the EAGLE Help is stored in a single HTML file and can be

viewed for example with a web browser, as well. It also offers a full-text

search.

After typing in a search term in the Find line, EAGLE help no longer shows

all pages but only the pages containing this expression. The keys F3 and

Shift+F3 allow you to go to the next or previous location. Each search term

4 A First Look at EAGLE

found will be marked. Green indicating the currently found term, yellow for

all others.

➢

EAGLE Help window

Command Parameters

A number of EAGLE commands need additional parameters. Refer to the

help pages for a description of the textual entry of parameters (via command

line or script file).

Most of the parameters can be entered by clicking the appropriate icons in

the parameter toolbar, which changes according to the selected command.

These icons also show bubble help explanations.

This is how the parameter toolbar appears when the NET command is

activated.

➢

Parameter toolbar of the NET command

On the left is the GRID icon for setting the grid pitch. To the right are

buttons for the bend mode (SET WIRE_BEND) of the net line, followed by

the miter radius for smoothing line joints with the options straight or

rounded (see MITER command). Next to this is the Style menu where the

type of line is defined. On the far right is a value menu for assigning a Net

class.

4.2 The Schematic Editor Window

GRID

This icon is available at any time. It is used to adjust the grid and to select the

current unit. In EAGLE, any value relates to the current unit.

A right-click onto the icon opens a popup menu that contains the entry Last.

So you can switch back to the previously chosen grid setting. The New...

entry allows to define so-called Aliases. More about this in chapter 5.

The Action Toolbar

This toolbar is composed of the following icons:

From the left: Open file, save file, print file, call CAM Processor, open/create

corresponding board file (BOARD command).

Load, remove, or create a new schematic sheet.

USE

Select libraries which will be taken into consideration by the ADD dialog. Can

also be done with the Library/Use menu item or by clicking the markers in

the Libraries branch of the Control Panel's tree view. The context menu of

the entry Libraries or of its subfolders contains the entries Use all and Use

none for a quick and simple selection/deselection of all libraries (of the

folder).

This command has to be used in script files in order to choose the library you

want to take parts from.

SCRIPT

Execute a script file. This enables you to execute any command sequence

with a few mouse clicks.

A right-click onto the icon shows a list of recently executed script files.

RUN

Start a User Language program (ULP).

A right-click onto the icon shows a menu that contains a list of recently used

User Language Programs.

WINDOW

These icons represent different modes of the WINDOW command:

Fit drawing into the screen (WINDOW FIT, Alt-F2), zoom in (F3), zoom out

(F4), redraw screen (WINDOW or F2), select new area.

4 A First Look at EAGLE

To move the current drawing window, click the middle mouse button

and move your mouse!

WINDOW LAST returns to the previous display window.

UNDO/REDO

These commands allow you to cancel previous commands and to execute

commands which have previously been cancelled. If you are working with a

consistent pair of schematic and layout the UNDO/REDO commands now

display in the status bar which command was undone/redone and whether

the command was originally executed in the board or in the schematic editor.

Default function keys: F9 and F10.

Typing UNDO LIST into the command line opens a dialog that contains the

entire contents of the undo buffer. Alternatively you can use the

Edit/Undo/redo list... menu. Here you can undo a certain number of actions

and let them redo again.

The Undo/Redo window shows the list of recent actions. In parenthesis you

find information how long ago this was done. Use the mouse, the up/down

keys or the Undo and Redo buttons in order to place the delimiter. Click Ok

in case you are sure you want to have undone all the actions listed below the

delimiter.

Caution: This is a very powerful tool! By going all the way back in

the UNDO list (which can be done with a single mouse click) and

executing any new command, the undo buffer will be truncated at

that point, and there is no way back! So use this with care!

Stop Icon

Terminates the execution of EAGLE commands (Edit/Stop command).

➢

Undo/redo list

4.2 The Schematic Editor Window

Go Icon

Starts the execution of an active EAGLE command, which allows further

parameters to be entered by the user, like it is with the AUTO or the MARK

command.

The Command Toolbar of The Schematic Editor

INFO

Shows the properties of the selected object. If you know the name of the

object, you can use it as a parameter in the command line. Depending on the

selected object some of the properties can be altered in this dialog.

SHOW

Highlights the object to be selected with the mouse.

It's also possible to enter the object's or Gate's name (even several names at

once) in the command line. You may use the characters * and ? as

wildcards, as well. Ctrl + SHOW toggles the show state of the selected object.

If you are looking for very small objects, it can be useful to use the SHOW

command with the @ option, like in

*+,-.

The location of part C12 will be recognized at once, because the part is

marked with a surrounding frame.

If the searched object is not located on the current sheet, the SHOW window

opens and informs you about the sheet where it is located. In case of objects

that consist of more than one part, like elements with several gates or nets

that spread over several sheets, the window will list several entries. Clicking

on one of the entries center the selected object on the screen. If the searched

object is not found in the whole schematic, the Sheet column will be marked

with a minus sign '-'.

DISPLAY

Select and deselect the layers to be displayed. See the Appendix for the

meaning of the layers

DISPLAY LAST shows the recently used layer combination that was

previously selected for display.

For further details please see help function.

MARK

The following mouse click defines the new origin for the coordinate display.

Relative coordinates (R x-value y-value) and polar values (P radius angle)

are shown in addition to absolute coordinates in the coordinate display box.

4 A First Look at EAGLE

If you first click the MARK icon and then the traffic-light icon, only the

absolute coordinate values will be displayed again.

MOVE

Move any visible object. The right mouse button rotates the object while it is

attached to the mouse cursor.

If you move a net over a pin, no electrical connection will be established. If

you move the pin of a Gate over a net or another pin, an electrical connection

will be created.

To move groups of objects:

Define the group with the GROUP command, click the MOVE icon, press the

Ctrl key, then click into the drawing with the right mouse button, and move it

to the desired location.

If you don't press the Ctrl key, the context menu pops up after clicking with

the right mouse button. It contains an entry Move:Group that allows you to

move the group, too. The right mouse button rotates the group by 90 degrees

while it is attached to the mouse cursor.

If you like to move the group onto another sheet, click the sheet combo box in

the action toolbar or select it from the Sheets preview. Place the group there.

MOVE can be used in the command line with various options. See the help

function for details.

COPY

Copy parts and other objects.

When copying nets and buses the names are retained, but in all other cases a

new name is assigned.

Keep the Ctrl key pressed while clicking onto an object and the object will be

grabbed at its origin. So it will be moved into the currently chosen grid.

COPY can be used with groups. The group will be put into the clipboard of

the operating system. It is possible to copy it into another running EAGLE

program, for example.

MIRROR

Mirror objects.

ROTATE

Rotate objects by 90 degrees (also possible with MOVE).

GROUP

Define a group which can then be moved, rotated, or copied with COPY and

PASTE to another drawing or whose properties are to be changed. After the

icon has been clicked, a rectangular group can be defined by holding down

the left mouse button and dragging the cursor to the diagonal corner of the

4.2 The Schematic Editor Window

rectangle. If you want to define a group by a polygon, use the left mouse

button to determine the corners of the polygon. Then click the right mouse

button to close the polygon.

GROUP ALL in the command line selects all objects on the current sheet, if

the respective layers are displayed.

The following command (ROTATE, CHANGE, MOVE...) has to be applied to

the group with the right mouse button while the key is pressed.

If you like to add further groups to an already existing one, press the Shift

key and define the first corner of the selection area with a mouse click.

In case you want to add an object to or remove it from the group, press the

Ctrl key and click onto the object in question.

Press Ctrl + Shift to toggle the membership of an object and its hierarchically

superior objects: Clicking for example, on a net segment in the Schematic

inverts the group membership of the whole net.

CHANGE

Change the properties of an object, e.g. the width of a line, the Package

variant or the size of text. See help for details.

An object's properties can be checked and even changed, where applicable,

by the Properties entry of the context menu. To access the context menu,

click onto the object with the right mouse button.

PASTE

Insert objects from the paste buffer into the drawing.

It is also possible to paste from a file into schematic and layout directly. To

do so, use the PASTE command with a file name in the command line or use

the menu entry Edit/Paste from...

For further information see help function.

DELETE

Delete visible objects.

Also in combination with GROUP command. If a group has been defined, it

can be deleted with the right mouse button while the Ctrl key is pressed.

The DELETE command deletes an entire part in the Schematic when clicking

onto a Gate with the Shift key pressed. In that case, the tracks connected to

the Package in the board, if already existing, will stay unchanged.

Clicking onto a net or bus wire with the Shift key pressed deletes the entire

net or bus segment.

ADD

Add library elements to the schematic. A search function helps Devices to be

found quickly. USE specifies which libraries are available.

A right-click onto the ADD icon opens a popup menu that lists recently

fetched Devices.

4 A First Look at EAGLE

PASTE DBL

Add a Design Block into the drawing.

PINSWAP

Swap two nets connected to equivalent pins of a Device, provided the pins

have been defined with the same Swaplevel.

A pin that is connected to several pads can't be swapped.

GATESWAP

Swap two equivalent Gates of a Device, provided the Gates have been defined

with the same Swaplevel. In EAGLE terminology, a Gate is a part of a Device

which can be individually placed on a schematic (e.g. one transistor from a

transistor array).

Gates that come with pins connected to several pads, can't be swapped.

REPLACE

Replace a component (Device) with another one from any library. This can

only work if the new component has at least as many pins as the current one

and the pins as well as the pads have identical names or the same positions.

A right-click onto this icon opens a popup menu that shows a list of recently

replaced Devices.

NAME

Give names to components, nets, or buses.

VALUE

Provide values for components. Integrated circuits normally get the type (e.g.

74LS00N) as their value.

A right-click onto this icon opens a list of already used values. Select an entry

and apply it to one or more components by clicking onto them successively.

SMASH

Separate name, value, and, if any, attribute texts from a Device, so that they

can be placed individually. The size of detached (smashed) texts can also be

individually changed. Also in combination with GROUP. If a group is

defined, you can smash it with a right mouse click while the Ctrl key is

pressed.

Use DELETE to hide smashed texts.

Keep the Shift key pressed while using the SMASH command in order to

unsmash text. Text is not editable any more and appears at original

position(s) after a window refresh (also possible in the context menu with

4.2 The Schematic Editor Window

unSmash).

Alternatively you can also switch on or off the option Smashed in the context

menu's Properties entry.

MITER

Round off or bevel wire joints (also possible for nets, buses, polygon

contours). The grade of mitering is determined by the miter radius. Positive

sign results in a rounded joint, negative sign in a bevel.

The miter radius influences some wire bends, too (see help function: SET

command, Wire_Bend).

SPLIT

Insert an angle into a wire or net.

SLICE

Cuts lines in two parts. The parameter width decides about the width of the

gap.

INVOKE

Devices that consist of more than one Symbols (Gates) can be fetched Gate

by Gate, for example in certain order (Gate D before Gate C), if wanted.

INVOKE can also be used to fetch power supply Gates that do not appear

automatically in the Schematic. This is useful and required, for example,

when you are adding decoupling capacitors to your design.

This command allows you also to add a Gate from a Device which is located

on another sheet. In such a case, type the name of the Device (e.g. IC1) into

the command line after the INVOKE command has been selected.

LINE (was WIRE)

Draw line (this command was is called WIRE in previous versions). The type

of line can be changed with CHANGE STYLE. Clicking the right mouse

button changes the bend mode (SET WIRE_BEND).

LINE can also be used to draw arcs.

Please note the particularities in combination with the Ctrl and Shift key in

the help function:

If you press, for example, the Ctrl key while starting to draw a wire, the wire

begins exactly at the end of an already existing wire nearby. Even if this wire

is not in the currently set grid. Wire width, style and layer will be adopted

from the already existing wire.

4 A First Look at EAGLE

TEXT

Placing text.

Text size, thickness of the lines for vector font texts, the alignment and the

font can be defined in the parameter toolbar of the TEXT command. In case

the text is already placed in your drawing you can make theses changes via

the Properties entry of the context menu or via the different options of the

CHANGE command (Size, Ratio, Align, Font).

Shift + Enter inserts a line break for multi-line texts in the text window.

You can change label texts by assigning a different name to the bus or to a net

by means of the NAME command. See also LABEL command.

CIRCLE

Draw a circle. Circles with a width of 0 are drawn as filled circles.

ARC

Draw an arc (also possible with LINE).

CHANGE CAP FLAT | ROUND defines straight or rounded ends for arcs.

RECT

Draw a rectangle.

POLYGON

Draw a polygon (copper areas in any shape).

BUS

Draw a bus line. The meaning of a bus is more conceptual than physical. It is

only a means to make a schematic easier to read. Only nets define an

electrical connection. Nets, however, can be dragged out of a bus.

The name of a bus can consist of a synonym and the net names that are part

of the bus. In case there is a synonym defined, a LABEL would show the

synonym only, not the whole name of the bus.

Example:

/0$$1-23/0$$1-233+4

A LABEL shows the synonym ATBUS. The bus contains the nets A0 to A31,

B0 to B31, RESET and CLOCK.

NET

Draw a net. Nets with the same name are connected (even if located on

different sheets).

4.2 The Schematic Editor Window

Nets and pins which appear to the eye to be connected are not necessarily

electrically connected. Please check with the SHOW command, the ERC, or

by exporting a netlist or pinlist (EXPORT NETLIST or PARTLIST). See also

the help for MOVE.

JUNCTION

Place the symbol for a net connection. In general, junctions are placed

automatically, but nets which cross over can also be joined manually by the

JUNCTION command.

LABEL

Place the name of a bus or net as a label. Labels cannot be changed with

CHANGE TEXT but rather with the NAME command because the label

represents the net name.

If the label option XREF (in the parameter toolbar or by CHANGE XREF

ON) is set, a cross reference pointing to an further instance of the chosen net

on the next sheet is generated automatically.

The cross reference label format can be defined in the menu

Options/Set/Misc, Xref label format. See the help function of the LABEL

command for the meaning of the placeholders that can be used.

For a proper location of the object you should use a drawing frame with

classifications for columns and rows. Such frames can be defined with the

FRAME command. The library frames.lbr already contains such frames.

ATTRIBUTE

Defines an attribute for a component. Attributes are free definable and can

contain any information.

Through the menu Edit/Global attributes.. you can define attributes that are

valid for all components respectively for the whole schematic.

DIMENSION

Can be used to draw dimension lines.

It is possible to dimension objects drawn in the schematic or you can start

dimensioning at any position in the schematic with Ctrl + left mouse click.

Please look into the description of the DIMENSION command in the section

about the Layout Editor window for more details.

MODULE

The MODULE command defines modules. A module can contain parts and

nets as a part of the whole schematic. The MODULE command also inserts

module instances in the hierarchical schematic. A module instance is drawn

as a simple symbol and represents the usage of a module.

4 A First Look at EAGLE

PORT

The PORT command defines an interface between the nets inside a module

and the higher schematic level. Ports belong to module instances and can be

connected to nets, similar to pins of components.

ERC

Perform an Electrical Rule Check and a consistency check for schematic and

board, if already existing. A positive consistency check allows the

Forward&Back Annotation engine to run.

Commands Not Available in the Command Toolbar

Menu items already explained in the Control Panel section are not discussed

here.

The following commands can be entered into the command line as text

inputs. Some of them are available as menu items. Most of them can be used

in the Schematic and in the Layout and even in the Library Editor.

ASSIGN

Assign function keys.

The most convenient way of doing this is to use the Options/Assign menu.

CLASS

Select and define net classes (Edit/Net classes...). A net class specifies the

width of a track, the clearance from neighbouring signals, and the diameter

of vias for the Autorouter and the ROUTE command. These settings are also

used in polygons. See also page 123.

Text command for closing an editor window (File/Close).

CUT

Transfer the objects of a previously defined group into the paste buffer.

Activate the CUT command and click with the left mouse button into the

group to set a reference point. PASTE inserts the group into the drawing.

Since version 6 this approach has been replaced by the new functionality of

the COPY command. Further information about CUT and COPY can be

found in the help function: Editor commands/CUT.

EDIT

Text command for loading a file or a library object. You can, for instance,

load a board from the Schematic Editor (EDIT name.brd).

The EDIT command is also used to create or edit a module in a schematic

diagram.

5$

loads or creates a module in a circuit diagram.

4.2 The Schematic Editor Window

5$.

loads or creates page number 2 of a module.

FRAME

Define a drawing frame for the Schematic (Draw/Frame). Also possible for a

board drawing.

EXPORT

Output lists (especially netlists), directories, script files, or images

(File/Export...).

Takes care on the hierarchical structure, if existing.

LAYER

Choose or define the drawing layer. When using drawing commands the

layer can be chosen in the parameter toolbar.

To create, for example, a new layer with number 200 and layer name

Mylayer, type in the command line:

6.0078!8

In case you created a Layout, for example, with the EAGLE Light Edition and

upgraded to the Standard Edition because you would like to use two

additional inner signal layers, you have to create these layers with the LAYER

command first:

6.)&.

6-9)&-9

Specifies the contents of the text menu. Now it is located right next to the

action toolbar and can handle small images, as well. See also the example in

the appendix. The text menu can be made visible with the aid of

Options/User Interface. See help function for details.

OPEN

Text command for opening a library for editing (Library/Open). This

command is not identical to the File/Open menu item of the Schematic

Editor, which only lets you select schematics. You can use the OPEN

command as an alternative to the File menu of the Control Panel.

PACKAGE

In case there is more than one Package variant defined in the library for a

part (Device), a typical example would be a resistor from rcl.lbr, it is possible

to change the currently used Package with the PACKAGE or with the

CHANGE PACKAGE command. This can be done in the Schematic or in the

Layout Editor.

4 A First Look at EAGLE

Call up the print dialog with the printer icon in the action toolbar or

from the menu item File/Print.... Usually the PRINT command is used to

print schematics or for checking the drawings needed for the PCB

production.

The actual production data are generated with the CAM Processor.

If you want to output your drawing in black and white check the Black option

(and Solid, if you don't want layers to be printed in their different fill styles).

The caption text is suppressed unless you check Caption. Set Page limit to 1,

if your drawing is to be fitted on one page. If you prefer to print the currently

visible drawing window instead of the whole drawing, select Window instead

of Full in the Area option.

QUIT

Quit EAGLE. Identical with the menu item File/Exit or Alt-X.

REMOVE

Delete files or schematic or module sheets.

7+:$1←

for instance, deletes sheet 3 of the loaded schematic.

SET

Set system parameters and modes. Best done via the Options/Set menu item.

Please note that not all of the possibilities are available through this dialog.

Presettings can be defined in the script file eagle.scr by using text

commands. Further information can be found in the help function.

TECHNOLOGY

If a part (Device) has been defined with various technologies in the library,

see typical examples in 74xx.lbr, it is possible to change the currently used

technology with the TECHNOLOGY or with the CHANGE TECHNOLOGY

command. This can be done in the Schematic or in the Layout Editor.

UPDATE

The UPDATE command checks the parts in a board or schematic against

their respective library objects and automatically updates them if they are

different. (Library/Update... or Library/Update all).

The context menu in the Control Panel's' tree view offers the Options Use all

and Use none for a quick selection of libraries.

VARIANT

This command offers the possibility to define different assembly variants of a

project. It opens a dialog that allows to decide about components to be

assembled or not, or about different values or technologies of the

components used in the different variants of the project. This function can be

reached through the Edit/Assembly variants menu or by typing the

command VARIANT into the command line of the Schematic or the Layout

4.2 The Schematic Editor Window

editor. Further information will be given in chapter 6.10 beginning with page

192.

WRITE

Text command for saving the currently loaded file. Please note that, in

contrast to Save as, the name of the currently edited file is never changed

when the WRITE command is used.

Mouse Keys

The middle and right mouse button have a special meaning for a number of

commands. You can use the middle mouse button only if the operating

system knows your mouse is a 3-button mouse, that is your mouse must be

installed this way.

If you are working with a wheel mouse, you can zoom into and out of the

drawing with the help of the mouse wheel. The option Mouse wheel zoom in

the Options/User Interface menu determines the zooming in/out factor per

step. The value is set to 1.2 by default.

Selecting a value of 0 allows you to use the wheel for scrolling.

Keep the mouse wheel or the middle mouse button pressed for panning.

Mouse clicks in combination with the Shift, Ctrl, and Alt key can have various

functions, for example, while selecting objects with MOVE or while drawing

lines with LINE.

The help section on Keyboard and Mouse and the help of the referring

command gives you more details.

Selecting Neighbouring Objects

If one of two objects which are very close together is to be selected, the

individual objects are highlighted one after the other. The user can select the

highlighted object with the left mouse button, or proceed to the next one with

the right mouse button. The status bar of the editor window shows

information about the pre-selected object. See also help function (SET

command, SELECT_FACTOR).

4.3 The Layout Editor Window

The Layout Editor window opens when you open an existing board file or

create a new board. If you own the Schematic Editor you will normally draw

a schematic first and then generate the board file with the BOARD

command, or by clicking the Board icon.

The Layout Editor window appears very much like the Schematic Editor

window. Even if you don't work with the Schematic Editor, you should study

the previous section, as most of the information there applies to the Layout

Editor, too.

4 A First Look at EAGLE

Only the commands in the command toolbar are discussed again, as some

commands differ in their use.

Descriptions of commands that cannot be reached through the command

toolbar are also to be found in the section concerning the Schematic Editor

window. All of the commands can also be reached through the pull-down

menus in the menu bar. This also applies, of course, to the Schematic and

Layout Editor windows.

The Commands on the Layout Command Toolbar

INFO

Shows the properties of the selected object. Typing INFO IC1 in the

command line results in the properties dialog of the object named IC1.

Depending on the selected object some of the properties can be altered here.

SHOW

Highlights the object to be selected with the mouse.

It's also possible to enter the object's name (even several names at once) in

the command line. * and ? are allowed to be used as wildcards, as well.

Ctrl + SHOW toggles the show state of the selected object.

➢

Layout Editor window

4.3 The Layout Editor Window

DISPLAY

Select and deselect the layers to be displayed. Components on the top side of

the board can only be selected if the layer 23, tOrigins, is displayed. The

same applies to components on the bottom side of the board and layer 24,

bOrigins.

See Appendix for the meaning of the layers.

The DISPLAY command supports so-called Layer Presets (Aliases). This

allows you to name certain combinations of layers and use it as a parameter

with the LAYER command. A quick change from one view to another layer

combination is possible with this command.

Double-click one of the layer entries for changing its color or fill style.

DISPLAY LAST switches to the last displayed layer combination.

The DISPLAY menu shows only those layers defined in the Layer

Setup of the Design Rules!

Further information about DISPLAY can be found in the help function.

➢

The Display menu

➢

Change layer properties

4 A First Look at EAGLE

MARK

The following mouse click defines the new origin for the coordinate display.

Relative coordinates (R x-value y-value) and polar values (P radius angle)

are shown in addition to absolute coordinates in the coordinate display box.

If you first click the MARK icon and then the traffic-light icon, only the

absolute coordinate values will be displayed again.

GROUP

Define a group which can then be moved, rotated, or copied with COPY and

PASTE to another drawing or whose properties should be changed.

By default the GROUP command is always active. If you click into empty

space of a drawing and hold the mouse button you can drag a rectangle or

draw a polygon around the objects in the group. After defining the group you

can immediately move it without having to select a command icon by clicking

and holding the mouse button onto a groups’ object.

If the option GROUP command default on is not active or you want to

execute another command with the group, define the group, select for

example a command icon (for rotate, copy…..) and execute it on the group

with Ctrl + right mouse-click.

GROUP ALL in the command line selects all objects.

To be sure that all objects are selected DISPLAY ALL layers before. On the

other hand, deselecting specific layers can exclude certain objects from the

selection.

Further information about GROUP can be found in the section about the

Schematic Editor and in the help function.

MOVE

Move any visible object. The right mouse button rotates the object.

The MOVE command cannot connect signals even if a wire (trace) is

moved over another wire or a pad. Use ROUTE to route signals.

Keeping the Ctrl key pressed while selecting an object selects it in a

particular manner. Please consult the help function for details (CRICLE,

ARC, LINE, MOVE, ROUTE etc.).

For moving groups, please see MOVE in the Schematic Editor section.

MIRROR

Mirror objects. Components can be placed on the opposite side of the board

by using the MIRROR command.

4.3 The Layout Editor Window

ROTATE

Rotate objects (also possible with MOVE). Keep the left mouse button

pressed to rotate the selected object by moving the mouse. The parameter

toolbar shows the current angle. This can be done with groups (GROUP and

right mouse button)as well.

ROTATE can be used with groups, as well. Activate ROTATE, press the Ctrl

key and click with the right mouse button into the drawing to set the center

of rotation. The group will be rotated counterclockwise by the given angle.

Alternatively type in the angle in the Angle box or in the command line.

Details about the syntax can be found in the help function.

ALIGN

The ALIGN command can be used to align selected objects in relation to each

other or to move their origin location to the nearest grid point.

The following modes are supported:

- Align Edges Top | Bottom | Left | Right

- Align Centers Vertical | Horizontal

- Distribute Vertically | Horizontally

- Align Origin to Grid

COPY

Copy parts and other objects.

When copying objects, a new name will be assigned, but the value will be

retained. When copying a single wire, the copy will have the same name.

Keep the Ctrl key pressed while clicking onto an object and the object will be

grabbed at its origin. So it will be placed in the currently chosen grid.

COPY can be used with groups. The group will be put into the clipboard of

the operating system. It is possible to copy it into another EAGLE program,

for example.

PASTE

Insert objects from the paste buffer.

Use the menu Edit/Paste from... in order to paste a whole layout (and

schematic, if available) into your current drawing. See help for further

information.

DELETE

Delete visible objects.

If a group has been defined, it can be deleted with the right mouse button

while the Ctrl key is pressed.

4 A First Look at EAGLE

DELETE SIGNALS in the command line erases all tracks and signals in the

layout, provided there is no consistent schematic loaded.

The DELETE command deletes an entire polygon when clicking on a polygon

wire with the Shift key pressed.

Keeping the Ctrl key pressed while clicking with the left mouse button on a

wire bend will delete the bend. A new direct connection between the next

bends will be drawn now.

If objects cannot be deleted, the reason can lie with error polygons related to

the DRC command. They can be deleted with the ERRORS command

(ERRORS CLEAR). If layer 23, tOrigins, or 24, bOrigins, is not displayed,

components cannot be deleted.

CHANGE

Change the properties of an object, for example the width of a wire or the size

of a text. If the Esc key is pressed after changing a property, the previously

used value menu will appear again. In this way a new value can be

conveniently chosen. See also the help function.

Alternatively, object properties can be viewed and some of them even

changed with the context menu's Properties entry. The context menu opens

after a right mouse click onto the object.

PASTE DBL

Add a Design Block into the drawing. If the Design Block consists of board

and schematic the Layout part can be placed with the mouse cursor. The

Schematic part will be added automatically to the Schematic on new sheets

accordingly.

ADD

Add library elements to the drawing. It offers a convenient search function

for Packages here. USE specifies which libraries are available.

A right-click onto the ADD icon opens a popup menu that contains a list of

recently placed Devices.

PINSWAP

Swap two signals connected to equivalent pads of a component, provided the

pins have been defined with the same Swaplevel.

A pin that is connected to several pads can't be swapped.

REPLACE

Replace a component (or a Package, if there is no schematic) by another one

from any library.

If you want to change the Package variant only and not the whole Device, use

CHANGE PACKAGE or the PACKAGE command.

4.3 The Layout Editor Window

A right-click onto the REPLACE icon opens a popup menu that shows a list

of recently replaced components.

LOCK

Locks the position and orientation of a component on the board. If a

component is locked, you can't move it or duplicate it with CUT and PASTE.

Shift + LOCK unlocks the component. This is also possible with the unLock

entry of the context menu.

To be able to distinguish locked from unlocked components, the origin cross

of a locked component is displayed like a 'x' instead of a '+'.

The position of a locked component can be changed, however, by typing in

new coordinate values in the properties dialog.

NAME

Give names to components, signals, vias, and polygons.

With NAME it's possible to move a polygon from one signal to another.

VALUE

Provide values for components. A resistor, for example, gets 100k as its

value. A right-click onto this icon opens a list of already used values. Select an

entry and apply it to one or more components by clicking onto them

successively.

SMASH

Separate name, value, and attribute (if any) texts from a Device, so that they

can be placed individually. The size of detached (smashed) texts can also be

individually changed.

Also in combination with GROUP. If a group is defined, you can smash it

with a right mouse click while the Ctrl key is pressed.

Use the DELETE command to hide smashed texts.

Keep the Shift key pressed while using the SMASH command in order to

unsmash texts. They are not editable any more and appear at their original

positions after a window refresh (also possible with unSmash in the context

menu).

Alternatively you can switch on or off the option Smashed in the context

menu's Properties entry.

MITER

Round off or bevel wire joints (also possible for polygon contours). The grade

of mitering is determined by the miter radius. Positive sign results in a

rounded joint, negative sign in a bevel.

The miter radius influences some wire bend modes, too (see help function:

SET, Wire_Bend).

4 A First Look at EAGLE

SPLIT

Insert a bend into a wire.

If you want to change, for example, the layer for a section of an already

routed track, you can insert two wire bends with the SPLIT command and

change the layer of the newly created segment with the CHANGE LAYER.

EAGLE will set vias automatically at the position of the wire bends.

You can use the SPLIT command for a quick re-routing of an already existing

track. Click onto the track to insert a wire bend. Now move the mouse and

route it anew. To remove the previous track use the RIPUP command or

DELETE in combination with the Ctrl key.

OPTIMIZE

Joins wire segments in a signal layer which lie in one straight line.

MEANDER

Draw meanders in order to balance the length of signals, especially of

Differential Pairs. Can be used for measuring the length of a signal, when

pressing the Ctrl key.

SLICE

The SLICE command cut lines in two parts. If it is a routed trace the gap

contains an airwire that connects the two parts of the signal. So a signal is

actually not cut into two different parts, but it rips up the trace according to

the given width of the gap. Simply click left to start the cutting wire, a second

click ends it. All objects crossing the cutting wire will be slices. Exception is a

polygon’s contour. SLICE can be used in the command line. The cutting line

is defined by start and end coordinates, like SLICE (0.2 3) (0.5 4);

ROUTE

Route signals manually. Airwires are converted to wires.

By default the ROUTE command works in “Obstacle Avoidance” mode. So it

automatically takes care on Design Rules and avoids obstacles that are along

the path of a trace. If the routing mode is set to “Ignore Obstacle” mode by

clicking on the icon in the parameter toolbar, the user has to take care on all

the Design Rules by himself.

The ROUTE command also supports the Follow-me router mode which

automatically processes the trace of a selected signal with the Autorouter

running in the background.

ROUTE offers several options with the different mouse buttons, also in

combination with the Ctrl and Shift key.

Ctrl + Left starts routing at any given point along a wire or via

Shift + Left if the airwire begins at an already existing wire and

this wire has a different width, the new wire adopts

4.3 The Layout Editor Window

this width

Center selects the layer

Right changes the wire bend style

Shift +Right reverses the direction of switching bend styles

Ctrl + Right toggles between corresponding bend styles

Shift + Left places a via at the end point of the wire

Ctrl + Left defines arc radius when placing a wire's end point

More information can be found in the help function of the ROUTE

command. See also Group Default On.

RIPUP

Convert routed wires (tracks) into unrouted signals (airwires). Change the

display of filled (calculated) polygons to outline view.

Using signal names in the command line allows you to ripup only certain

signals, to exclude particular signals, or to execute the command exclusively

for polygons. More details can be found in the help function.

Wires not connected to components must be erased with DELETE.

LINE

Draw lines and arcs. If used in the layers 1 through 16, the LINE command

creates electrical connections.

The Style parameter (CHANGE) determines the line type. The DRC and the

Autorouter always treat a LINE as a continuous line, regardless of what Style

is used.

Clicking the right mouse button changes the wire bend (SET WIRE_BEND).

Please note the particularities in combination with the Ctrl and Shift key in

the help function:

If you press, for example, the Ctrl key while starting to draw a wire, the wire

begins exactly at the end of an already existing wire nearby. Even if this wire

is not in the currently set grid. Wire width, style and layer will be adopted

from the already existing wire.

TEXT

Placing text. Use CHANGE SIZE to alter the height of the text. If the text is

using a vector font, CHANGE RATIO will alter the thickness. CHANGE TEXT

is used to alter the text itself. CHANGE FONT alters the typeface. CHANGE

ALIGN defines the alignment (the location of the origin) of the text.

The option Always vector font (Options/User Interface) shows and prints all

texts in vector font, regardless of which font is actually set for a particular

text.

If you want to have inverted text in a copper layer, you have to enter the text

in the layers 41, tRestrict, or 42, bRestrict, and draw a copper plane in Top or

Bottom layer around the text with the POLYGON command. The polygon

keeps the restricted areas (which is the text) free from copper.

4 A First Look at EAGLE

Use Shift + Enter in order to insert a line break for multi-line texts. The line

distance can be set via the Properties window or in the parameter toolbar, as

long as the text is not yet placed and still attached to the mouse cursor.

It is strongly recommended to write texts in copper layers as vector

font! So you can be sure that the CAM Processor's output is identical

with the text shown in the Layout Editor. See also help function.

CIRCLE

Draw a circle. This command creates restricted areas for the

Autorouter/Follow-me router, if used in the layers 41, tRestrict, 42,

bRestrict, or 43, vRestrict. Circles with wire width = 0 are drawn as filled.

ARC

Draw an arc (also possible with LINE).

CHANGE CAP FLAT | ROUND defines straight or rounded ends for arcs.

If the arc is a part of a trace and both ends are connected to a wire, caps will

be round.

Arcs with flat caps are emulated when generating manufacturing data in

Gerber format with the CAM Processor. That means they will be drawn with

small short straight lines. Arcs with round caps won't be emulated.

RECT

Draw a rectangle. This command creates restricted areas for the Autorouter

or Follow-me router, if used in the layers 41, tRestrict, 42, bRestrict, or 43,

vRestrict.

POLYGON

Draw a copper areas or restricted areas in signal layers.

Polygons in the signal layers are treated as signals. They keep an adjustable

distance to objects belonging to other signals (copper pouring, flood fill). This

enables you to realize different signal areas on the same layer and make

isolated regions for your design.

The contour of a polygon in the outline mode is displayed as a dotted line.

The POLYGON command creates restricted areas for the Autorouter/Follow-

me router, if used in the layers tRestrict, bRestrict, or vRestrict. For other

possibilities of the POLYGON command see help.

Polygons with special fill style cutout can be used as restricted areas for

signal polygons in inner and outer layers. Such a polygon will be subtracted

from all other signal polygons in the same layer. The dotted contour line will

always be visible. The wire width for such a polygon may be 0 as well.

4.3 The Layout Editor Window

VIA

Place a plated-through hole. Vias are placed automatically if the layer is

changed during the ROUTE command. You can assign a via to a signal with

the NAME command by changing it's name to the name of the signal. Vias

can have different shapes in the outer layers (round, square, octagon) , but

are always round in inner layers.

SIGNAL

Definition of a signal. This is not possible if the Forward&Back Annotation is

active. In that case you have to define the connection with the NET command

in the Schematic Editor.

HOLE

Define a mounting hole (not plated-through).

ATTRIBUTE

Defines an attribute for a component.

Through the menu Edit/Global attributes.. you can define attributes that are

valid for the whole layout.

DIMENSION

Can be used to add dimensioning to the board. It can either be applied to an

object or you can draw arbitrary dimensions. When you select an object

EAGLE selects a suitable dimensioning type (Dtype). If it is not the one

needed, click the right mouse button to change it. If you want to start at any

location in the drawing use Ctrl key + left mouse click.

There are different dimensioning types: Parallel, Horizontal, Vertical,

Radius, Diameter, Angle, and Leader.

Configuration of dimensioning lines, text size units and so on can be done in

the objects' properties dialog or with the CHANGE command, which can be

executed for groups of objects, as well:

CHANGE Dtype changes the dimensioning type

CHANGE Dunit decides about the measurement unit,

the precision,

and about showing or hiding the unit.

CHANGE Dline determines the width of the measurement line,

the width of the extension line,

the Extension length after the dimension arrow head,

the distance from the object measured (Extension,

offset).

4 A First Look at EAGLE

RATSNEST

Calculate the shortest airwires possible and the real mode (filled) display of

polygons.

Use the RATSNEST command with a signal name in order to calculate and

display or hide a certain airwire. A preceding exclamation mark hides the

airwires of the given signal name. More information can be found in the help

function.

The polygon calculation can be deactivated with the SET command. Either

through the menu Options/Set/Misc or by typing in the command line:

SET POLYGON_RATSNEST ON | OFF or in short: SET POLY ON | OFF.

RATSNEST will be executed automatically for the selected signal while

drawing a wire with ROUTE.

While RATSNEST is active the status bar of the Layout Editor displays the

name of the currently calculated signal.

AUTO

Start the Autorouter.

If you type AUTO FOLLOWME in the command line, the Autorouter Setup

window opens in the follow-me mode, which allows to set the parameters for

the follow-me router only.

AUTO BGA

Start the BGA Autorouter.

If you type AUTO BGA or click this icon, EAGLEs start a special Autorouter

in order to route signals connected to BGA components out of the BGA area.

In a first step you select the BGA component(s) in the layout. Second, you

select the signals that shall be routed. You can also decide about the layer

assignment for the signals. Micro Vias are supported, if this option is

enabled.

Please verify Design Rules before starting the BGA router!

ERC

Perform a consistency check for schematic and board.

DRC

Define Design Rules and perform Design Rule Check.

Typing DRC * into the command line opens the Design Rules window where

you can check and adjust your settings and close the dialog window again

without starting the Design Rule Check.

4.3 The Layout Editor Window

ERRORS

Show errors found by the DRC. If you haven't already processed a Design

Rule Check for the board, it will be done automatically before showing the

error list, if there are any errors found.

There are further commands for the Layout Editor, as they are in the

Schematic, that are not available in the Command Menu. Please take

a look at the section beginning with page 62. Most of them are valid

in Schematic and Layout.

4.4 The Library Editor Window

The Library Editor window opens when you load one of your libraries for

creating or editing components. A library normally has three different

elements: Packages, Symbols, Devices, and, if assigned, a reference to a 3D

package.

A Package is a Device's housing, as will be used in the Layout Editor

(on the board).

The Symbol contains the way in which the Device will be shown in the

schematic.

The Device represents the link between one (or more) Symbol(s) and

a Package. Here we define the connection between a pin of a Symbol

and the referring pad(s) of the Package.

We call it a Device set if the component exists in more than one

Package and/or technology variant.

A 3D representation of a package can be an assigned model in STEP

file format. The 3D models are offered in our online repository or

could be your own uploaded 3D model.

All Managed Libraries have assigned simple 3D boxes by default

which can be replaced by 3D STEP file models with a web based

editor.

A library need not contain only real components. Ground or supply symbols

as well as drawing frames can also be stored as Devices in a library. These

Symbols do not normally contain any pins.

There are also libraries that only contain Packages. These libraries can only

be used in the Layout Editor.

Extensive examples of the definition of library elements are to be found in a

section entitled Component Design Explained through Examples, starting on

page 229 in this manual.

Table Of Contents

When a user library is loaded the following window appears first:

4 A First Look at EAGLE

➢

Library Editor: Table of Contents with four columns for

Devices, Packages, 3D Package, and Symbols

The table of contents of this library is shown. Four columns list all Devices,

Packages and Symbols available in the library file. Here no 3D packages are

assigned yet. This could be done by clicking the button Edit 3D Packages on

Web.

Double-click on of the entries to start the editing mode.

A right mouse-click opens a context menu offering a number of options, like

Edit, Remove, Rename and Edit Description.

The context menu of a Device contains also the entries Used packages and

Used symbols, of a Package or Symbol there is an entry Using DeviceSets.

This helps to understand where a Package or Symbol is used in a Device Set.

This information is already visible in the columns. In the Device column the

first entry is selected. Looking into Package and Symbol columns, you see

entries marked with underlying gray. These are the Symbols and the Package

used in the selected Device.

With clicking one of the Add…. buttons below the columns you can create a

new Device, Package or Symbol or import an object from another library.

4.4 The Library Editor Window

Important Icons in the Library Editor

Load Device, Package or Symbol for editing. This icon is located in the

command icon toolbar

From the left: Show table of contents, Load Device, load Package, load

Symbol. These icons are shown in the action toolbar.

If you click on one of these icons with the right mouse button, or long-click

with the left mouse button on one of theses icons (not show table of

contents), a list with the recently edited objects will pop up.

Alternatively there are available the options Description, Table of Contents,

Manage Devices/Symbols/Packages… (EDIT command), Remove, Rename,

and Update... through the Library menu.

Please check the chapter Library and Part Management and the help

function for additional information.

The Package Editing Mode

The definition of a component is described briefly below. There is a more

extensive guide in the Component Design Explained through Examples

section.

The icons available in the command toolbar are equivalent to the identical

icons of the Schematic or Layout Editor.

➢

A Library's Table of Contents: Options of the context menu

4 A First Look at EAGLE

Design New Package

You change into Package editing mode through the Package icon in the

action toolbar. Type in the name of a package, and reply to the confirming

question Create new package 'packagename'? with yes.

Place pads (though-hole contacts) or SMDs (SMD contact areas) with the

following commands which are only available in the Package Editor.

PAD

Place the pad of a conventional (through-hole) component.

The pad comes with a plated-through drill that goes through all signal layers.

The pad shape can be round, square, octagon or long in the outer signal

layers. In the inner signal layers pads are always round.

SMD

Place a SMD pad.

You can change the name of the pads or SMDs with the NAME command.

Use the LINE, ARC, etc. commands to draw

the symbol for the silkscreen on layer 21, tPlace,

additional graphical information for the documentation print

into layer 51, tDocu.

Draw restricted areas for the Autorouter, if needed, in layers 41, tRestrict, 42,

bRestrict, or 43, vRestrict, or in layers 39, tKeepout, or 40, bKeepout, by

using the commands CIRCLE, RECT, or POLYGON.

Place mounting holes with the HOLE command, if needed.

Use the TEXT command to place

the string >NAME in layer 25, tNames, serving as a text variable

containing the name of the component,

the string >VALUE in layer 27, tValues, serving as a text variable

containing the value of the component.

Use the DESCRIPTION command to add a description for the Package.

HTML text format can be used for this. You will find further information in

the help pages.

The Symbol Editing Mode

Defining a Symbol means defining a part of a Device which can be placed

individually in a schematic. In the case of a 74L00 this could be one NAND

gate and the two power pins, defined as another Symbol. In the case of a

resistor, the Device contains only one Symbol which is the representation of

the resistor.

You now change into Symbol editing mode through the Symbol icon in

the action toolbar. Enter the name of the Symbol, and reply to the confirming

question Create new symbol 'symbolname'? with Yes.

4.4 The Library Editor Window

Design a New Symbol

Use the commands LINE, ARC, etc. to draw the schematic representation of

the Symbol into layer 94, Symbols.

Place the pins by using the following PIN command, which is only available

in the Symbol editing mode:

Place pins.

You can adjust the pin parameters (name, direction, function, length, visible,

Swaplevel) in the parameter toolbar while the PIN command is active, or

later with the CHANGE command. The pin parameters are explained starting

on page 238 and in the help pages under the keyword PIN. Pin names are

changed using the NAME command.

Use the TEXT command to place

the string >NAME in layer 25, tNames, serving as a text variable

containing the name of the component,

the string >VALUE in layer 27, tValues, serving as a text variable

containing the value of the component.

The Device Editing mode

Components are defined as Devices. In the Device editing mode you do not

draw anything, but you define the following:

which Package variant is used,

which Symbol(s) is/are used (called Gate within the Device),

which names are provided for the Gates (e.g. A, B),

which technologies are available (e.g. 74L00, 74LS00, 74HCT00),

if the Device should have additional user-definable attributes,

if there are equivalent Gates which can be interchanged (Swaplevel),

how the Gate behaves when added to a schematic (Addlevel),

the prefix for the component name, if a prefix is used,

if the value of the component can be changed or if the value should be

fixed to the Device name,

which pins relate to the pads of the Package (CONNECT command)

whether a description for this component should be stored in the

library.

The following diagram shows the fully defined 7400 Device with four NAND

gates and a supply gate in various Package and technology versions.

If you click onto one of the gates with the right mouse button, the context

menu with the executable commands pops up. Furthermore you can display

the Properties of the gate. Click on Edit Symbol to open the Symbol Editor.

4 A First Look at EAGLE

➢

Device Editor window

Create Actual Components from Symbols and Packages

Switch to the Device editing mode by clicking the Device icon in the

action toolbar. Type in the Device name and confirm the question Create

new device 'devicename'? with Yes.

Use the following commands to create a Device.

ADD

Add a Symbol to a Device. Gate name, Swaplevel, and Addlevel can be

defined in the ADD command in the parameter toolbar, or redefined later

with the CHANGE command.

The Swaplevel specifies whether there are equivalent Gates.

The Addlevel defines, for instance, if a Gate is to be added to the schematic

only on the users request. Example: the power gate of an integrated circuit

which is normally not shown on the schematic.

NAME

Change Gate name.

4.4 The Library Editor Window

CHANGE

Change Swaplevel or Addlevel.

PACKAGE

Define and name Package variant(s). The PACKAGE command is started by

clicking on the New button in the Device Editor window, or by typing on the

command line. Choose the requested Package variant.

More information about this can be found on page 283.

CONNECT

Define which pins (Gate) relate to which pads (Package).

PREFIX

Provide prefix for the component name in the schematic (e.g. R for resistors).

VALUE

In the Device mode, VALUE is used to specify whether the component value

can be freely selected from within the schematic diagram or the layout, or

whether it has a fixed specification.

On: The value can be changed from within the schematic (e.g. for resistors).

The component is not fully specified until a value has been assigned.

Off: The value corresponds to the Device name, including, when present,

assignment of the technology and the Package version (e.g. 74LS00N).

Even if Value is Off, the value of a component can be changed. A query

checks if this action is intended.

The altered value of the component remains unchanged, if the Technology or

the Package version is altered later with CHANGE PACKAGE or CHANGE

TECHNOLOGY.

TECHNOLOGY

If necessary, various technologies can be defined, for example, for a logic

component. Click on Technologies therefore.

ATTRIBUTE

Click on Attributes to define any additional attribute for the Device. A

detailed description can be found in the chapter about libraries in this

manual.

DESCRIPTION

Compose a description of the Device which can also be examined by the

search function associated with the ADD dialog.

Information about Copying of Packages, Symbols and Devices can be

found from page 288 on.

4 A First Look at EAGLE

4.5 The CAM Processor

Manufacturing data is generated by means of the CAM Processor. A number

of drivers for the data output are available. The drivers are defined in the file

eagle.def, which can be edited with any Text Editor.

Output to matrix printers, however, is not created with the CAM Processor

but with a PRINT command.

The board manufacturer may use the EAGLE Freeware for generating

manufacturing data of your board.

➢

The CAM Processor

The CAM Processor can also be started directly from the command line. A

number of command line parameters can be passed to it when it is called.

These are listed in the appendix.

Generate Data

Starting the CAM Processor

There are different ways to start the CAM Processor:

You can do this directly from the Layout or Schematic Editor window with

the CAM Processor icon in the action toolbar or through the menu

File/CAM Processor. The current schematic or board will be loaded

automatically from the Control Panel by clicking on one of the entries in the

Tree View's CAM Jobs branch. Then the selected CAM Job will be loaded

automatically. You still have to load the schematic or board from which you

want to make the CAM Processor manufacturing data from through the

4.5 The CAM Processor

File/Open menu by using the command prompt (Windows command

prompt, Terminal or Console window) without graphical user interface.

Particular information can be found in the appendix chapter about EAGLE

Options.

Load Job File

A job defines the sequence of several output steps in an automatic data

creation task. You can, for example, use a job to generate individual files

containing the Gerber data for several PCB layers.

A job is loaded with the File menu of the CAM Processor or with a double-

click on one of the Tree view's CAM Jobs entries in the Control Panel.

A job is not absolutely essential for output. All the data can be made step by

step manually.

Load Board

Before you can generate an output you must open the File menu and load a

board file, if not already loaded automatically while stating the CAM

Processor from an Editor window. At the bottom left in the CAM Processor

window you will see the file name the data is being generated from.

The output of data for a Schematic, for example for a certain plotter, is also

possible.

Set Output Parameters

If a job file is loaded, the output parameters are already adjusted. A job can

contain several sections with different parameter sets. The various peripheral

devices accept different parameters.

If no job is loaded, set the parameters to whatever you need (see page 311).

Start Output

If you want to execute the job which has been loaded, click the Process Job

button. If you just want to get an output using the currently visible parameter

settings, click the Process Section button.

Define New Job

Perform the following steps to define a new job:

1. Click Add, to add a new section.

2. Set parameters.

3. Repeat 1. and 2. if necessary.

4. Save job with File/Save job.

The Description button allows to describe the job file. This description will be

shown in the Control Panel.

The chapter on Preparing the Manufacturing Data contains detailed

information on this subject.

4 A First Look at EAGLE

4.6 The Text Editor Window

EAGLE contains a simple Text Editor.

You can use it to edit script files, User Language programs or any other text

file. The EAGLE Text Editor stores its files with UTF-8 encoding.

The menus bring you to a variety of functions, such as commands for

printing, copying and cutting, searching, replacing (with support of Regular

Expressions), changing font and size, and so on.

The keyboard shortcuts in the EAGLE Text Editor follow the platform

specific standards.

When in the Text Editor, the right mouse button calls up a context menu.

In case you prefer an external text editor, define the program call in the

Control Panel's or in one of the Editor window's Option/User interface

menu, External text editor. If you want to prevent EAGLE to start any text

editor automatically, type in a minus sign '-' in the External text editor line.

Clear the line for the built-in EAGLE text editor.

Please note further information about the usage of an external text editor in

the help function, section Editor windows/Text Editor.

Chapter 5

Principles for Working with EAGLE

5.1 Command Input Possibilities

Usually the commands in EAGLE are executed by clicking an icon or an item

in the menu bar and then clicking onto the object you want to edit. But there

are also alternative to execute commands.

Possibilities for command input in Schematic, Layout, and Library Editor:

clicking a command icon

typing text commands in the command line

through the context menu

via function keys

via script files

via User Language programs

In any case it is necessary to understand the syntax of the EAGLE command

language which is described in the following section.

A detailed description of the EAGLE commands can be found on the help

pages.

Activate Command and Select Object

The classical way of working with EAGLE is to activate the command first,

and then choose the object you want to have it executed on. For example,

first activate the MOVE command by clicking the icon in the command menu

or selecting the command in one of the menus, and finally click onto the

object you want to move.

Command Line

As an alternative to the previously mentioned clicking onto an icon you can

use the command line. When entering commands you may abbreviate key

words as long as they cannot be mistaken for another key word, or you may

use small or capital letters (the input is not case sensitive), for example:

*5*0$0.;

is equivalent to

(<=0$0.;

5 Principles for Working with EAGLE

The actual unit for the values is set in the GRID menu. It's also possible to

specify the unit directly in the command line without changing the currently

set grid:

*5*0$>77

(<=.;=!

Most commands can be executed whilst declaring coordinate values in the

command line.

Examples:

7+:-?:@.$90-$A9B

The value placeholder text for part IC1 moves to position 2.50 1.75 in the

layout, provided it has been released with the SMASH command before.

7+-

Part U1 will be mirrored to the bottom side of the board.

*+0$-9@9#$9B

Place a hole with drill diameter 0.15 at position 5 8.5.

:C5C0$0A0)@.$01$0B

A round shaped via with a diameter of 0.070 belonging to signal GND will be

placed at position 2.0 3.0.

History Function

You can recall the most recently entered commands by pressing Crsr-Up ( )

or Crsr-Down () and edit them. The Esc key deletes the contents of the

command line.

The Context Menu

Another way of using EAGLE is to work with the object-specific command

menu. In this case you first click with the right mouse button onto the object

and then you select the command that you want to have executed.

The context menu contains all commands that can be executed with the

selected object. Additionally you can display all the object's properties by

clicking onto the Properties entry. Some of them can be even changed

directly in the Properties window.

5.1 Command Input Possibilities

Function Keys

Texts may be allocated to the function keys and to combinations of those keys

with Alt, Ctrl and Shift (for Mac OS-X additionally Cmd), if not occupied by

the operating system or a Linux Window Manager (for example F1 for help).

If a function key is pressed, this corresponds to the text being typed in via the

keyboard. Since every command is capable of being entered as text, every

command, together with certain parameters, can be assigned to a function

key. Even whole sequences of commands can be assigned to a function key in

this way.

The command

ASSIGN

displays the current function key assignments. Changes to the key

assignments can be carried out in the assign window.

The New button can be used to define a new key assignment. A click onto Del

will delete a marked entry, while Change alters an existing definition. OK

closes the dialog and saves the definitions, while Cancel aborts the dialog.

These settings can also be made via the Options/Assign menu in the

Schematic or Layout Editor.

To predefine certain assignments you can also use the ASSIGN command in

the file eagle.scr (see page 111).

➢

The context menu for a Device in the Schematic

5 Principles for Working with EAGLE

➢

The dialog for the ASSIGN command

Examples:

The combination of Ctrl + Shift + G displays a grid of 0.127mm:

DC5770$-.A+C

The combination of Alt + F6 changes the layer to Top and starts the ROUTE

command:

DE>C6++C

The combination of the keys Alt + R displays only the layers Top, Pads, Vias

and Dimension first and then starts the print out with the default printer:

DC56+--A-#.0C

A, C, M, and S are the modifiers for the Alt, Ctrl, Cmd (Mac OS-X only), and

Shift key.

The combination of Alt + 0 brings the Control Panel into the foreground. The

combinations Alt + 1 up to 9 are assigned to the various editor windows,

according to the window number which is shown in the respective title bar.

Script Files

Script files are a powerful tool. They can contain long sequences of

commands, such as the specification of specific colors and fill-patterns for all

layers, as for example in defaultcolors.scr. On the other hand they might

contain netlists converted from the data of other programs.

The SCRIPT command is used to execute script files.

5.1 Command Input Possibilities

Many User Language programs (ULP) create script files that can be read in

order to modify a layout or a schematic.

EAGLE outputs an entire library, for instance, as a script file with the aid of

the EXPORT command (Script option). This file can be modified with a text

editor, after which it can be read in again. This allows changes to be made to

a library quite easily.

There is more information about script files and export commands later in

this chapter.

Mixed Input

The various methods of giving commands can be mixed together.

You can, for instance, click the icon for the CIRCLE command (which

corresponds to typing CIRCLE on the command line), and then type the

coordinates of the center of the circle and of a point on the circumference in

this form

@..B@.1B←

in the command line.

The values used above would, if the unit is currently set to inch, result in a

circle with a radius of one inch centered on the coordinate (2 2). It is

irrelevant whether the CIRCLE command is entered by icon or by typing on

the command line.

Some EAGLE commands are used in combination with the Shift, Alt

or Ctrl keys. In case you are working with EAGLE for Mac OS-X,

please use the Cmd key instead of Ctrl.

5.2 The EAGLE Command Language

You only need a knowledge of the EAGLE command language if you want to

make use of the alternative input methods discussed in the previous section.

The syntax of the EAGLE command language will be discussed in this

section, and typographical conventions, which are important for

understanding the descriptions, will be specified.

Typographical Conventions

Enter key and Semicolon

If EAGLE commands are entered via the command line they are finished

with the Enter key. In some cases a command must have a semicolon at the

end, so that EAGLE knows that there are no more parameters. It is a good

idea to close all commands in a script file with a semicolon.

The use of the Enter key is symbolized at many places within this handbook

with the ← sign.

However in the following examples neither the Enter key sign nor the

semicolon are shown, since all of these commands can be used both on the

command line and within script files.

5 Principles for Working with EAGLE

Bold Type or Upper Case

Commands and parameters shown here in UPPER CASE are entered

directly. When they are entered, there is no distinction made between upper

and lower case. For example:

Syntax:

5

Input:

5or=!="

Lower Case

Parameters shown here in lower case are to be replaced by names, numbers

or keywords. For example:

Syntax:

5="=F=)!GH!

Input:

5--0

This sets the grid to 1 mm (assuming that the current unit is set to mm).

Every tenth grid line is visible. The figures 1 and 10 are placed into the

command instead of the placeholders grid_size and grid_multiple.

Underscore

In the names of parameters and keywords the underscore sign is often used

in the interests of a clearer representation. Please do not confuse it with an

empty space. As can be seen in the example above, grid_size is a single

parameter, as is grid_multiple.

If a keyword contains an underscore sign, such as COLOR_LAYER does in

the command

++6!8!<

then the character is to be typed in just like any other. For example:

++6++7

Spaces

Wherever a space is permissible, any number of spaces can be used.

Alternative Parameters

The | character means that the parameters are alternatives. For example:

Syntax:

+I+EE

Input:

+

+EE

The beep, which is triggered by certain actions, is switched on or off.

5.2 The EAGLE Command Language

Repetition Points

The .. characters mean either that the function can be executed multiple

times, or that multiple parameters of the same type are allowed. For

example:

Syntax:

56HG!8$$

Input:

56+:

The layer number can alternatively be used:

56--A-#

More than one layer is made visible here.

If a layer (in this case Bottom) is to be hidden:

56->

Mouse Click

The following sign ● usually means that at this point in the command an

object is to be clicked with the left mouse button.

For example:

7+:●●

Input:

7+:←@!=J&(=B

7)"!=J&( "&KL&&KM

7)"!=J&("GG

7)"!=J&("KL&&KM

"$

You can also see from these examples how the repetition points are to be

understood in the context of mouse clicks.

Entering Coordinates as Text

The program sees every mouse click as a pair of coordinates. If it is desired to

enter commands in text form on the command line, then instead of clicking

with the mouse it is possible to enter the coordinates through the keyboard in

the following form:

(x y)

where x and y are numbers representing units as selected by the GRID

command. The textual input method is necessary in particular for script files.

The coordinates of the current cursor position can be fetched with (@). For

example:

5+@,B

Examples of coordinate entry in text form:

You want to enter the outline of a circuit board with precise dimensions.

5 Principles for Working with EAGLE

577-

657+

0@00B@->00B@->0-00B@0-00B@00B

5

The first step is to switch to a 1 mm grid. The dimension layer is then

activated. The LINE command then first sets the line width to 0 and draws a

rectangle with the aid of the four given coordinates. The last command

returns the grid to whatever had previously been selected, since circuit

boards are usually designed using inches.

Relative values:

It is possible to use relative coordinate values in the form (R x y) which refer

to a reference point set with the MARK command before. If you don't set a

reference point the absolute origin of the coordinate system will be taken.

Setting a via relative to the reference point:

5770$9

74@.0-0B

:@9-.$9B

74

First the grid is set to Millimetres, then the reference point at the position

(20 10) is placed. The via is located at a distance of 5 mm in x and 12.5 mm in

y direction from the this point. Then the reference point is removed.

Polar values:

Polar coordinates are given in the form of (P radius angle).

577

74@-.$9A$-.9B

6.-

@00B@0;0B

5@;00B

5@;0-.0B

5@;0.;0B

This examples shows how to set the reference point at position (12.5 7.125).

Then a circle with a radius of 40 mm is drawn in layer 21, tPlace. Three pads

are placed on the circumference with an angle of 120°.

Here the circle is easily drawn with the help of relative coordinates. So we do

not have to worry about absolute values of a point on the circumference for

the second coordinates pair to determine the circle.

Right Mouse Click:

The > character within parenthesis represents a right mouse click. That way

one can move a whole group, for example:

7+:@?00B@-00B

The previously selected group will be moved 10 units in x direction.

Modifier:

Within parenthesis one can use some modifiers. For combinations you don't

have to care about the order:

5.2 The EAGLE Command Language

Arepresents the pressed Alt key, the alternative grid

Crepresents the pressed Ctrl key, Mac OS-X: Cmd

Srepresents the pressed Shift key

Rrelative coordinates

Ppolar coordinates

>right mouse click

C and S cause miscellaneous commands to behave in different manners.

More information can be found in the help function of the respective

command.

If the commands are being read from a script file, each one must be closed

with a semicolon. In the above cases the semicolons can be omitted if the

commands are being entered via the keyboard and each is being closed with

the Enter key.

Examples:

A component is to be transposed to a specified position.

577-

7+:-@-.0.9B

Alternatively you can use the object's coordinates:

7+:@0$-.A.$9;B@-.0.9B

IC1 is located at coordinates (0.127 2.54) and is moved to position (120 25).

The current position of a Device can be obtained with the aid of the INFO

command.

E+-

When a Symbol is defined, a pin is placed at a certain position.

C5C+*+-#0@0$.0$;B

You draw a rectangular forbidden area in layer 41 tRestrict:

6

@0$90$9B@.$9;B

5.3 Grids and the Current Units

EAGLE performs its internal calculations using a basic grid size of

0,00325 µm (about 0.000123 mil).

Microns (µm), mils (1/1000 inch), inches and mm can be chosen as a unit.

The current unit as set with the GRID command applies to all values.

You should always use the pre-set 0.1 inch grid for schematic

diagrams and for drawing Symbols in the Library Editor!

5 Principles for Working with EAGLE

When starting the design of circuit boards or libraries it pays to give prior

thought to the question of which grid size (or sizes) will be used as a basis.

For example, it is only the origin of a Package that will be pulled onto the

board's placement grid. All other objects constituting the Package (such as

pads) are placed relative to that point on the board, just as it was defined in

the library.

The basic rule for boards is: always make the grid as big as possible

and as small as necessary.

Various grid sizes can be pre-set in the eagle.scr file for different types of

editor windows (see page 104).

The current grid Size is set in the grid menu. The units chosen in the combo

box are used.

The Multiple option indicates how many grid lines are displayed. If, for

instance, the value 5 is entered at Multiple, every fifth line will be displayed.

The Alt line allows to set an alternative grid which can be activated by

pressing the Alt key (while, for example, MOVE, ROUTE, ADD, or LINE is

active). This can be very useful for placing parts in a dense layout or

arranging labels in the schematic. If you decide not to place it in the

alternative grid and release the Alt key before placing it, the object stays in its

origin grid.

Style specifies the way it is displayed: Lines or Dots. The options On and Off

under Display switch the grid display on or off. Finest sets the finest grid that

is possible. Clicking on default will select the editor's standard grid.

Beginning with a certain zooming limit, grid lines are not displayed anymore.

This limit can be set in the menu Options/Set/Misc, Min. visible grid size.

Grid lines and grid dots can have any color. Click the colored button of the

respective palette (depends on the background color) in the menu

Options/Set/Colors and select the color as requested. This can also be done

in the command line, for example:

++5

➢

The Grid menu

5.3 Grids and the Current Units

Instead of the color name the color number can be given, as well. It can be in

the range 0 .. 63. The shown color depends on the (self-)defined colors of the

current palette.

See also the hints concerning Color settings on page 107.

5.4 Aliases for DISPLAY, GRID, and WINDOW

For the commands DISPLAY, GRID, and WINDOW you can define so-called

aliases. This is a set of parameters which you can save with any name and

executed it with the command. To access such an alias simply click with the

right mouse button onto the command icon.

The aliases are stored in the eaglerc file for Schematic, Layout, and Library

separately. They are available for all Schematics, Layout, and Libraries then.

Example: DISPLAY Alias

Display the layers you want to see in the Layout Editor with the

DISPLAY command, for example Top, Pads, Vias, and Dimension

Right-click onto the DISPLAY icon and a popup menu appears

Select the New.. entry

Enter the name of the alias, for example Top_view

Click the OK button

From now on the popup menu of the DISPLAY icon contains the entry Top

view.

If you prefer the command line for activating this alias you have to enter:

DISPLAY TOP_VIEWordisp top_v

It does not matter if you write in upper or lower case letters hers. You may

use abbreviations as long as the name is clear.

There are no limitation to the number of aliases used.

Use DISPLAY LAST in the command line or the entry Last of the DISPLAY's

popup menu icon to return to the last layer selection.

More details can be found on the help page of the DISPLAY command.

Example: GRID Alias

The how to and the function of a grid alias is exactly the same as it is

explained for the DISPLAY command. Set the appropriate grid in one of the

Editor windows, right-click onto the GRID icon , and select the New..

entry in the popup menu to define the alias.

This can be done in the command line as well. for the grid command it could

look like this:

578==(0$009!="

The command

=8=or in short=8

5 Principles for Working with EAGLE

executes the alias. The command is case insensitive, the alias can be

abbreviated.

Example: WINDOW Alias

The WINDOW command allows you to define an alias for a certain part of

the drawing area. Aliases help you to navigate comfortably from one location

to another in your drawing. The definition of a WINDOW alias is similar to

the DISPLAY alias as described above:

Select the appropriate display window in the drawing

Right-click onto the Select icon of the WINDOW command to

open the popup menu

Click the New.. entry now and name your alias

Let's assume the alias name is upper_left: You can restore this display detail,

for example, in the command line with:

5+HHNor in short<=)HH!

Alternatively right-click onto the Select icon of the WINDOW command and

select the entry upper_left in the popup menu.

In a Schematic that consists of more than one sheet an alias is

executed always on the currently active sheet, independent of where

it was defined originally.

Editing, Renaming, Deleting of an Alias

In the case you want to delete an alias, you can do this in the command icon's

popup menu. First right-click onto the command icon to open the popup

menu. Then use a right mouse click onto the alias entry. This opens a context

menu. Click the Delete option there.

The same methods can be used to Rename or Edit an alias.

These actions can be executed also via the command line. Further

information can be found in the help pages about the DISPLAY, GRID, and

WINDOW commands.

➢

Deleting a WINDOW alias

5.5 Names and Automatic Naming

Length

Names in EAGLE can have any desired length. There is no limit.

Forbidden and Special Characters

No names may contain spaces, semicolons or umlauts. Quotation marks and

other exotic characters (above 127 in the ASCII table) should be avoided as

far as possible.

Device names must not contain either question marks or asterisks, since

these characters are used as placeholders for Package variants (?) and

technologies (*).

Commas must be avoided in pad names.

Part-bus names must not contain colons, commas or square brackets.

The exclamation mark is a special character that starts and ends a bar over

the text. See the help function for the TEXT command for details. If an

exclamation mark should be visible in the text, it needs to be escaped by a

leading backslash.

In order to have a backslash displayed in a name or text, you have to type it,

for example with the NAME or TEXT command, twice.

Automatic Naming

If a name is given together with one of the commands PIN, PAD, SMD, NET,

BUS or ADD, then other names will be derived from it as long as the

command is still active.

The name is simply typed into the command line before placing the object

(while it is attached to the mouse). Note that the name must be placed within

simple quotation marks. Entry is completed with the Enter key ( ) .←

The examples illustrate how automatic naming functions:

555-;C-C←• • •

fetches three DIL14 Packages to the board and names them U1, U2 and U3

(corresponds to a mouse click).

5+C-C←• • • •

places four octagonal pads with the names 1, 2, 3, and 4.

If the name consists of only one character from A...Z, then the following

objects receive the following letters of the alphabet as names:

555CC←• • • •

fetches four NAND gates with the names A, B, C and D. If the generated

name reaches Z, then names with the default prefix will again be generated

(e.g. G$1).

5.6 Import and Export of Data

EAGLE provides a number of tools for data exchange.

5 Principles for Working with EAGLE

Script files for importing

The export command for exporting

EAGLE User Language programs for import and export.

The User Language is very flexible, but does call for a suitable program to be

created. You will find further details in the section on The EAGLE User

Language.

Script Files and Data Import

The SCRIPT command makes a universal tool available to the EAGLE user

for data import.

Since every EAGLE operation can be carried out with the aid of text

commands, you can import all types of data with the aid of a script file. A

script file can in turn call other script files.

Script files can be created with a simple text editor. The prerequisite for the

development of your own script files is that you understand the EAGLE

command language. You will find the precise functioning and the syntax of

the individual commands in the EAGLE help pages.

The file euro.scr in the eagle/scr directory, which draws the outline of a

eurocard with corner limits, provides a simple example.

If a netlist is to be imported into a board design which already contains the

appropriate components, then a script file of the following form is necessary:

SIGNAL GND IC1 7 IC2 7 J4 22

SIGNAL VCC IC1 14 IC2 14 J4 1

A Netscript of this sort can easily be created from the schematic diagram by

the EXPORT command (menu File/Export/Netscript) and imported into the

layout.

You will get a further impression of the power of importing, if you output a

library with the EXPORT command into a script file (File/Export/Script).

The script file that is generated provides an instructive example for the

syntax of the script language. It can be examined with any text editor. If

SCRIPT is then used to read this file into an empty library, a new library file

will be created.

Comments can be included following a #-character.

The execution of a script file can be stopped by clicking the Stop icon in the

action toolbar.

The File/Import menu offers a P-CAD/Altium/Protel import option. Files

that are saved in the ACCEL-ASCII data format can be transferred into

EAGLE. Further information is displayed when you start this function.

File Export Using the EXPORT Command

The EXPORT command and the menu File/Export... offers, depending on

the active editor window, the following modes:

See also page 300.

Output in graphical formats.

Data output for component insertion machines, in-circuit testers etc.

Linking to an external database.

Manipulation of the silk screen print, the solder stop mask, and so on.

Import of graphic data files (for example import-bmp.ulp for logos or

the like)

A lot of valuable ULPs can be found on our web pages.

103

5 Principles for Working with EAGLE

5.8 Forward&Back Annotation

A schematic file and the associated board file are logically linked by

automatic Forward&Back Annotation. This ensures that the schematic and

the board are always consistent.

As soon as a layout is created with the BOARD command , the two files

are consistent. Every action performed on the schematic diagram is

simultaneously executed in the layout. If, for instance, you place a new

Device, the associated housing will appear on the layout at the edge of the

board. If a net is placed, the signal lines are simultaneously drawn in the

layout. Certain operations such as the placement or deletion of signals are

only allowed in the schematic. The Layout Editor does not permit these

actions, and issues an appropriate warning. Renaming Devices or changing

their values, for example, are permitted in both files.

The EAGLE help pages contain a closer description of the technical details.

It is not necessary for you, as the user, to pay any further attention to this

mechanism. You only have to ensure that you do not work on a schematic

whose associated board file has been closed, and vice versa. This means that

both files must always be loaded at the same time. Otherwise they loose

consistency, and the annotation can no longer work.

If you have, however, once edited the board or the schematic separately, the

Electrical Rule Check (ERC) will check the files for consistency when they are

loaded. If inconsistencies are found, the ERC opens an Error window with

appropriate messages about the Schematic and the Layout. Section 6.13,

starting with page 198, shows how to proceed in such a case.

5.9 Configuring EAGLE Individually

There are a number of settings that permit the program to be adjusted for

individual needs. We distinguish between program, user and project-specific

settings.

Basic program settings that will apply to every user and every new project are

made in the eagle.scr file. Under Windows, personal preferences are stored

in the file eaglerc.usr, or, under Linux, in ~/.eaglerc.

EAGLE remembers settings that only apply to one particular project in the

eagle.epf project file.

Values that, for instance, only apply to one specific board, such as the Design

Rules, special layer colors, unique newly defined layers or the grid setting are

stored directly in the layout file. This also applies, of course, to schematic

diagram and library files.

Configuration Commands

Most of the options are usually set by means of the Options menus of the

individual EAGLE editor windows.

104

5.9 Configuring EAGLE Individually

The Control Panel allows settings to be made for Directories, file Backup and

the appearance of the editor window (User interface). These options are

described in the chapter on the Control Panel under the

Options menu heading, starting on page 46.

Through the User interface settings it is possible to select the icon-based

menu or a configurable text menu.

The MENU command allows the text menu to be given a hierarchical

configuration by means of a script file. There is an example of this in the

appendix.

The Options menu in the editor windows for schematic diagrams, layouts

and libraries contains, in addition to the User interface item, two further

entries:

Assign and Set.

The ASSIGN command alters and displays the assignment of the function

keys. You will find information about this on page 89.

General system parameters are altered with the SET command.

The CHANGE command allows a variety of initial settings for object

properties.

The GRID command sets the grid size and the current unit. Further

information about this starts on page 95.

The Menu Options/Set (SET Command)

Most common options of the SET command are available in the Settings

window of the menu Options/Set. This window can be reached also by

entering on the command line:



Display Certain Layers Only

The number of available layers shown in the DISPLAY or LAYER menu can

be set with the option Used_Layers. That way it is possible to hide unused

layers for clarity reasons.

56-->-A-#-O.0.-.1.9.A.O1-;;;99-

stored in the file eagle.scr shows only the mentioned layers. After

56

all layers are available again.

Context Menu Entries

The right mouse button context menu can be extended by arbitrary entries

for different objects which are selectable with the mouse. This can be a

simple command, a sequence of commands, or maybe a script file or a User

Language Program you want to start. The syntax for the SET command looks

like this:

SET CONTEXT objecttype text commands;

105

5 Principles for Working with EAGLE

objecttype can be: attribute, circle, dimension, element, frame, gate,

hole, instance, junction, label, modinst, pad, pin, rectangle,

smd, text, via, wire

text is the menu text entry

commands is the command sequence, that is executed after clicking

onto the menu entry

Example:

SET CONTEXT wire Go_bottom 'change layer 16';

The context menu for wires (also polygons are member of object type wire)

has an additional entry named Go_bottom which changes the layer to 16

when clicking this entry.

In order to delete all self-defined entries in the context menu of a certain

objecttype, type:

+P<=

To achieve the default settings for all context menus:

+P

Contents of The Parameter Menus

The parameter menus for Width, Diameter, Dline (for dimensioning) Drill,

SMD, Size, Isolate, Spacing, and Miter, which are available, for example,

through the CHANGE command, can be configured and filled with any

values by the SET command. Simply list the values, separated by blanks, in

the command line.

Example for the Miter menu:

770$-0$.0$10$;0$90$>--$9.1;

The units of the given values are determined by the currently used GRID in

the Editor window. A maximum number of 16 entries is allowed.

Example for the SMD menu:

757-$..$00$90$O0$-=0$-;=

For each entry of the three value pairs the unit is given directly. A maximum

number of 16 value pairs is allowed.

The values in the menus are always shown in the currently selected GRID

unit.

Write the SET command in the file eagle.scr to make it default for all you

projects.

To return to the EAGLE default settings use for example for the Width menu:

5*7

ROUTE Command Settings

There are several option that can be used with the ROUTE command:

+7+54+5

is set by default. If you prefer the fully manual routing mode (as it was in

EAGLE version 7 and before) choose

+7+5+

106

5.9 Configuring EAGLE Individually

Loop Removal can be controlled by the SET command as well:

++7+:+++7+:+EE

If you prefer better visibility while routing, activate the Single Layer mode

that displays the current routing layer colored and all other layers in a

grayish color:

67+5+

Confirm Message Dialogs Automatically

Sometimes EAGLE prompts the user with a warning or informational

message and wants to know how to proceed. This may be unwanted for

automatic processes, for example, for executing a script file. You can decide

on how such a message shall be answered.

+E76

answers the question in the positive sense (Yes or OK).

In order to use the negative option (No button, if present, or simply confirms

the dialog) type

+E7+

To switch off automatic confirmation, use

+E7+EE

Please be careful with this option! Do not use it as a general option,

for example, in the beginning of a script file. This could lead to

unexpected results! See help of the SET command for details.

Color Settings

The Colors tab contains settings for layer and background colors and colors

for grid lines or dots.

Three color palettes are available: for black, white and colored background.

Each palette allows a maximum of 64 color entries, which can be given any

value for the Alpha channel and any RGB value.

107

➢

Settings window: Color settings

5 Principles for Working with EAGLE

If you prefer the old raster OP behaviour of previous EAGLE versions on

black background, deactivate the Use alpha blending check box. In this case

the alpha value is ignored when using a black background. Colors are mixed

now using an OR function.

By default EAGLE uses 64 values. Eight colors followed by further eight so-

called highlight colors.

The first entry of the palette determines the background color. In the white

palette, however, it is not possible to change the background color because

it's needed for print-outs, which normally are made on white paper.

The image above shows three buttons in the Palette column. Click on one of

them. For example, the button for Colored Background. The Color window

opens now.

On the left an 8 x 8 matrix is visible. There are alternating eight 'normal'

colors with their corresponding eight highlight colors. A color of the palette

at position x can be given the corresponding highlight color at position x+8.

In order to define new values select a box of the matrix and adjust the new

color with the help of the color selection area and the saturation bar on the

right. Click Set Color to apply your color. Now select a new color box in the

matrix and repeat the procedure for the next color.

You may also enter values for Red, Green, Blue or Hue, Sat, Val and Alpha

channel directly.

Alpha channel determines the transparency of the color. The value 0 means

the color is totally transparent (invisible), the maximum value 255 stands for

non-transparent. For printouts the value of the alpha channel is set to 255 for

each color.

In order to change the color palette for an editor window select the

appropriate Background in the menu Options/User Interface.

You should always define at least one pair of colors: a normal color

108

➢

Color window: Defining colors

5.9 Configuring EAGLE Individually

and its related highlight color.

Alternatively, the color definition and change of palette can be made in a

script file or in the command line.

Q=%?QαK?

defines a color for the currently used palette, where the value for the alpha

channel and the color value has to be given hexadecimal. Index stands for the

color number, αrgb for the values for alpha channel, the colors red, blue, and

green. Example:

->0%;EEEE0

sets the color number 16 to yellow, which corresponds to the decimal RGB

value 255 255 0 which is hexadecimal FF FF 00. The first byte B4

determines the value of the alpha channel (decimal 180).

Hexadecimal values are marked by a leading 0x.

To activate the black color palette type in the command line:

4

The new palette will become visible after refreshing the drawing area with

the WINDOW command.

The color assignment for layers is done with the DISPLAY command or with

SET COLOR_LAYER.

++6->;

defines, for example, the color number 4 for layer 16.

More details about the syntax can be found in the SET command's help.

If you prefer to use the default color values again, start the script file

defaultcolors.scr

Miscellaneous SET Options

The Misc tab of the Settings window contains the most common options,

which are switched on or off by check boxes. Some options allow entering

values.

sOptions overview:

109

5 Principles for Working with EAGLE

Beep:

Switches on/off the confirmation beep. Default: on.

Check connects:

Activates the package check while placing parts in the schematic.

Default: on.

Undo:

Switches on/off the undo/redo buffer of the current editor window. In case

you are working with a consistent schematic/layout pair, this setting is valid

for both editor windows. Default: on.

Optimizing:

Enables the automatic removal of bends in straight lines. Default: on.

Ratsnest processes polygons:

The contents of polygons will be calculated with the RATSNEST command.

Default: on.

Display pad names:

Pad names are displayed in the Layout or Package Editor. Default: off.

Display signal names on pads:

Signal names are displayed on pads in the Layout or Package Editor. Default:

on.

Display signal names on traces:

The traces in the layout show their signal names. Default: on.

Display via lengths:

The length of a via (start layer – end layer) will be displayed in the Layout

Editor. Default: off.

Display drills:

Pads/vias are shown with a drill hole or without it. Default: on.

110

➢

Settings at Options/Set/Misc

5.9 Configuring EAGLE Individually

Auto end net and bus:

If placing a net on a pin or a bus the net drops from the mouse cursor.

Default: on.

Auto set junction:

Ending a net on another net a junction will be set automatically.

Default: on.

Auto set route width and drill:

If this option is active, the Follow-me-Router uses the values for wire width

and via drill diameter given by the Design Rules or the net classes for the

tracks. These values will be set automatically as soon as you are clicking onto

a signal wire.

If this option is switched off, EAGLE will take the value you have set with, for

example, the previous CHANGE WIDTH command.

Group command default on:

If no command is active in the Layout editor, you can select a group as

default mouse action Default: off.

Min. visible text size:

Only texts with the given minimum size are displayed.

Default: 3 pixels.

Min. visible grid size:

Grid lines/dots which are closer than the given minimum distance are no

longer displayed on the screen. Default: 5 pixels.

Catch factor:

Within this radius a mouse click can reach objects. Set the value to 0 in order

to switch this limitation off. So you can reach even objects that are placed far

beyond the area of the currently displayed window. Default: 5% of the height

of the current display window.

Select factor:

Within this radius (given in % of the height of the current drawing window)

EAGLE offers objects for selection. Default: 2%.

Snap length:

Defines the radius of the magnetic-pads function of pads and SMDs.

If you are laying tracks with the ROUTE command and approach a pad or a

SMD beyond the given value – that is to say the dynamically calculated

airwire becomes shorter than the given radius – the wire will be snapped to

the pads/SMDs center. Default value: 20 mil.

All SET options can be used in the command line. Entering

+6++EEor, in short+6+EE

for instance, switches off polygon calculation for the RATSNEST command.

The help function offers additional instructions about the SET command.

The eagle.scr File

The script file eagle.scr is automatically executed when an editor window is

opened or when a new schematic diagram, board or library file is created,

unless a project file exists.

111

5 Principles for Working with EAGLE

It is first looked for in the current project directory. If no file of this name

exists there, it is looked for in the directory that is entered in the Script box

in the Options/Directories dialog.

This file can contain all those commands that are to be carried out whenever

an editor window (other than the Text Editor) is opened.

The SCH, BRD and LBR labels indicate those segments within the file which

are only to be executed if the Schematic, Layout or Library Editor window is

opened.

The DEV, SYM and PAC labels indicate those segments within the file which

are only to be executed if the Device, Symbol or Package editor mode is

activated.

Commands which are defined before the first label (normally BRD:) are valid

for all Editor windows.

If, because of the specifications in a project file, EAGLE opens one or more

editor windows when it starts, it is necessary to close these and to reopen

them so that the settings in eagle.scr are adopted. It is, as an alternative,

possible simply to read the file eagle.scr through the SCRIPT command.

Comments can be included in a script file by preceding them with #.

Example of an eagle.scr file:

R(=" !K)"& )&(=&<=<"$

""=DE1C=<;C

""=DE;C=<0$.9C

""=DEAC=C

""=DE#C==(C

7)C/"=!=J..$H2(S

!)"=!=J$)!H!I

(G)"=!=J$)!H

TC

BRD:

R7)(H85!&5="H!8=)H7M

RU)=&&)&=H&(<=!H!=&

R%&:!):==<CC==&=&

==(0$09

=!&=(0$0-

&"

&=&()0$00#0$0-0$0->

&5=!!)0$0.;0$01.0$0;0

&=F)0$090$0A0$-.

&"!8"-->-A-#-O.0.-...1.;.9.>

.A.#1O;0;-;.;1;;;9

(<=&(0$0-

(=!!0$0.;

("=F0$0A

SCH:

=5V)!&

(=&(0$00>

R7))"(H85!&5="H!8&"<H

R=)HMJW)GK!7M&

R="<HU)=&=H&(<H!=&:!)=<CC

R==&=&

LBR:

R7)!"%H&+H=H&=&CC=&

DEV:

=5V)!&

R7)(H8&5!&5="H!8%H&

112

5.9 Configuring EAGLE Individually

R=7MJ %U)=&=H&(<

R:!)=<CC=&=&

SYM:

5="H!8!!

=5V)!&+

(=&(0$0-0

R7)(H85!&5="H!8%H&

R=)H7M"&=U)=&=H&

R(<H!=&%&:!)=<CC==&=&

PAC:

=5V)!&+

=!&=(0$009

(=&(0$009

(=F0$090

(0$01O0$01O

R7)(H85!&5="H!8=)H

R7MU)=&=H&(<H!=&%&

R=<CC==&=&

The eaglerc File

Under Windows, user-specific data is stored in the file eaglerc.usr, or,

under Linux and Mac, in ~/.eaglerc. This file is stored in the user's home

directory. If there is no home environment variable set, the following

Windows registry entry is taken:

HKEY_CURRENT_USER\Software\Microsoft\Windows\Current-

Version\Explorer\Shell Folders\AppData

It contains information about the:

SET command (Options/Set menu)

ASSIGN command (function key assignments)

User Interface

Currently loaded project (path)

EAGLE looks for the configuration file in various locations in the given

sequence and executes them (if existing):

<prgdir>/eaglerc (Linux, Mac, Windows)

/etc/eaglerc (Linux , Mac)

$HOME/.eaglerc (Linux, Mac)

$HOME/eaglerc.usr (Windows)

These files should not be edited.

It is possible to start EAGLE with the command line option -U which can be

used to define the location of the eaglerc file. This can be useful in case you

are working with different EAGLE releases and want to keep things separate.

EAGLE Project File

If a new project is created (by clicking the right mouse button on an entry in

the Projects branch of the tree view and then selecting New/Project in the

context menu in the Control Panel), a directory is first created which has the

113

5 Principles for Working with EAGLE

name of the project. An eagle.epf configuration file is automatically created

in every project directory.

EAGLE takes note of changes to object properties that are made with the

CHANGE command during editing and the contents of the Width, Diameter,

and Size menus in the project file.

It also contains information about the libraries in use for this project.

The position and contents of the active windows at the time the program is

closed are also saved here. This assumes that the Automatically save project

file option under Options/Backup in the Control Panel is active. This state

will be recreated the next time the program starts.

114

Chapter 6

From Schematic to Finished Board

This chapter illustrates the usual route from drawing the schematic diagram

to the manually routed layout. One section explains the design of a

hierarchical schematic. Particular features of the Schematic or Layout Editor

will be explained at various points. The use of the Autorouter, the Follow-me

router, and the output of manufacturing data will be described in subsequent

chapters.

We recommend to create a project(folder) first. Details can be found

on page 43.

6.1 Creating the Schematic Diagram

The usual procedure is as follows:

Devices are taken from existing libraries and placed on the drawing area. The

connecting points (pins) on the Devices are then joined by nets (electrical

connections). Nets can have any name, and can be assigned to various

classes. Power supply voltages are generally connected automatically. In

order to document all the supply voltages in the schematic diagram it is

necessary to place at least one so-called supply symbol for each voltage.

Schematic diagrams can consist of a number of pages. Nets are connected

across all the pages if they have the same name.

It is assumed that libraries containing the required components are

available. The definition of libraries is described in its own chapter.

It is possible at any time to create a layout with the BOARD command or

with the Board icon. As soon as a layout exists, both files must always be

loaded at the same time. This is necessary for the association of the

schematic diagram and the board to function. There are further instructions

about this in the section on Forward&Back Annotation.

Open the Schematic Diagram

You first start from the Control Panel. From here you open a new or existing

schematic diagram, for instance by means of the File/Open or the File/New

menus, or with a double click on a schematic diagram file in the directory

tree. The schematic diagram editor appears.

115

6 From Schematic to Finished Board

Create more schematic sheets if needed. For that purpose, open the combo

box in the action toolbar with a mouse click, and select the New. A new sheet

will be generated (see page 53). Another way to get a second sheet is to type

EDIT .S2

on the command line. If, however, you do not in fact want the page, the

entire sheet is deleted with

7+:$.

A right mouse click onto the sheet preview opens a context menu. The

Description entry allows to write a descriptive text for the schematic sheet

which is displayed in the thumbnail preview and in the sheet combo box in

the action toolbar.

If you would like to have a description of the whole schematic visible in the

Control Panel's treeview use the Schematic description entry in the Edit

menu or type in the command line:

5+

Set the Grid

The grid of schematic diagrams should always be 0.1 inch, i.e. 2.54 mm.

Nets and Symbol connection points (pins) should lie on this common grid.

All symbols in the libraries are drawn in this grid.

Place Symbols

First you have to make available the libraries you want to take elements from

with the USE command. Only libraries which are in use will be recognized by

the ADD command and its search function. More information concerning the

USE command can be found on page 53.

Load Drawing Frame

It is helpful first to place a frame. The ADD command is used to select

Devices from the libraries.

When the ADD icon is clicked, the ADD dialog opens.

It shows all the libraries that are made available with the USE command,

first. You can expand the library entries for searching elements manually or

you can use the search function.

A letter format frame is to be used. Enter the search key letter in the Search

line at the lower left, and press the Enter key. The search result shows a

number of entries from frames.lbr. If you select one of the entries

(LETTER_P), a preview is shown on the right, provided the Preview option

is active. Disabling the options Pads/Smds/Description excludes parts with

Pads/Smds or the part's descriptive texts.

In the Schematic Editor you are searching for Device names and

terms of the Device description. In the Attributes line you are

searching for attribute names or values.

In the Layout Editor you can search for Package names and terms of

116

6.1 Creating the Schematic Diagram

the Package description!

Clicking OK closes the ADD window, and you return to the schematic

diagram editor. The frame is now hanging from the mouse, and it can be put

down. The bottom left hand corner of the frame is usually at the coordinate

origin (0 0).

Library names, Device names and terms from the Device description can be

used as search keys. Wildcards such as * or ? are allowed. A number of

search keys, separated by spaces, can be used.

➢ADD dialog: Results from the search key A4

The ADD command may also be entered via the command line or in script

files. The frame can also be placed using the command:

!XH,V"$!K

Wildcards like * and ? may also be used in the command line. The command

!X,V"$!K

for example opens the ADD windows and shows various frames in letter

format to select.

The search will only examine libraries that are in use. That means that the

library has been loaded by the USE command (Library/Use).

Drawing frames are defined with the FRAME command.

This can be done in a library, where the frame can be combined with

a document field. EAGLE can also use the FRAME command in the

Schematic as well as the Board Editor. Details about defining a

drawing frame can be found on page 279.

117

6 From Schematic to Finished Board

Place Circuit Symbols (Gates)

All further Devices are found and placed by means of the mechanism

described above. You decide a Package variant at this early stage. It can easily

be changed later if it should turn out that a different Package form is used in

the layout.

If you have placed a Device with ADD, and then want to return to the ADD

dialog in order to choose a new Device, press the Esc key or click the ADD

icon again.

Give the Devices names and values (NAME, VALUE).

If the text for the name or the value is located awkwardly, separate them

from the Device with SMASH, and then move them to whatever position you

prefer with MOVE. Clicking with DELETE on a text makes it invisible.

Use the Shift key with SMASH to get the texts at their original positions. The

texts are now no longer separated from the Device (unsmash). Deactivating

the Smashed option in the context menu's Properties window is the same.

MOVE relocates elements, and DELETE removes them. With INFO or

SHOW information about an element is displayed on the screen.

ROTATE turns gates by 90°. The same can be done with a right mouse click

while the MOVE command is active.

Multiple used parts may be copied with the COPY command. COPY places

always a new part even if it consists of several gates and not all of them are

already used.

A group of objects (components, nets...) can be reproduced in the schematic

diagram with the aid of the GROUP, COPY and PASTE commands. First

make sure that all the layers are made visible (DISPLAY ALL).

Hidden Supply Gates

Some Devices are defined in the libraries in such a way that the power supply

pins are not visible on the schematic diagram. Visibility is not necessary,

since all the power pins with the same name are automatically connected,

regardless of whether or not they are visible.

If you want to connect a net directly to one of the hidden pins, fetch the gate

into the schematic diagram with the aid of the INVOKE command. Click onto

the INVOKE icon, and then on the Device concerned, assuming that it is

located on the same sheet of the schematic diagram. If the gate is to be

placed on a different schematic diagram sheet, go to that sheet, activate

INVOKE, and type the name of the Device on the command line. Select the

desired Gate in the INVOKE window, then place it. Then join the supply gate

to the desired net.

118

6.1 Creating the Schematic Diagram

➢

INVOKE: Gate P is to be placed

Devices with Several Gates

Some Devices consist not of one but of several Gates. These can normally be

placed onto the schematic diagram one after another with the ADD

command. To place a certain Gate you can use the Gate name directly.

Example:

The Device 74*00 from the 74xx-eu library with Package variant N and in AC

technology consists of for NAND gates named A to D and one power gate

named P. If you want to place the Gate C first, use the Gate name with the

ADD command:

55C-CCCA;00,A;%%)$!K

See also help function for the ADD command.

As soon as one Gate has been placed, the next one is attached to the mouse

(Addlevel is Next). Place one Gate after another on the diagram. When all the

Gates in one Device have been used, the next Device is brought in.

If the Gates in one Device are distributed over several sheets, place them first

with ADD, change to the other sheet of the schematic diagram, and type, for

example

:+4-

on the command line. Select the desired Gate from the INVOKE window.

If you select one of the already placed Gate entries in the INVOKE

window, the OK button changes to Show. Click the Show button, and

the selected Gate is shown in the center of the current Schematic

Editor window.

Designlink – Access to Farnell's Online Product Database

With the help of designlink-order.ulp you can do a general product search or

a search for all parts of your schematic, check price and availability and order

directly at Farnell/Newark. Found order codes can be saved as part

attributes the schematic. The order list can be exported.

119

6 From Schematic to Finished Board

Click onto the designlink icon to begin. This icon is shown next to

the action toolbar. It is part of the text menu which can be switched on or off

through the Options/User Interface menu.

The General option starts a general product search. The ULP shows a

window where you can enter a search string. You will be connected to the

Farnell/Newark-Server directly, where the ULP searches for the given search

string, and finally displays the matches.

The Schematic option starts a search for all the parts used in your schematic.

The search term is the value of each component. As a result you will get a

parts list with Farnell/Newark order codes.

Some EAGLE libraries already contain attributes with information about

Farnell/Newark order codes. In case there is no order code available in the

library, or there is no match at the Farnell/Newark web site, the list will

mark the order code as unknown. Double-click onto this entry for starting a

manual search. As soon as all the components you would like to put into the

Farnell/Newark shopping cart have got an order code, click onto Add to

shopping cart.

The ULP comes with a detailed help which explains functionality and usage.

As an alternative you can start the ULP with the RUN command.

"=!=J/!2I/"H2

For updating libraries with Farnell/Newark order codes you can use

designlink-lbr.ulp. Start it in a Library Editor window and it loops through

all Devices searching for order codes at the Farnell/Newark web site. Finally

there will be created three attributes:

>MF for manufacturer, >MPN for manufacturer part number, >OC_FARNELL

or OC_NEWARK for the order code.

Wiring the Schematic Diagram

Draw Nets (NET)

The NET command defines the connections between the pins. Nets begin and

end at the connection points of a pin. This is visible when layer 93, Pins, is

displayed (DISPLAY command).

As soon as a net approaches a pin, a marker that indicates the pin connection

point is shown; even if layer 93, Pins is not displayed. A left mouse-click

connects the net with the pin then.

Nets are always given an automatically generated name. This can be changed

by means of the NAME command. Nets with the same name are connected to

one another, regardless of whether or not they appear continuous on the

drawing. This applies even when they appear on different sheets.

If a net is taken to another net, a bus, or a pin connecting point, the net line

ends there and is connected. If no connection is made when the net is placed,

the net line continues to be attached to the mouse. This behaviour can be

changed through the Options/Set/Misc menu (using the Auto end net and

bus option). If this option is deactivated, a double click is needed to end a

net. Nets are shown on layer 91, Nets.

120

6.1 Creating the Schematic Diagram

Nets must end exactly at a pin connecting point in order to be joined.

EAGLE will inform you about the resulting net name or offer a selection of

possible names if you are connecting different nets.

The JUNCTION command is used to mark connections on nets that cross

one another. Junctions are placed by default. This option, (Auto set

junction), can also be deactivated through the Options/Set/Misc menu.

Nets must be drawn with the NET command, not with the LINE command.

Do not copy net lines with the COPY command. If you do this, the new net

lines won't get new net names. This could result in unwanted connections.

If the MOVE command is used to move a net over another net, or over a pin,

no electrical connection is created.

To check this, you can click the net with the SHOW command. All the

connected pins and nets will be highlighted. If a Gate is moved, the nets

connected to it will be dragged along.

A simple identifier (without XREF option, see next section about Cross

References) can be placed on a net with the LABEL command. Provided you

have defined a finer alternative grid, labels can be arranged comfortably in

the finer grid with the Alt key pressed.

Defining Cross-References for Nets

If you place a LABEL with active XREF option for a net, a cross-reference will

be shown automatically. It points to the next sheet where the net occurs

again. Depending on the rotation of the label the cross-reference refers to a

previous or a following schematic sheet. If the label itself goes towards the

right or bottom border of the drawing, the cross-reference shows the next

higher page number. If the label points to the left or top border, the previous

pages are taken into consideration. In the case that the net is only available

on one sheet, this cross reference is shown, independently from the rotation

of the label.

If the net is only on the current sheet, only the net name and possibly the

label's frame around it is shown. This depends on the Xref label format

definition which can be done in the menu Options/Set/Misc (can be defined

via SET, too).

The XREF option can be activated in the parameter toolbar of the LABEL

command or after placing the label with CHANGE XREF ON.

The following placeholders for defining the label format are allowed:

YEenables drawing a flag border around the label

Ythe name of the net

Ythe next sheet number

Ythe column on the next sheet

Ythe row on the next sheet

The default format string is %F%N/%S.%C%R. Apart from the defined

placeholders you can also use any other ASCII characters. If %C or %R is used

and there is no frame on that sheet, they will display a question mark '?'. See

also page 279.

121

6 From Schematic to Finished Board

The lower label in the picture points to the right and refers to the net ABC on

the next page 3, field 4A, the upper XREF label points to the left (beginning

with the origin point) and refers to the previous page 1, field 2D.

If a XREF label is placed on a net line directly, it will be moved together with

the net.

More information about cross-references can be found in the help function

for the LABEL command.

Cross-References for Contacts

In case you are drawing an Electrical Schematic and using, for example,

electro-mechanical relays, EAGLE can display a contact cross-reference. In

order to do that, place the text >CONTACT_XREF inside the Schematic's

drawing frame. This text is not displayed in the drawing (excepted its origin

cross), but its position (the y coordinate) determines from where on the

contact cross-reference will be drawn on the current sheet. As soon as this

text is placed the contact cross-reference will be displayed.

The format of the contact cross-references can be defined - as for net cross-

references – in the Options/Set/Misc menu. It uses the same format

variables as described in the previous section Defining cross-references for

nets. The default setting is: /%S.%C%R, which

means /Pagenumber.ColumnRow.

The variables %C for column and %R for row can only work with a drawing

frame that was defined with the FRAME command and comes with a

column/row graduation.

For a proper display of the contact cross-references in the Schematic the

elements have to be defined in the Library Editor according to certain rules.

More information about this can be found in the help function under Contact

cross-reference and in the chapter about Libraries and Component Design

later in this manual.

122

➢

Cross-reference with a XREF

label

6.1 Creating the Schematic Diagram

Specifying Net Classes

The CLASS command specifies a net class (Edit/Net classes menu). The net

class specifies the minimum track width, the minimum clearance to keep

away from other signals and the minimum hole diameter for vias in the

layout. Each net primarily belongs to net class 0. By default all values are set

to 0 for this net class, which means that the values given in the Design Rules

are valid. You can use up to 16 net classes. Creating a net class can be

cancelled with the UNDO command.

➢

Net classes: Parameter settings

123

➢

Electrical Schematic with contact cross-reference

6 From Schematic to Finished Board

The image shows three additional net classes defined:

All nets that belong to class 0, default, will be checked by the settings of the

Design Rules.

Net class number 1, for example, has got the name Power and defines a

minimum track width of 40 mil.

The minimum drill diameter for vias of this class is set to 24 mil.

The clearance between tracks of net class 1 and tracks that belong to other

net classes is also set to 24 mil.

The left column Nr pre-defines the net class of the next net that is drawn

with the NET command. This selection can be made in the parameter toolbar

of the NET command, as well.

If you would like to define special clearance values between certain net

classes, click the button marked with >>. The Clearance Matrix opens. Enter

your values here.

➢

Net classes: The Clearance Matrix

To return to the simple view, click the << button. This is only possible,

however, if there are no values defined in the matrix. The net classes can be

changed later by means of the CHANGE command (the Class option) in the

Schematic and in the Layout Editor.

Net class definition can be done in the Layout Editor, as well.

A net class can be assigned to a single net/signal (left mouse click) or to a

number of nets/signals (Ctrl + right mouse click) that have been selected

with the GROUP command before.

Drawing a bus (BUS)

Buses receive names which determine which signals they include. A bus is a

drawing object. It does not create any electrical connections. These are

always created by means of the nets and their names. The associated menu

function is a special feature of a bus. A menu opens if you click onto the bus

with NET. The contents of the menu are determined by the bus name.

The bus in the diagram is named Bus1:A[0..12],D[0..7],Clock.

124

6.1 Creating the Schematic Diagram

Clicking on the bus line while the NET command is active, opens the menu as

illustrated above. The name of the net that is to be placed is selected from

here.

➢

Bus menu

The index of a partial bus name may run from 0 to 511.

The help function gives further information about the BUS command.

Pinswap and Gateswap

Pins or Gates that have the same Swaplevel can be exchanged with one

another. These properties are specified either when the Symbol is defined

(Pinswap) or when the Device is created (Gateswap).

Provided the Swaplevel of two pins is the same, they can be exchanged for

one another. Display layer 93, Pins, in order to make the Swaplevel of the

pins visible.

Pins or Gates may not be swapped if the Swaplevel = 0.

➢

Swaplevel: Pins layer is

visible

Input pins 1 and 2 have Swaplevel 1, so they can be exchanged with one

another. The output pin, 3, which has Swaplevel 0, cannot be exchanged.

You can find the Swaplevel of a Gate by means of the INFO command, for

example, type in the command line INFO IC2A. Alternatively via the context

menu, Properties entry.

125

6 From Schematic to Finished Board

Power Supply

Pins defined as having the direction Pwr are automatically wired up. This is

true, even if the associated power gate has not explicitly been fetched into the

schematic. The name of the Pwr pin determines the name of the voltage line.

This is already fixed by the definition of the Symbols in the library.

If nets are connected to a Device's Pwr pins, then these pins are not

automatically wired. They are joined instead to the connected net.

For every Pwr-pin there must be at least one pin with the same name but the

direction Sup (a supply pin). There must be one on every sheet. These Sup

pins are fetched into the schematic in the form of power supply symbols, and

are defined as Devices in a library (see supply*.lbr). These Devices do not

have a Package, since they do not represent components. They are used to

represent the supply voltages in the schematic diagram, as is required by the

Electrical Rule Check (ERC) for the purposes of its logical checks.

Various supply voltages, such as 0 V or GND, which are to have the same

potential (GND, let's say), can be connected by adding the corresponding

supply symbols and connecting them with a net. This net is then given the

name of that potential (e.g. GND).

➢

Supply symbols

If you place a supply pin (direction Sup) onto a net (with ADD or MOVE),

you will be asked for a new net name. Should it be the name of the supply pin

or should the net name remain unchanged?

Click Yes (default) for renaming the net with the name of the supply pin (in

the image above: AGND). Click No to preserve the current net name (VA1).

If the net has an automatically generated name, like N$1, you may suppress

this warning message. Use the SET command in the command line:

=$)HH!8=)&+M<=&&&-

If the last supply pin of a net is deleted, the net will get an automatically

generated name, like N$1.

126

➢

Supply pin name as new net name?

6.1 Creating the Schematic Diagram

If there is no supply pin in the supply libraries that fits to your

voltage in the schematic, you have to define a new supply pin!

Renaming an already existing supply pin is the wrong way and can

lead to unexpected results!

Define Attributes

Global Attributes

It is possible to define Global Attributes in the Schematic, for example, for

the author or a project identification number, that can be placed anywhere in

the schematic, often used in the docfield of the drawing frame.

Open the dialog through the Edit/Global Attributes... menu. Click the button

New to define a new Global Attribute. It consists of the attribute's name and

its value.

If you want to make a global attribute visible in the schematic, write a

placeholder with the TEXT command. For the AUTHOR attribute, write the

text >author.

It does not matter, if it is written in lower or upper case letters. The

> character in front of the text indicates that this is special text.

It is possible to define the placeholder text already in the Library, for

example, in a Symbol of a drawing frame. In this case the global attribute will

be shown on each schematic sheet containing this frame.

Global Attributes can be defined in the Schematic and Layout

separately.

More information on this can be found in the ATTRIBUTE command's help.

Attributes for Elements

The ATTRIBUTE command allows you to define attributes for Devices. An

attribute consists of the attribute name and its value that may provide any

information. If there already exists an attribute that has been defined in the

library, you may alter the value in the schematic.

127

➢

Global Attributes: The Author attribute is created

6 From Schematic to Finished Board

Clicking the ATTRIBUTE icon and then onto a Device opens a dialog

window. It lists the part's attributes already defined in the schematic or in

the library.

The image above shows the attributes DISTRIBUTOR, ID-NUMBER, and

TEMP for part R1. The icons on the right indicate where the attribute comes

form:

globally in the Schematic

globally in the Layout

in the Library's Device Editor

for the element in the Schematic

for the Package in the Layout

Attributes that are defined in the Layout Editor are not shown in the

Schematic Editor. A newly defined attribute in the Schematic adopts

the value of an already existing attribute in the Layout.

Defining a New Attribute

Click onto the New button to define a new attribute in the schematic. In the

following dialog you can define Name, Value, and the Display mode.

128

➢

Attribute dialog

➢

Create and change attributes

6.1 Creating the Schematic Diagram

In this image the attribute's name is TOLERANCE, its value is 1%.

With the Display option you manage the way the attribute is displayed in the

drawing. There are four options available:

Off: The attribute is not visible

Value:

Only the attribute's value is visible (1%)

Name:

Only the attribute's name is visible (TOLERANCE)

Both: Name and value are visible (TOLERANCE = 1%)

If the Display option is not set Off, the respective text will be displayed at the

Device's or Gate's origin. The layer which is preset in the Schematic, for

example with CHANGE LAYER before creating the attribute, determines the

text's layer. Location and layer can be changed any time.

If there is an already defined placeholder text for an element in the library,

the text shows up at the given location. It is possible to unfix such texts with

the SMASH command. Now you can move it, change its layer, the font, its

size and so on.

Changing an Attribute's Value

Values of attributes that are already defined in the library can be changed in

the Schematic Editor. After changing an attribute's value, the attributes

dialog displays special icons that indicate the attribute's status. The icons

have the following meaning:

the yellow icon indicates that the attribute initially was defined

with a variable value and that the value has been changed.

the red icon indicates that the value of the attribute which was

initially defined as constant has been changed after a confirmation

prompt.

the plain brown icon indicates that a global attribute was

overwritten by a part attribute. The value, however, remained

unchanged.

the brown icon with the unequal sign indicates that a global

attribute was overwritten by a part attribute and the value has

been changed.

➢

Attribute dialog with different attributes

129

6 From Schematic to Finished Board

Grayed text in the Attributes' dialog indicates that it can't be changed or

rather the element's attribute value was defined as constant in the library.

The icons inform you about the attribute's origin and its current status. Move

the mouse cursor onto one of the icons to let EAGLE display tool tip texts to

explain its meaning, provided the Bubble help in Options/User interface is

active.

More details on defining attributes can be found in the library chapter

beginning with page 271.

ERC – Check and Correct Schematic

A schematic diagram must be checked with the aid of the Electrical Rule

Check (ERC), when the design of the schematic diagram has been completed,

if not before. It is actually a good idea to run the (ERC) many times during

your design process to catch errors immediately. To start the Electrical Rule

Check click onto the ERC icon in the command menu or the entry Erc...

in the Tools menu.

All the errors and warnings are listed in the ERC Error window. Errors are

marked with a red icon, warnings with a yellow icon.

In the case of a corresponding board file, the ERC also checks the consistency

between schematic and board. If there are no differences, ERC reports Board

and schematic are consistent. Otherwise the ERC Errors window contains a

branch with Consistency errors. For further information on this see page

198.

130

➢

The ERC Errors window

6.1 Creating the Schematic Diagram

It is possible to sort the errors and warnings, ascending or descending, by

error types or sheet numbers. click onto the column headers Type or Sheet

therefore.

If you select an entry in the Errors or Warnings branch, a line points to the

corresponding location in the schematic diagram. In case you zoomed into

the drawing, you can click the option Centered. The currently selected error

is shown in the middle of the drawing window now.

Please check each error and every warning.

In some situations it may be the case that you want to tolerate an error or a

warning. Use the Approve button for this. The error/warning entry will be

removed from the Errors or Warnings branch and appears in the Approved

branch.

If you want to have the capability of displaying an approved error/warning

occurrence in the Errors or Warnings branch, expand the Approved branch,

select the error entry and click the Disapprove button. Now it is treated as a

normal error/warning and is marked in the schematic.

An approved error/warning retains its approved status as long as you do not

disapprove it by clicking the Disapprove button. Even a new ERC won't

change this status.

If the Errors window lists approved errors or warnings only, it won't open

automatically after running the Electrical Rule Check again. The status line

of the Schematic Editor, however, will show the following hint:

ERC: 2 approved errors/warnings

Moving an entry from one branch into the other, marks the schematic file as

changed and not saved.

While correcting the error on the board, the ERC Errors window may remain

open. After correcting one error or warning you can mark the entry as

Processed in the error list by clicking onto the Processed button. The

error/warning icon turns gray now. Entries marked as processed will be

remembered as long as you don't start ERC again. Re-opening the ERC

Errors window with the ERRORS command, shows the same status as

you left it at last.

If you click onto the Clear all button, the Errors and Warnings branches will

be cleared. Approved errors and warnings, however, will remain in the

Approved branch. The message List was cleared by user is shown then.

If you did not run an ERC before, the ERRORS command will start it

automatically before opening the errors window.

The ERC checks the schematic diagram according to a rigid set of

rules. It can sometimes happen that an error message or warning

can be tolerated.

If necessary, make an output of net and pin lists with the EXPORT

command.

131

6 From Schematic to Finished Board

SHOW allows nets to be traced in the schematic diagram.

Organize Schematic Sheets

If your schematic is a bit more complex or you want to use more than one

sheet, for example, for better readability, you can add (and also remove)

sheets with the help of the sheet thumbnails' context menu. Click with the

right mouse button onto one of the thumbnails that are located on the left

side of the Schematic Editor window.

A new sheet is always added as the last one.

The schematic sheets can be sorted by dragging and dropping the

thumbnails. Therefore click with the left mouse button on a thumbnail and

drag it to its new position.

Alternatively you can sort the sheets with the EDIT command in the

command line:

5$"9$".

moves sheet number 5 at the position before sheet number 2. Further

information about this can be found in the EDIT command's help function.

Go to the Options/User interface menu in order to switch on/off the sheet

preview.

When switching between schematic sheets, the current zoom level of

each sheet will be maintained.

Points to Note for the Schematic Editor

Superimposed Pins

Pins will be connected if the connection point of an unconnected pin is placed

onto the connection point of another pin. Pins will not be connected if you

place a pin that is already connected to a net line onto another pin.

Open Pins when MOVEing

If a Gate is moved then its open pins will be connected to any nets or other

pins which may be present at its new location. Use UNDO if this has

happened unintentionally.

Duplicating a Section of the Schematic

If you want to use a certain section of your schematic several times, you can

use GROUP and COPY commands in order to put this part into the

clipboard, and then use PASTE to place the group on the same or on a

different sheet of your schematic.

The duplicated components will get new names. Nets connected to a supply

pin or marked with a LABEL will keep their original name, provided the

supply pin and the label is part of the selected group. All other nets will get

new names.

132

6.1 Creating the Schematic Diagram

With Consistent Layout

In case you already created a board from your schematic, the pasted

components in the layout will be placed left of the board's origin. As usual the

components have to be arranged and the airwires routed then.

Merge Different Schematic Files

It is possible to paste a whole schematic file into the current drawing. This

can be done in the menu File/Import/EAGLE drawing.... The new sheet(s)

will be appended to the current one(s), depending on the number of sheets of

the source schematic. You can re-order the sheets by drag&drop afterwards.

While inserting a group EAGLE checks the objects' names and compares

them with those already existing in the current schematic. EAGLE will show

a window where you get information about the net names. The table shows a

list with the original names of the schematic you want to paste, in the column

Old name, and the net names, in the column New name, EAGLE suggests for

this schematic after pasting it into the current drawing. By clicking onto an

entry you can influence the net names and decide about them by yourself.

Names of nets that have a label or are connected to a supply pin, will remain

unchanged by default. In the Paste... list such nets are marked with icons

that want to tell you what's the reason for leaving this net name unchanged.

Of course you are allowed to change such a net name as well.

It is not allowed to change the names of nets that are member of a bus or that

are connected to an implicit power here.

It's possible to pre-define an offset for the enumeration of the components, if

you use the PASTE command in the command line:

.00(!-$"(

133

➢

Netnames before and after pasting the

schematic

6 From Schematic to Finished Board

adds the schematic with name channel1.sch into the drawing and increments

the components' names with an offset of 200. R1 of channel1.sch will be

named R201 in the current drawing then.

This function is also available through the File/Import... menu.

With Consistent Layout

In case you are working with a consistent pair of schematic and board files,

and you want to import another consistent schematic/board pair into your

current project via the File/Import/EAGLE drawing... menu, the schematic

will be placed on a new sheet (or several sheets) and the board will be placed

left of the already existing layout. It can be moved with GROUP and MOVE

afterwards.

As an alternative to the File/Import menu and the PASTE command which

can be used in the command line, you are allowed to drag&drop a schematic

or a layout from the treeview's projects branch of the Control Panel into your

currently opened Schematic or Layout Editor window.

Multi-Channel Devices

This functionality can be used to easily create multi-channel devices:

Finish the schematic of one channel and create the board of it. Then arrange

the components and route your layout. When this is done use Paste from....

and copy the schematic/layout pair as often as needed into on common

schematic/board file pair.

If you start File/Import/EAGLE drawing... in the Layout Editor, the layout

will be attached to the mouse cursor and you can place it where you would

like to have it. The schematic part will be added on a new page in the current

schematic. If you are using the command line in the Layout Editor you can

use coordinates for an exact placement.

$5@-010B

for example, places the board from test.brd with an offset of (10 30) in grid

units compared to the original position.

In case you start the import from the Schematic Editor, the referring layout

will be placed automatically left of the already existing design in the layout

editor.

Design Blocks

A Design Block (*.dbl) may contain a schematic or a board, or ideally both. If

there is only a Schematic editor open, it will paste the schematic part of the

Design Block only, accordingly for boards. To paste both, a consistent

schematic/board pair has to be loaded.

In its tree view the Control Panel shows a branch with Design Blocks

available. Clicking onto one of these entries displays a preview of the Design

Block. Double-clicking an entry pops up the Modify Design Block window.

Here you can modify the Description, create, delete or change attributes, or

enter the Design Block editing mode by clicking the Edit.. button. Then a

Design Block Schematic or a Design Block Layout Editor window appears. It

looks the same as a Schematic or Layout Editor window, with the exception

of the text in the title bar.

134

6.1 Creating the Schematic Diagram

Adding Design Blocks into Your Current Design

For inserting Design Blocks Schematic and Layout Editor have a “PASTE

DBL” icon . Alternatively you can insert it from the Control Panel. Right-

click on one of the entries in the Tree View’s Design Block branch and choose

the Add to schematic/board option.

If the PASTE DBL command is started from Layout Editor, it has the same

behaviour like pasting from a drawing file. The board can be placed by mouse

click and new sheets are added to schematic.

If the command is started from the Schematic Editor and the Design Block

has only one sheet, it can be placed by mouse click into the current sheet, as

well. No new sheet will be created in that case.

Save a Drawing as a Design Block

With File/Save as Design Block… (WRITE DBL) a Design Block is generated

from the currently loaded schematic and/or board (depending, from which

editor executed and whether schematic and board are in consistent state)

and saved under the given name.

135

➢

Modify Design Block Properties

6 From Schematic to Finished Board

If no name is given, the Design Block dialog pops up (see image above). It

allows entering an HTML description and defining Attributes. In the upper

left there is a preview of the description. The description can be written in

the text field below.

Attributes can be managed with the buttons New, Change, and Delete at the

bottom left. There also can be automatically generated Attributes which are

not editable.

The preview on the right represents the drawing(s) to be included in the

Design Block. At the bottom you can enter the file name or select where to

store it.

Save a Selection of the Drawing as a Design Block

With the pulldown menu entry File/Save selection as Design Block it is

possible to select objects of the current schematic, board or of both, if it is a

consistent pair of files, and save it as a Design Block.

The selection works in additive mode and may be adjusted several times.

Deselection with Ctrl + left click is supported. The selection in the first Editor

window has to be finished with Ctrl + right click.

Please check the hints displayed in the status bar of the editor window.

There are a couple of criteria for the selection that will be checked (see

below). If these criteria are not met, an according error message is displayed

and the user may continue and correct the selection.

If there's only one editor window opened, the Design Block dialog pops up,

presenting the current selection in the preview. The selection can now be

saved.

If both editors are open, you can continue your selection after the Ctrl +

right click in the second editor. The initially selected corresponding objects

are already selected due to the back/forward annotation (for example

element R1 in the layout, if part instance R1 in the schematic has been

selected first). In the second editor window additional objects can be added

to the selection, as long as they do not severe consistency. Selection or

deselection of any object that might severe consistency are automatically

filtered out.

For example, objects without electrical relevance like texts, dimensions etc.

are allowed to be selected. Routed traces or signal polygons can be added or

removed from the selection, if the corresponding nets were already selected

in the previous editor window. The selection process is completed with a

further Ctrl + right click. The Design Block dialog shows up now. The whole

selection is visible in the preview area and can be saved as a Design Block for

future reuse.

The combined selection is only possible, if a consistent schematic/board pair

is loaded. It works in both directions.

The selection is not yet supported within hierarchical schematics.

136

6.1 Creating the Schematic Diagram

Selection criteria

If the schematic has multiple sheets and the selection is started from a

board, only objects with counterparts on the currently active sheet are

supported.

If the selection is started from a schematic, it is checked that the user

selects net segments completely, in particular not leaving behind

some net wires or labels.

For each part all of its instances must be selected.

With a net segment being selected, all connected part instances

connected to this segment must be selected.

6.2 The Hierarchical Schematic

A hierarchical diagram differs from the schematic generated in section 6.1 in

its structure. It contains subordinate units, so-called modules, each

representing a part of the entire circuit diagram.

Modules can be edited just the same like a simple Schematic. Modules can be

drawn across multiple module pages. The sheets of the modules are

displayed in the icon preview of the Schematic Editor window; just like

normal, schematic sheets.

Modules are usually represented by module instances that are drawn as

simply symbols (boxes) at schematic main level. Module instances of one and

the same module can be used repeatedly.

For the module instances ports are defined, which serve as an interface

between the nets inside the module and a higher schematic level. Ports are

used, for example, to connect various module instances or to establish

connections between nets inside a module and nets on schematic main level.

Ports can export not only individual nets, it is also possible to export simple

buses via a port.

The hierarchical schematic can have any number of levels. This allows to use

a module instance of another module inside a module, and so on. The depth

of the hierarchy can be arbitrarily deep.

If a layout is generated from a hierarchical schematic, the result is

comparable with the layout of a schematic without hierarchy.

Creating a Module

Click onto the MODULE icon to create a module. The Module Dialog

opens. Type in the line New: the name of the module, for example FILTER.

The module will be created. Attached to the mouse cursor, you already see

the module instance of the module FILTER which can be placed on the first

page of the schematic. If you cancel the command before you place the

module instance, the module is nevertheless already created. You can see it

in the sheet preview: There is module sheet named FILTER:1 (Module

FILTER, Module sheet 1) displayed.

137

6 From Schematic to Finished Board

If you want to create multiple modules without placing a module instance,

use the command line:

7+5E

7+57

7+5+6

Each command creates after your confirmation a new module. For the

POWERSUPPLY module there is already defined the prefix PS for the

module instances. They are finally named PS1, PS2, and so on.

The hierarchical schematic may contain any number of modules.

The picture shows a newly created module with name FILTER. The module

sheet is still empty. There are no components and nets drawn.

The corresponding module instance has already been placed on the

schematic page and has the name FILTER1.

Module instances and their ports are automatically drawn in layer 90

Modules.

In the next step, you define the contents of the module. Switch to the module

sheet by clicking on the sheet preview or in the action bar on the sheet

selection box. Now draw the module as in the normal schematic, just as in

the previous section Creating the Schematic Diagram beginning with page

115 described.

A module can be drawn over several sheets. In order to create a new module

sheet, click on the module sheet preview with the right mouse button. Select

the appropriate option in the context menu.

138

➢

Module Instance for Module Filter (yet without ports and

contents)

6.2 The Hierarchical Schematic

In the context menu of the module sheet you can create a new additional

module sheet, remove a module sheet, or completely remove a whole module

with all its module instances from the schematic (Remove Module).

The description of a module can be formatted with HTML tags. The first line

of the description will be displayed in addition to the module name in the

module sheet preview and in the Sheet combo box.

In Properties, you have the option to define a prefix and the size of the

symbol of the module instance that represents the module in the schematic.

Prefix defines the name of the module instances, as it is with the prefix for a

device in a library. If you choose for a module named Power_Amplifier, for

example, as a prefix PA, the name of the first module instance will be PA1,

the second PA2, and so on. If there is no prefix defined, the module name +

number will be used.

In addition, you can see the list of ports that connects the module with its

environment.

The order of the module sheets can be changed by drag&drop in the preview.

It is also possible to move a schematic sheet from main level into a module.

The result is a corresponding module sheet.

You can also move sheets out of a module into main schematic level. But

please keep in mind that this can have a significant impact on your design

under certain circumstances. If you have already started to create the layout,

such an action may have a significant impact on it.

Organizing the sheets of the module can also be done via the command line

using the EDIT command (see help).

139

➢

Context menu of module sheet Filter:1

6 From Schematic to Finished Board

Define Ports

A Port serves as an interface for the nets within a module and the world

outside. In the main level schematic ports can be connected to nets that

connect different module instances or components that are not member of a

module (i.e. in the main schematic level).

Click on the PORT icon and then click the module instance for the port to

be created. The first port is attached to the mouse cursor. It can be moved

along the module instance's contour. The parameter toolbar of the PORT

command shows a combo box that offers different port directions.

The Direction describes the logical direction of signal flow. There are the

following options:

NC not connected

In input

Out output (totem-pole)

IO in/out, bidirectional (default)

OC open collector or open drain

Hiz high impedance(3-State) output

Pas passive

Pwr power pin (Vcc, Gnd, Vss ...), supply voltage input

The direction is shown at the ports by corresponding arrows.

After choosing the direction place the port with a left mouse click. This opens

a selection window from which you select the module net, which should be

connected via the port to outside the module. If there is yet no corresponding

net present in the module, you can define a New name, as well. This net has

to be created in the module then!

In the Select windows can also appear module buses. A port can even handle

simple buses, for example PA[0..7]. The nets PA0...PA7 will be exported

through this “bus port”. The bus port will be drawn with a wider line width.

Click OK to confirm the selection. The next port is attached to mouse cursor

now and can be placed as described at the contour of the module instance. If

all ports are placed, terminate the PORT command with Esc or click onto

another module instance for further placement of ports.

140

➢

Select the Module Net for the Port

6.2 The Hierarchical Schematic

The connection point of the port is displayed the same way as for pins of

components in layer 93, Pins.

Using Module Instances

Module instances are defined with the MODULE command. Click the

MODULE icon and select the module for which the module instance should

be created.

Place the module instance in the schematic.

A module instance can be moved as a whole, for example, with MOVE.

Do you want to move only one port to another location or change the

Direction or the name of the port, however, select the MOVE or INFO, hold

down the Ctrl key and click on the port.

141

➢

Module Instance with Ports; on the right: Properties Dialog

➢

Module Selection

6 From Schematic to Finished Board

A change to a module instance that is used multiple times in the hierarchical

schematic is transferred to all module instances.

If you would, for example, add a new port to the module instance Filter1 in

the image above, there would be added the same port to the module instance

Filter2 simultaneously.

A change in the size of the symbol of a module instance can be done via the

properties dialog or by Ctrl+MOVE on one of the borders of the box. The

change applies to all module instances of this module.

Resulting Component Names in the Layout

For components that are used in modules, special rules apply when

generating the component name. Each module has its own namespace.

ModulInstanceName:PartName

Supposed a component with the name C1 is used in the module FILTERS and

also used in a module named POWERSUPPLY.

If these modules are represented by two module instances in the schematic

(Filter1 and Powersupply1), the resulting component names on the board will

be composed of the module instance name followed by a ':' and the part

name. So in our example, the components will have the names Filter1:C1 and

Powersupply1:C1.

This is the default method used by EAGLE.

Offset

Optional you can specify an offset for module instances on schematic main

level. For example, the module instance Filter1 has defined an offset of 100

and the module instance Powersupply1an offset of 200, the resulting

component name on the board will be C101 instead of the previous Filter1:C1

and C201 instead Powersupply1:C1.

The offset can be defined only for module instances on main schematic level

and applies only to components. In case of components and nets in deeper

levels the module instance name is always prefixed.

The offset has to be a multiple of 100. It is specified in the properties dialog

of the module instance or directly with the MODULE command in the

command line. The syntax is described in the help of the MODULE

command.

Assembly Variants for Modules

Within modules, assembly variants can be defined. Edit a module sheet and

click onto the Assembly variants entry in the Edit menu of the Schematic

Editor. How to create assembly variants is described in section Creating

Assembly Variants beginning with page 192.

Module assembly variants are limited to the module parts. Module assembly

variants can be used via the module instance. For each module instance a

specific module assembly variant can be selected.

142

6.2 The Hierarchical Schematic

There is no direct switching between assembly variants in a module, but the

element's value, populate state and attributes in the board are set following

the chosen variant in the corresponding module instance.

If used on schematic main level, the VARIANT command works for the parts

on main level as it is in non-hierarchical schematics.

The assembly variant definitions are now kept only in the schematic.

For standalone boards, assembly variants are no longer supported, but it's

possible to set the populate option of elements with the CHANGE command

or in the properties dialog.

Special Features between Schematic and Layout

SHOW command

Show executed on a module instance displays all associated components and

signals in the layout generated by this module instance.

Click on a component in a module and EAGLE shows all components in the

board that are generated by the multiple use of a module – there are several

module instances that represent the same module in the schematic.

Consistency

To avoid inconsistencies between schematic and board regarding

components and nets and the corresponding signals in the hierarchical

design, some commands can not be executed in the Layout Editor.

This must therefore be done in the schematic and will be transferred to the

appropriate element or signal on the board then. These includes the

commands NAME and VALUE.

EAGLE prompts in such situations an appropriate message.

This restriction applies only to objects in a hierarchical structure, if there is

consistency.

6.3 Considerations Prior to Creating a Board

Checking the Component Libraries

The EAGLE component libraries are developed by practising engineers, and

correspond closely to present-day standards. The variety of components

available is, however, so wide that it is impossible to supply libraries which

are suitable for every user without modification.

There are even different Packages which are supplied by various

manufacturers using the same identification! Manufacturers recommend

very different sizes for SMD pads, and these depend again on the soldering

procedure being applied.

In short: You cannot get away without checking the components, in

particular the Package definitions, being used when laying out.

143

6 From Schematic to Finished Board

In the case of SMD components, please take particular care to ensure

that the Package from the library agrees with the specifications of

your component. Housings from different manufacturers with the

same name but different dimensions are often found.

Agreement with the Board Manufacturer

If you plan to have your PCB professionally manufactured, now is the time to

inquire at your board manufacturer whether they stipulate any particular

values for the following parameters:

track width

shape of solder lands

diameter of solder lands

dimensions of SMD pads

text size and thickness

drill hole diameters

number of signal layers

in case of multilayer boards: manufacturing directions for Blind and

Buried vias and composition of the board (see page 178)

clearance values between different potentials

parameters concerning solder stop mask and cream frame

You will save yourself time and money if you take these stipulations into

account in good time. You will find more details on this in the section on the

Preparing of Manufacturing Data (Chapter 9).

Specifying the Design Rules

All the parameters relevant to the board and its manufacture are specified in

the Design Rules.

Use the menu Edit/Design Rules.. to open the Design Rules window shown

below:

144

6.3 Considerations Prior to Creating a Board

➢

DRC: Adjusting the Design Rules

General Principles

The first time that you call this dialog, the Design Rules are provided by the

program. If necessary, adjust the values to suit your or your Board house's

requirements.

The Apply button stores the values that are currently set in the layout file.

Changes to various Design Rules, like the settings concerning the Restring,

are immediately displayed in the Layout Editor after clicking Apply.

The Design Rules can be saved in a special Design Rules file (*.dru) by the

use of the Save as.. button. So you can easily use this set of rules for another

board.

To apply a set of Design Rules to a board, you can drag any dru file of the

Design Rules branch of the tree view in the Control Panel into the Layout

Editor window or click the Load.. button in the File tab of the Design Rules

window.

Edit Description.. can be used to alter the descriptive text for the current

parameter set. The description usually appears in the File tab, as can be seen

in the image above. HTML text can be used. You will find notes on this in the

help system.

The Design Rules dialog offers a range of different options that can be

selected through the tabs. The options include:

File Manage the Design Rules

Layers Number of copper layers, structure of multilayer

boards, kind and length of vias, thickness of copper

and isolation layers

Clearance Distances between objects in the signal layers

representing signals that may be different or the same

145

6 From Schematic to Finished Board

Distance Distances from the board edge and between holes

Sizes Minimum track width and hole diameter, particularly

for Micro and Blind vias

Restring Width of the remaining ring at Pads and (Micro) vias

Shapes Shapes of Pads and SMDs

Supply Thermal symbols in copper plains

Mask Values for solder stop and solder cream masks

Misc Additional checks

Most parameters are explained with the help of a small image. As

soon as you click into a parameter line, the associated display

appears.

Layers

Define the number of signal layers and the kind of vias (Blind or Buried vias)

here. With the help of a mathematical expression in the Setup line the proper

structure of the board, the appropriate combination of cores and prepregs

and the resulting facilities for vias can be defined.

In most cases (for simple two or more layer boards) the vias are drilled

through all layers. The image above shows the default setup for a two layer

board. The expression (1*16) defines one core with layers 1 and 16, which

can be connected with vias. Parenthesis around the expression define

through-hole (continuous) vias.

Basic examples:

1 layer:

16 Only layer 16, no vias.

146

➢

Design Rules: Layer Setup

6.3 Considerations Prior to Creating a Board

4 layers, vias through all layers:

(1*2+15*16) Two cores are affiliated with each other.

6 layers, vias through all layers:

(1*2+3*14+15*16) Three cores are affiliated with each other.

The fields for Copper and Isolation are used to define the thickness of copper

and isolation layers. These settings are only relevant for complex multilayer

boards that use Blind or Micro vias.

The commands DISPLAY, LAYER, LINE, and ROUTE work only with those

signal layers defined in the Layer Setup.

Further information and examples about the Layer setup can be found in the

section Multilayer Boards beginning with page 178.

Loading a board file that was made with an older version causes

EAGLE to check which signal layers contain wires. These layers

appear in the layer setup. Please adjust it if necessary.

Minimum Clearance and Distance

Clearance refers to the minimum distances between tracks, pads, SMDs and

vias of different signals, and between SMDs, pads and vias of the same signal.

Setting the values for Same signal checks to 0, disables the respective check.

Distance allows settings to be made for the minimum distances between

objects in layer 20, Dimension, in which the board outline is usually drawn,

and between holes.

Setting the value for Copper/Dimension to 0 switches off the minimum

clearance check between copper and dimension.

In this case EAGLE does not recognize holes that are placed on wires.

Polygons don't keep their distance to objects in layer 20, Dimension,

either!

If a net belongs to a special net class, the values for Clearance and for the

drill diameter of vias (Drill), defined by means of the CLASS command, are

taken into consideration, provided these values are higher than those given

in the Design Rules (Clearance and Minimum Drill in the Sizes tab).

Sizes

The minimum values for track width and for hole diameter allowed in the

layout are selected here.

If additionally net classes are defined and values for clearance, width, or

minimum drill, are set, the respectively higher value is taken into

consideration.

Here you set the aspect ratio of drill depth to drill diameter for boards that

contain Blind vias. Please contact your board house for this information! If

the board house specifies, for example, an aspect ratio of 1:0.5 you have to

enter the value 0.5 in the line Min. Blind Via Ratio.

147

6 From Schematic to Finished Board

For micro vias you have to set the minimum drill diameter in the line Min.

MicroVia. Setting this value higher than the value in Minimum Drill means

that there are no micro vias used (default). To put this into other words: If

the drill diameter is between the value for Min. MicroVia and Minimum

Drill the via is considered a micro via.

Restring (Pad and Via Diameter)

The settings made under Restring determine the width of the ring remaining

at pads, vias, and micro vias. The remaining ring refers to the ring of copper

that remains around a hole after a pad or via has been drilled. Different

selections can be made for the width of the remaining ring in the inner and

outer layers. Pads may also differ between the Top and Bottom layers.

Usually the value is expressed as a percentage of the hole diameter.

Minimum and maximum values can additionally be specified.

As soon as you change a parameter and click the Apply button you can

directly see the effects in the layout. If you want to use different values for the

upper and lower layer (or different shapes, see Shapes tab), it is

recommended to set the layer color for layers 17, Pads, and 18, Vias, the

same as the background color (black or white). In this case you can recognize

the real size and shape of the pad/via in its respective layer.

The INFO command which has the same dialog as the context menu's

Properties entry, informs you about the via diameter in outer and inner

layers, and about the initial user-defined value. For example, in the following

image:

➢

Displaying Via properties with

INFO

Pre-defined value (by CHANGE DIAMETER): 0.7

Actual calculated diameter in the outer layers: 0.9

Actual calculated diameter in the inner layers: 0.8

148

6.3 Considerations Prior to Creating a Board

Here the resulting via diameter is bigger than the pre-defined value,

according to the given minimum value in the Design Rules' Restring settings

for vias.

The following image illustrates the template for setting the width of the

residual ring. The standard value for the restring around holes is 25 % of the

hole diameter. Since the width of the ring on small holes specified this way

would soon fall below a technically feasible value, a minimum value (here: 10

mil for pads, 8 mil for vias, 4 mil for micro vias) is specified here. It is also

possible to specify a maximum value.

Example:

The ring around a hole with 40 mil diameter is 10 mil (25 %). It therefore lies

in between the maximum and minimum values.

If the hole is only 24 mil in diameter (e.g. for a via), the calculation yields a

restring value of only 6 mil. For a board made in standard technology this is

extremely fine, and cannot easily be made. It might well involve extra costs.

In this case a minimum value of 10 mil is given.

If you like to define a restring with a fixed width, use the same value for

minimum and maximum. The value in percent has no effect in this case.

Diameter check box:

In case you defined a diameter for a pad in the library or for a via in the

Layout Editor, and you want to have this given diameter taken into

consideration for the inner layers, activate the Diameter option. This can be

of interest if a pre-defined pad or via diameter exceeds the value calculated

by the Design Rules. Otherwise the pad or via in the inner layers would be

smaller than in the outer layers. If you want pads/vias to have the same

diameter in all layers, set the option Diameter.

The option is set off, by default, for new created boards, but will be set on for

149

➢

Design Rules: Restring settings

6 From Schematic to Finished Board

boards that are updated from version 3.5 or prior because in these versions

pads and vias had the same diameter in all layers. Thus the update process

does not change the original layout.

All the values can also be given in Millimetres (for example 0.2mm).

Shapes

SMDs:

A rounding factor can be specified here for SMD pads. The value can be

between 0 % (no rounding) and 100 % (maximum rounding).

A square SMD has been placed instead of an oblong one on the far right of

the diagram. After assigning the property Roundness = 100 %, the SMD

becomes round.

Pads:

This is where the form of the pads is specified. It is possible to give different

settings for the top and bottom layers.

The As in library option adopts the form defined in the Package Editor.

Clicking on Apply shows the change immediately in the Layout Editor.

Pads and Vias within inner layers are always round, no matter what

they are in Top or Bottom layer. The diameter is determined by the

restring settings.

Provided a pad was given the First flag in the library one can specify a certain

shape for all those pads in the layout.

Elongation defines the aspect ratio of length to width of Long and Offset

pads (see image). The value is given in percent. Click with the mouse into the

field Long or Offset and the image on the left shows the corresponding

calculation rule.

100 % is equivalent to an aspect ratio of 2:1. 0 % results in a normal octagon

pad with an aspect ratio of 1:1. The maximum is 200 % (ratio 4:1).

150

➢

Roundness: 0 - 10 - 25 - 50 - 100 [%]. Right: 100 %,

square

6.3 Considerations Prior to Creating a Board

➢

Design Rules: Adjusting pad shapes

Notes on the display in the Layout Editor:

If pads or vias have different shapes on different layers, the shapes of the

currently visible (activated with DISPLAY) signal layers are displayed on top

of each other.

If the color selected for layer 17, Pads, or 18, Vias, is 0 (which represents the

current background color), the pads and vias are displayed in the color and

fill style of their respective layers. If no signal layer is visible, pads and vias

are not displayed.

If the color selected for layer 17, Pads, or 18, Vias, is not the background

color and no signal layers are visible, pads and vias are displayed in the shape

of the top and bottom layer.

This also applies to printouts made with PRINT.

Supply

Specifies the settings for Thermal symbols.

The value for Thermal isolation determines the distance between a polygon

and the restring of the pad or via that is joined to the polygon through a

Thermal symbol.

The Generate thermals for vias flag permits Thermal symbols at through-

holes. Otherwise vias are fully connected to the copper plane. This applies

also for polygons. But you can disable this option for individual polygons

with CHANGE THERMALS OFF and a mouse click onto the polygon's

contour.

Inside hatched polygons EAGLE doesn't generate Thermal symbols

151

6 From Schematic to Finished Board

for vias that do not have a direct contact to one of the polygon lines.

Pads or SMDs marked with the flag NOTHERMALS (CHANGE THERMALS

OFF) in the Package Editor will be connected basically without Thermal

symbols.

Masks

Settings for the overmeasure of the solder stop mask (Stop) and the solder

cream mask (Cream) are made here.

The default value for solder stop is 4 mil, i.e. minimum value is maximum

value is 4 mil. The percent value has no effect in this case.

The value for the cream frame is set to 0, which means that it has the same

dimensions as the SMD.

If values are given in percent, in the case of SMDs and pads of the form Long

or Offset, the smaller dimension is the significant one. The values are

constrained by minimum and maximum values.

The value for Cream is given positively, as is Frame, although its effect is to

reduce the size of the solder cream mask (cream frame).

The solder cream mask is only generated for SMDs, and is displayed on layer

31, tCream, or layer 32, bCream.

The solder stop mask is drawn in layers 29, tStop, or 30, bStop.

Setting the flag STOP or CREAM (only for SMD) to OFF for a pad or SMD at

the Package definition forbids EAGLE to generate a solder stop mask or a

cream frame for it.

Limit determines, together with the hole diameter, whether or not a via is to

be covered with solder stop lacquer.

152

➢

Design Rules: Settings for Solder Stop and Cream Frame

6.3 Considerations Prior to Creating a Board

Example:

The default value for Limit is 0. This means all vias get a solder stop symbol.

They are free of solder stop lacquer.

Set the Limit = 24:

All through-plated holes with diameters up to 24 mil don't get a solder stop

symbol (they are lacquered), but vias with larger hole diameters get a solder

stop symbol.

For vias with hole diameters below the Limit the STOP flag can be set

(CHANGE STOP ON). EAGLE generates a solder stop mask then.

Misc

Here you can select/deselect various checks which are made by the Design

Rule Check:

Check grid

examines whether objects lie precisely on the grid currently set by the GRID

command. This test is not always worthwhile, since in many cases Devices

built to both metric and imperial grids are in use at the same time. No

common grid can be found in such a case.

Check angle

ensures that all tracks are laid at whole multiples of 45 degrees. This test is

normally switched off, but can be activated if required.

Check font

(de-)selects the font check.

The DRC checks if texts are written in vector font. Text which is non-vector

font is marked as an error. This check is necessary due to the fact that the

CAM Processor can't work with others than vector font for the generation of

manufacturing data.

Assumed you use proportional font text in the bottom layer, place it between

two tracks, and use the CAM Processor to generate Gerber files, it could

happen that the tracks are shorted by the text (height and length of the text

can change)!

Default: on.

Check restrict

can be set off if copper objects should not be checked against restricted areas

drawn in layers 39, tRestrict, and 40, bRestrict. Default setting: on

If restricted areas and copper objects are defined in a common Package,

EAGLE does not check them against each other. Restricted areas that are

realized by cutout polygons are not checked by DRC!

Setting the Design Rules is captured by the UNDO/REDO function.

6.4 Create Board

After you have created the schematic, click the Board icon.

An empty board is generated, next to the components that are to be placed,

joined together by airwires. Supply pins are connected by those signals which

correspond to their name, unless another net is explicitly joined to them.

153

6 From Schematic to Finished Board

The placement grid for components is set to 50 mil (1.27 mm) by default.

If you prefer a different placement grid, you are allowed to specify it

optionally with the BOARD command in the Schematic Editor's command

line.

To have the components placed, for example, in a 1 mm grid, type:

+5-

The unit has to be specified in the command line directly.

The board is linked to the schematic by the Forward&Back Annotation

engine provided that both files are always loaded. If both loaded during

editing they are guaranteed to remain consistent. Alterations made in one file

are automatically carried out in the other.

If you already generated a board from your schematic and continue placing

components in the schematic, the referring packages in the board are placed

in the current grid setting of the Layout Editor.

If, for example, the Schematic is loaded and edited without the

Layout, consistency can be lost. The Forward&Back Annotation

Engine no longer functions. Differences must then be rectified

manually with the aid of the error messages provided by the ERC

(see page 198).

If you would like to see a descriptive text for your board file in the Control

Panel's treeview Projects branch, you can define it by the Layout Editor's

Edit/Description menu. You are allowed to use HTML tags for formatting the

text.

Without the Schematic

If you work without a Schematic, you must generate a new board file, place

the Packages with the ADD command and define the connections with the

SIGNAL command.

To understand this process, please read the section on Placing Components

on page 116, and the section on Specifying Net Classes on page 123. These

two points apply to the Layout Editor as well as to the Schematic Editor.

You are also allowed to define attributes in the Layout Editor. Please read the

chapter about defining Attributes beginning with page 127.

The remaining procedures are identical for users with and without the

Schematic Editor.

Specify the Board Outline

A board that has just been generated from a schematic diagram initially

appears as in the following image. Here a few components have been already

moved into the board area.

154

6.4 Create Board

➢

Board command: Create the layout from the schematic

The Devices are automatically placed at the left of the board.

The board outline can be drawn as a simple narrow line in layer 20,

Dimension with the LINE command.

It's easily possible to draw round outlines, too. Therefore use the CIRCLE

command with a small width near 0.

You can also place a board contour from a library (such as 19inch.lbr) with

ADD.

EAGLE detects properly drawn contours (single closed outline, non self-

intersecting) and shows the board area in a different background color

compared to the rest of the background in the Layout Editor. Mounting holes

and milling contours, drawn in layer 46, Milling, are also recognized.

Only a board with a properly drawn contour can be pushed into

Autodesk Fusion 360 with the FUSIONSYNC command in order to

get a full 3D representation of your design.

A script file can, alternatively, be read by the SCRIPT command. The

euro.scr file, for instance, can be used. Simply type

+

on the command line.

The board outline serves simultaneously as a boundary for the autorouter or

Follow-me router.

155

6 From Schematic to Finished Board

If your board has additional cut-outs, you should draw the necessary milling

contours in a separate layer, for example in 46, Milling. Use the LINE

command with wire width = 0 to define your lines.

Arrange Components

Drag the various components to the desired positions.

With the default option Group command default on set, you can move a

group of components by simply clicking into empty space in the drawing and

dragging a rectangle around the objects or by defining a group polygon

(subsequent left-clicks). Now move the selection by clicking into the selection

and holding the left mouse button and moving it.

Single components can be clicked and dragged into the board area. Release

the mouse button and the component is placed.

Devices can be clicked on directly, or addressed by name.

If you type, for example,

7+:-;

in the command line, the Device named R14 will be attached to the mouse

cursor, and can be placed.

Precise positioning results from input such as:

7+:-;@0$.9.$90B

R14's locating point is now located at these coordinates.

Keep the Ctrl key pressed while selecting a component in order to let

its origin jump at the mouse cursor and move it onto the currently

used grid.

If the above mentioned default setting is off, click onto the GROUP icon and

then draw a frame around the desired elements, click MOVE, and then click

into the group with the right mouse button in order to select it. With a click

of the left mouse button you can place the group at the desired location.

ROTATE, or a click with the right mouse button while the MOVE command

is active turns a Device through 90 degrees. This also applies to groups.

In order to place a component in any angle you may specify the rotation

directly with the ADD command or later with ROTATE or MOVE in the

parameter toolbar.

Next to the Angle box are the buttons for the Spin and Mirror flag.

The left-hand Spin icon is selected , if the spin flag is not set (default).

This means that texts are displayed always readable from the right or from

the bottom side of the drawing.

156

➢

Parameter toolbar for ROTATE, MOVE, ADD, COPY

6.4 Create Board

If the spin flag is activae – the right-hand Spinned icon is marked – the

texts can be displayed in any rotation, also upside down.

The Mirror icons used with components determine where a component is

placed: on the top side (default) or on the bottom side of the board. If a

component is placed on top, the left-hand icon is active. If you want to place

it on the bottom side, click onto the right-hand Mirrored icon.

As an alternative you can work with the command line:

+;9C-C

adds a rotation of 45° to the current position of part IC1. Assumed you tried,

for example, to rotate the component with the ROTATE command and

pressed mouse button, and you decided that it is not possible to obtain the

exact rotation angle this way (because of a too coarse grid) type in the

command line:

+;9C-C

The rotation of IC1 is now exactly 45°. The = sign stands for absolute values.

The initial position does not matter.

If, for example, a SMD should be placed on the bottom side of the board you

may add the Mirror flag, as in:

+7;9C-C

An additional Spin flag causes texts to be written upside down (by a rotation

of 180°), that means they can be read from the top view:

+7-#0C-C

The Spin flag is alternating, i. e. using it again causes the text to be displayed

'normal' again.

Check frequently whether the placement is optimal. To do this, use the

RATSNEST command. This calculates the shortest connections of the

airwires between two pints.

In boards that contain a huge number of signals it may be useful to hide

some of the airwires or display only a few of them. If you want to hide, for

example, the signals VCC and GND, type in the command line

Z:5

if want to see them all again, type:



More information about this can be found in the EAGLE help section.

The position of particular Devices can be displayed by typing the Device

name onto the command line or by clicking directly on an object while the

SHOW command is active.

INFO shows detailed information about the selected object. Depending on

the object you clicked on, some of its properties can be altered in the dialog.

The LOCK command allows you to fix components on the board. They can't

be moved any more then. Shift+LOCK releases the component again. LOCK

can be used with groups as well.

157

6 From Schematic to Finished Board

If the text for the name or the value is located awkwardly, separate them

from the Device with SMASH and move them to whatever position you prefer

with MOVE. At the same time EAGLE shows a line from the text's origin to

the belonging object. Clicking with DELETE on either of the texts makes it

invisible.

Activate the SMASH command, hold down the Shift key, and click onto the

component to have the texts displayed at their original positions again. They

are no longer editable and unsmashed, again. Another way to archive this is

to deactivate the option Smashed in the context menu's Properties entry.

Please keep in mind that the CAM Processor always uses vector font

for generating manufacturing data.

We recommend to write texts in the layout always in vector font (at

least in the signal layers). If you do so the shown text meets exactly

reality. Further information can be found on pages 48 and 177.

Attributes for Components and Global Attributes

If you want to assign any further information than name and value to a

component in the Board, you can do this with the ATTRIBUTE command.

In case a component does not have library-defined attributes you can create

attributes for a component the Schematic, as well as in the board file. If

Back&Forward Annotation is active, any attribute change in the schematic

will affect the board.

However, attribute changes made in the Layout editor won't be back-

annotated into the schematic. They are kind of independent. It is also

possible to delete them in the board. Consitency between schematic and

board remains unchanged nevertheless.

Global attributes are not valid for single components but for the whole board.

They can be defined in Board and Schematic separately.

You will find more information about this in the Creating the Schematic

chapter on page 127.

Boards with Components on Both Sides

If the board is also going to have components on the Bottom layer, the

MIRROR command is used. It causes Devices on the underside to be

inverted. SMD pads, the silk screen and the layers for the solder stop and

solder cream masks are automatically given the correct treatment here.

While ADD, COPY, MOVE, or PASTE is active it is possible to mirror an

object or a selected group with the middle mouse button.

Define components in the Package Editor always on the top side!

158

6.4 Create Board

Exchanging Packages

If, as the layout is developed, you want to replace the selected Package

variant with a different one, then you can use either the PACKAGE or the

REPLACE command, depending on the situation.

PACKAGE Command

It is assumed that the layout and the schematic diagram are consistent and

the Device has been defined with more than one Package variant.

Type in the command line PACKAGE and click onto the Package to be

replaced or alternatively click onto the Package with the right mouse button

and select the Package entry from the context menu. A third variant would

be to click onto the CHANGE icon and select the Package option.

Now you select the desired Package, and confirm it with OK, in the dialog

that then appears.

If the Show all technologies option is active, the Package versions for all the

technologies available for this Device are displayed. If this option is not active

you will only see Packages that are defined in the selected technology.

The Package can also be exchanged from within the schematic diagram.

Devices that don't have alternative Package variants defined, can be modified

in the Library Editor. Add further Package variants as needed and update

your drawing with the new library definition. See page 262 Choosing the

Package Variants for further information.

If you change the Package variant of a Device which you gave a new value

with the help of the VALUE command, although it has been defined with

VALUE Off, the value will remain unchanged. See also page 83.

If you would like to change the Package variant for several identical parts,

you can do this in the command line.

Define a GROUP with all parts that shall get a new Package variant, first.

Now type in the command line

*4C<M=C

159

➢

CHANGE package dialog

6 From Schematic to Finished Board

and click with Ctrl + right mouse button into the drawing.

The name of the new Package variant has to be enclosed in inverted commas.

REPLACE command

Consistent Schematic/Layout Pair

The REPLACE command allows you to substitute one component with

another. The well-known ADD dialog window opens where you can select the

new part. Now click onto the part you want to have replaced in the Schematic

or Layout. The old and new Device must be compatible, which means that

their used Gates and connected pins/pads must match, either by their names

or their coordinates. Otherwise the substitution is not possible.

Layout without Schematic

If you have a layout without an associated schematic diagram, you exchange

the Package with the aid of the REPLACE command. REPLACE opens the

window that is familiar from the ADD dialog, in which it is possible to search

for Devices. When the Package has been chosen you click on the part that is

to be replaced in the layout.

The REPLACE command operates in the Layout Editor in two ways, chosen

in the Parameter toolbar or with the SET command:

The first mode permits Packages whose pad or SMD names are identical to

be exchanged. The connecting areas can have any position.

In the second case (replace_same coords) the pads or SMDs in the new

Package must be located at the same coordinates (relative to the origin). The

names may differ.

The text for the name and value of a Device is only exchanged if they have not

been separated from the Device with SMASH.

The new Package can come from a different library, and can contain

additional pads and SMDs. Connections on the old Package that were

connected to signals must exist correspondingly in the new Package. The new

Package can even have fewer connections, provided that this condition is

satisfied.

160

➢

Select REPLACE mode

6.4 Create Board

Changing the Technology

It is possible to change the technology of a Device in the layout at any time ,

provided there are various technologies defined in the library. Use the

CHANGE command with the Technology option or the Technology

command of the context menu (available by clicking onto the Package with

the right mouse button). This procedure is identical to the one described

before in which Package forms are exchanged using PACKAGE.

Define Forbidden Areas

Areas in the form of rectangles, polygons or circles in layers 41, tRestrict, and

42, bRestrict, are forbidden for the Autorouter/Follow-me router. No copper

objects may be drawn in the top or bottom layers inside these areas. These

regions are tested by the Design Rule Check and taken into consideration by

the Autorouter/Follow-me router.

Layer 43, vRestrict, is for drawing restricted areas where the Autorouter or

the Follow-me router may not set vias. Manually placed vias in such a

vRestrict region are not examined by the DRC and therefore not reported as

an error.

Routing – Placing Tracks Manually

The ROUTE command allows the airwires to be converted into tracks.

ROUTE offers two different modes: Walkaround obstacles (default) and

Ignore obstacles . These modes can be selected in the parameter toolbar

of the ROUTE command.

Walkaround Obstacles

In this mode the routing engine takes care on Design Rules. If there is an

obstacle along the routing path, EAGLE will calculate a new path for your

trace.

Ignore Obstacles

This mode is the classic EAGLE routing mode. Here the user has to take care

on all the Design Rules by his own. This means taking care on clearances, net

classes, copper – dimension distances, overlaps, but you have full control

over the routing paths.

How to route

After activating the ROUTE command select the starting layer in the

parameter toolbar and click onto an airwire. Now the first segment of the

trace follows the mouse cursor. Please check the wire width! Does it fit? With

a left click you fix the segment.

In case you want to change the routing layer for the next segment, click the

middle mouse button. Depending on the layer setup a layer selection menu

will popup, or in a two-layer board the alternative layer will be chosen

automatically. Now a via is displayed the trace’s end. The following left

mouse click fixes the via and the next segment is following the mouse cursor

161

6 From Schematic to Finished Board

in the chosen layer. The layer change can also be initiated by hitting the

Space bar. This way you subsequently step through the routing layers

available.

Clicking with the right mouse button changes the way in which the track is

attached to the mouse and how it is laid (SET command, Wire_Bend

parameter). Among them are modes which allow to use a wire as 90-degree

or as free-definable arc.

In the parameter toolbar you see two additional Wire_Bend icons for the

Follow-me router. The Follow-me router can route a selected airwire

automatically. The position of the mouse cursor determines the trace of the

connection. The settings of the Design Rules and the relevant Autorouter

settings are taken into consideration. In this mode vias are set automatically.

Please check the Autorouter chapter for more information about function

and usage of the Follow-me router.

The signal's name and net class will be displayed in the status bar. When a

signal line has been completely laid, EAGLE confirms that there is a correct

connection with a short beep as it is placed.

The signal name can be used in the command line directly, for example

ROUTE VCC. EAGLE starts the trace at a signal's connection point which is

nearest to the current mouse position.

You can start routing at any point of an already laid trace, via, pad or SMD.

In case you want to re-route a part of an already routed trace, the obsolete

path of the trace will be removed. The Loop Remove options is on by default.

It can be switched off and on in the parameter toolbar of the

ROUTE command.

If there is no longer enough room for routing a signal, other tracks can be

relocated with MOVE and SPLIT, or the properties of tracks (width, layer)

can be modified in the traces’ Properties dialog or with the CHANGE

command.

SPLIT can be used to insert bends into a trace.

If a plated-through hole (a via) is to be placed at a certain point, this can be

done with the VIA command. Use the NAME command to assign the via with

the signal it should be connected to.

Airwires with length of 0 (for example, from Top to Bottom layer) are drawn

as a cross in layer 19, Unrouted.

Ending a wire at the same position where another wire of the same signal but

in another layer already exists and pressing the Shift key at the same time

causes EAGLE to place a via. Otherwise it won't.

If you intend to design a multilayer board and use Blind and Buried or Micro

vias, please note the details (also for the VIA command) in the section about

Multilayer Boards beginning at page 178.

While laying out wires EAGLE calculates the shortest connection to the

closest point of the current signal automatically. This connection is

represented by an airwire.

162

6.4 Create Board

Pads and SMDs that belong to the currently routed signal have the so-called

magnetic-pads function:

Within a certain radius around the pad the wire will be snapped to the pad's

center automatically. That is to say as soon as the length of the automatically

calculated airwire is shorter than the given value for snap length, the wire

jumps into the pad's or SMD's center point. It doesn't matter whether the

pad or SMD is exactly located at the currently used grid. The snap point is

always the center point.

As soon as you move the mouse cursor away from this pad beyond the limits,

the airwire will be shown and the wire to be routed follows the mouse again.

The snap length can be defined in the menu Options/Set/Misc. Default value

is 20 mil.

As the routing proceeds it is helpful to run the RATSNEST command

frequently, in order to recalculate all the airwires.

For more complex boards it may be useful to adjust the Snap Length in the

Options/Set/Misc menu as described on page 111.

For a better visibility of the traces in the routing layer you can enable the

Single Layer mode. All visible layers except the currently selected routing

layer are displayed in a grayish color. This mode is accessible in the ROUTE

commands parameter toolbar. Click to switch the mode off, or to

activate it.

Un-route traces

Use RIPUP if you want to convert the whole or part of a track or a via that

has been laid back to a signal line. By clicking on a track it is decomposed

between the nearest bends. If you click on this location again (on the

airwire), the whole signal branch back to the nearest pads is decomposed. If

you want to undo the whole of the signal, click RIPUP and enter the name of

the signal on the command line. More than one may be entered at the same

time.

The command

5:D9:

converts the three signals GND, VCC and +5V back to airwires.

Z5:

on the other hand converts all signals apart from GND and VCC to airwires.



converts all signals (that are visible in the editor) into airwires. To truly

include every track, all the layers in which tracks have been drawn must be

visible (DISPLAY).

Traces with arcs

If you want to use wires as arcs or try to smooth the wire bends see the hints

concerning the MITER command in the help function. The miter radius

determines how the wire joints are mitered. A positive value generates a

rounding, a negative one a straight line. The miter radius influences some

163

6 From Schematic to Finished Board

bend modi (0, 1, 3, 4; see SET command) and is shown additionally in the

parameter toolbar of the commands SPLIT, ROUTE, LINE, and POLYGON.

While LINE or ROUTE is active it is possible to click through the previously

mentioned wire bends (bend modes) with the right mouse button. EAGLE

knows ten different modes (0..9) which are shown as icons in the parameter

toolbar. Mode 8 and 9 are special modes for the Follow-me router.

Holding down the Shift key while clicking the right mouse button reverses

the direction of selection.

Holding down the Ctrl key allows to toggle between complementary wire

bends.

If you want to have only some wire bends available for the right mouse

button, you can define this, for example, in the eagle.scr file.

Supposed you want to work with wire bends number 2, 5, 6, and 7 use the

following syntax:

5,.9>A

However, if you want to use another bend mode you can always chose it from

the parameter toolbar.

It is also possible to leave the track laying to the Autorouter which

has its own chapter in this manual.

Laying tracks with the Follow-me router is explained in a subsection

of the Autorouter chapter.

Defining a Copper Plane with POLYGON

EAGLE can fill regions of a board with copper. Simply draw the borders of

the area with the POLYGON command. The polygon is displayed as a dotted

line in the outline mode. You give the polygon a signal name, using NAME

followed by a click onto the border of the polygon. Then all the objects that

carry this signal are connected to the polygon. Both pads and, optionally, vias

(as specified in the Design Rules) are joined to the copper plane through

Thermal symbols. Elements not carrying this signal are kept at a specified

distance.

RATSNEST calculates and displays the surface area of all polygons in the

layout. If you call RATSNEST with a signalname, for example

5

only the GND polygon(s) will be calculated. All other polygons in the layout

will remain unchanged in the outline mode.

RIPUP, followed by a click on the polygon border, makes the content

invisible again. If there are several polygons in your layout, and you want to

have them displayed in the outline mode again, type in the command line:

,

To have all polygons of a particular signal switched to outline mode, specify

the signal name, like

,5

More information about the syntax can be found in the help about RIPUP.

164

6.4 Create Board

The content of the polygon is not saved in the board file. When you first load

the file, you will only see the dotted outline of the polygon. It is only

calculated and displayed again by RATSNEST.

Various options can be changed via the parameter toolbar, either as the

polygon is being drawn or, with CHANGE, at a later stage.

Width:

Line thickness with which the polygon is drawn. Select the largest possible

width. That avoids unnecessary quantities of data when the board is sent

for manufacture. If the wire width is lower than the resolution of the

output driver in the CAM Processor, a warning is issued.

A finer line width permits the polygon to have a more complex shape.

Pour:

Specifies the filling type: the whole area (Solid) or a grid (Hatch).

The special type Cutout can be used to define polygons that get subtracted

from all other signal polygons within the same layer. Suitable for cut-outs

(restricted areas) in polygons in inner signal layers.

Rank:

Overlapping polygons must not create any short-circuits. Rank can

therefore be used to determine which polygons are to be subtracted from

others. A polygon with rank = 1 has the highest priority in the Layout

Editor, no other polygon drawn in the layout is ever subtracted from it,

while one with rank = 6 has the lowest priority. As soon as there is an

overlap with a higher rank, the appropriate area is cut out from the

polygon with rank = 6.

Polygons with the same rank are compared by the DRC. The rank property

works only for polygons with different signals. For overlapping polygons

with the same signal name it is without effect. They will be drawn one over

the other.

Polygons that are created in the Package Editor and not assigned to a

signal, will be subtracted from all other polygons. There is no rank

parameter available.

Spacing:

If the option Hatch is chosen for Pour, this value determines the spacing of

the grid lines.

Isolate:

Defines the value that the polygon must maintain with respect to all other

copper objects not part of its signal and objects in Dimension, tRestrict or

bRestrict layer. If higher values are defined for special signals in the

Design Rules or net classes, the higher values apply.

165

➢

POLYGON command: Parameter toolbar (split into two

lines)

6 From Schematic to Finished Board

In the case of polygons with different Ranks, Isolate always refers to the

drawn contour which is shown in the outline mode of the polygon, even if

the calculated polygon has got another contour, for example, due to a wire

that supersedes the polygon. The actual clearance can become greater than

the given Isolate value.

Thermals:

Determines whether pads in the polygon are connected via Thermal

symbols, or are completely connected to the copper plane. This also applies

to vias, assuming that the option has been activated in the Design Rules.

The width of the thermal connectors is calculated as the half of the pad's

drill diameter. The width has to be in the limits of a minimum of the wire

width and a maximum of twice the wire width of the polygon.

The length of the thermal connectors is defined by the Thermal isolation

value in the Design Rules' Supply tab.

Don't choose the polygon's width too fine, otherwise the thermal

connectors won't handle the current load.

This is also true for bottlenecks in the board! The polygon's wire

width determines the smallest possible width of the copper area.

Orphans:

Determines if a polygon may contain areas (islands) which are not

electrically connected to the polygon's signal.

If Orphans is set Off such un-connected areas won't be drawn.

When drawing a polygon, please take care to ensure that the outline

is not drawn more than once (overlapping) anywhere, and that the

polygon outline does not cross over itself. It is not possible for EAGLE

to compute the contents of the area in this case.

An error message 'Signalname' contains an invalid polygon! is

issued, and the RATSNEST command is aborted.

If this message appears, the outline of the polygon must be corrected.

Otherwise, manufacturing data cannot be created by the CAM

Processor.

The CAM Processor automatically computes the polygons in the

layout before generating its output.

If the polygon stays in the outline mode after calculating it with

RATSNEST, you should check the parameters for width, isolate, and

orphans and the polygon's name. Probably the polygon's filling is not

able to reach one of the objects that should be connected with its

signal.

Renaming a polygon with the NAME command, connects it with

another signal!

166

6.5 FUSIONSYNC – Synchronise EAGLE Board and Fusion 3D Board

6.5 FUSIONSYNC – Synchronise EAGLE

Board and Fusion 3D Board Model

In the Layout Editor on the right hand side you see a FUSIONSYNC flyout.

It’s displayed by default, but could also be hidden by switching off this option

in the Options/User Interface menu.

The ECAD world and the MCAD world now are unified. With FUSIONSYNC

it is possible to exchange board data between EAGLE and Autodesk Fusion

360. Synchronizing board data works in both directions. Either you push

your EAGLE board into Fusion or you pull the board object from Fusion into

EAGLE.

How does this work?

Synchronise with Fusion

Design your board as usual. At any time, when you think it’s time to

synchronise your board with Fusion, click the FUSIONSYNC flyout. By doing

so EAGLE and Fusion exchange all data needed. Now your design entered

the mechanical world.

What if There Need to be Changes in the Board’s Geometry?

In case there have to be made changes in the board’s geometry – maybe a

mounting hole has to be moved, the board size has to be amended so that it

fits exactly into the enclosure, or one of the bigger components have to be

moved some millimeters – the Fusion designer can move component objects

or amend the board contour or move a mounting hole, or add a cut-out in the

board. If this is done, you will get notice in EAGLE that your board is out of

sync.

You can pull in the new board object into EAGLE and see the new board

contour, or the hole or a component moved to another position. Now you

have to check your layout and it’s might be a good idea to run a DRC. Please

check the positioning of your components, board contour, and traces that

were already routed to a component which has been moved and so on.

Continue designing your board and as soon as you think all is okay,

synchronise and push it into Fusion again.

How to Synchronise

Click onto the FUSIONSYNC flyout and choose one of the options

presented in the dialog: Either synchronize with an already existing

project or choose a new Fusion project.

If you want to sync with an existing Fusion project, select the first

option and klick Next.

167

6 From Schematic to Finished Board

Choose one of your Fusion projects from the list. The Fusion project has

already to have the PCB feature created. In the image below you can see, that

the Hello World project has already a PCB1 feature which was created before

in the Fusion project. Click OK to proceed.

In the next dialog we see the current sync status.

168

➢

FUSIONSYNC: Select Fusion type

➢

FUISONSYNC: Choose the Project

6.5 FUSIONSYNC – Synchronise EAGLE Board and Fusion 3D Board

Here the projects are out of sync. This is also indicated by the

FUSIONSYNC flyout that changed its color to red.

The Edit Source button will open the selected project in Fusion.

169

➢

FUSIONSYNC: Syncing EAGLE and Fusion

➢

FUSIONSYNC: Board shape drawn in Fusion

6 From Schematic to Finished Board

View on Web

If you click View on Web, your web browser will open and bring you to the

“bridge” between electronic and mechanical design. This is the place where

your board from EAGLE and the board object from Fusion are managed.

You could review, for example, the different versions that were synchronised

between EAGLE and Fusion. It’s also possible to view and share a 3D

representation of your project in Fusion Team. It allows to have markups,

make comments, add measures, show, for example, an exploded view, and

export in different data formats.

Pull from Fusion

Click on the Pull from Fusion button. A description that was created in

Fusion when the PCB object was defined is show in the dialog.

Click the Pull button to start syncing now. The syncing process will take some

seconds and finally you will see the new board shape in the Layout Editor.

170

➢

FUSIONSYNC: Online 3D View in Fusion Team

6.5 FUSIONSYNC – Synchronise EAGLE Board and Fusion 3D Board

In the Pull from Fusion section of the Fusion Sync window now it says

UP TO DATE. The FUSIONSYNC flyout is displayed in green now.

The section Push to Fusion still says OUT OF SYNC. The reason is that you as

the EAGLE designer have the last word in finalizing the project. Typically you

go on designing the board and at a final point you decide to push your design

into Fusion.

Push to Fusion

Therefore click the FUSIONSYNC flyout. In the Fusion Sync window’s

Source page click the Push to Fusion… button. What happens first now, is

showing you a list of the components on your board and the information if

there is already assigned a 3D model for it.

In case there are not all packaged assigned to a 3D model, you should change

this in the EAGLE libraries and update your design. Otherwise you do not see

the components as proper 3D representation in Fusion.

171

➢

FUSIONSYNC: New Board Shape Pulled from Fusion

6 From Schematic to Finished Board

Enter a Version Description so that everyone knows what’s going on and

then click the Push button. The board will be transferred into Fusion.

In Fusion it is allowed to modify the board shape, moving components,

adding holes or slots in the board. If this is done, you have to pull the design

into EAGLE again and clean up your layout. Please run DRC in order to

recognize all possible problems that could be in the design now. After

cleaning up the board and finishing the design process, push it into Fusion

again.

172

➢

FUSIONSYNC: Push to Fusion - 3D Package Assignment

➢

FUSIONSYNC: EAGLE Board in Fusion

6.6 DRC – Checking the Layout and Correcting Errors

6.6 DRC – Checking the Layout and

Correcting Errors

The Design Rule Check (DRC) is carried out at the end of the board design, if

not before. If you have not yet specified any Design Rules for the layout, this

is your last opportunity. See the section on Specifying the Design Rules from

page 144. To start the Design Rule Check click onto the DRC icon in the

command toolbar or the entry DRC... in the menu Tools.

Usually one sets the common Design Rules with the Edit/Design

Rules.. menu first and starts the Design Rule Check when required

with the DRC command. But it is also possible to adjust the Design

Rules if you use the DRC command. Some settings, like those for

Restring, affect the layout directly.

➢

Starting the Design Rule Check

When you have finished the adjustments, start the error check by clicking

Check. At the same time the Design Rules are stored in the board file itself.

By clicking Select you specify the region of the layout that is to be examined.

Simply drag a rectangle over the desired region with the mouse. The error

check will then star automatically.

Clicking on Apply transfers the settings to the board file. This means that the

values that have so far been chosen are not lost if you do not immediately

start the error check and if you want to leave the DRC dialog via the Cancel

button.

173

6 From Schematic to Finished Board

All signal layers and the Airwires are always examined by the

Design Rule Check, no matter if visible or not (DISPLAY command).

The DRC Errors Window

If the Design Rule Check finds errors or unrouted signal wires, an error

window opens automatically. It lists all the errors/airwires found. The

window can be opened at any time by means of the ERRORS command.

➢

DRC Errors list in the Layout Editor

Each error is marked with an error polygon. Its size tells you, for example in

the case of a clearance error, about how much the limit is exceeded. The error

polygons are visible in the Layout Editor, only. They won't be printed nor

exported with the CAM Processor. It's not possible to erase them with the

DELETE command. Click the Clear all button to delete them. Or type in the

command line:

+

Errors are marked with a red icon in the errors window. If an error in the list

is selected, a line points to the corresponding location in the board.

It is possible to have the error list sorted, ascending or descending, by error

types or layer numbers. therefore click onto the column headers Type or

Layer.

174

6.6 DRC – Checking the Layout and Correcting Errors

The errors dialog shows only errors that occur in the currently

displayed layers.

In case you zoomed into the drawing and there is only a partial view of the

board, you can click the option Centered. The currently selected error is

shown in the middle of the drawing window now. If you prefer to have the

Centered option deactivated for browsing the error list, you are nevertheless

able to center an error in the middle of the drawing area by pressing the

Enter key.

While correcting the error on the board, the DRC Errors window may remain

opened. After correcting one error you can mark it as Processed in the error

list by clicking onto the Processed button. The red error icon turns gray now.

In some situations it may be the case that you want to tolerate an error. Use

the Approve button for this. The error entry will be removed from the Errors

branch and appear in the Approved branch and the error polygon is no

longer shown in the Layout Editor.

If you want to treat an already approved error as a quite normal error, select

it in the Approved branch, and click onto the Disapprove button. Now it is a

member of the Errors branch again.

Clicking the Clear all button does not delete approved errors. They remain in

the Approved branch.

Moving an entry from one branch into the other, marks the board file as

changed and not saved.

In some cases it might be useful to approve all errors that are shown. To do

so, select the superior Errors entry in the errors list. Now the Approve

button will be named Approve all. Click it in order to have all errors moved

into the Approved list. This is also feasible the other way round for

disapproving all errors.

Error Messages and their Meaning

Airwire:

Shows a remaining signal wire that still needs to be routed. Only if there

are no Airwires left in the layout, one can be sure that all connections are

made properly.

Angle:

Tracks are not laid in an angle of 0, 45, 90 or 135°. Default: off.

Blind Via Ratio:

The limit of the ratio of via length (depth) to drill diameter is exceeded. In

this case you have to adjust the via's drill diameter (Design Rules, Sizes

tab) or the layer thickness of your board (Design Rules, Layers tab).

Clearance:

Clearance violation between copper objects. The settings of the Design

Rules' Clearance tab and the value for Clearance of a given net class are

taken into consideration. Of these two values the higher one is taken for

checking.

175

6 From Schematic to Finished Board

In addition the Isolate value will be taken into consideration for polygons

with the same rank and polygons which are defined as a part of a Package.

To deactivate the clearance check between objects that belong to the same

signal, use the value 0 for Same signals in the Clearance tab.

Micro Vias are treated like wires. The clearance value for wire to wire

applies in this case.

Dimension:

Distance violation between SMDs, pads, and connected copper objects and

a dimension line (drawn in Layer 20, Dimension), like the board's outlines.

Defined through the value for Copper/Dimension in the Design Rules'

Distance tab.

Setting the value Copper/Dimension to 0 deactivates this check.

In this case polygons do not keep a minimum distance to objects in layer

20, Dimension, and holes!

The DRC will not check if holes are placed on tracks then!

Drill Distance:

Distance violation between holes. Defined by the value Drill/Hole in the

Design Rules (Distance tab).

Drill Size:

Drill diameter violation in pads, vias, and holes. This value is defined in the

Design Rules' Sizes tab, Minimum Drill.

It is also possible to define a special drill diameter for vias in a given net

class (CLASS command, Drills). In this case the higher one is used for the

check.

Invalid Polygon:

Reason is a not properly drawn polygon contour. As soon as the contour

lines are overlapping or even crossing, the polygon can't be calculated

correctly. Change the polygon's contour in the Layout Editor or in the

Library, if it is part of a Package.

The RATSNEST command shows this error message, as well.

Keepout:

Restricted areas for components drawn in layer 39, tKeepout, or 40,

bKeepout, lie one upon another. This check is executed only if layers 39

and 40 are displayed and if the keepout areas are already defined in the

Package Editor of the library.

Layer Abuse:

Layer 17, Pads, or 18, Vias, contain objects which are not automatically

generated by EAGLE. Probably you drew something manually in these

layers, although they are reserved for pads and vias. Better move such

objects into another layer.

Layer Setup:

This error is shown if an object in a layer is found that is not defined by the

Layer setup. The same for vias that do not follow the settings of the Layer

setup, for example, if a via has an illegal length (Blind/Buried vias).

176

6.6 DRC – Checking the Layout and Correcting Errors

Micro Via Size:

The drill diameter of the micro via is smaller than the value given for Min.

Micro Via in the Sizes tab.

No Vector Font:

The font check (Design Rules, Misc tab) recognizes text in a signal layer

which is not written in EAGLE's internal vector font.

If you want to generate manufacturing data with the help of the CAM

Processor the texts, at least in the signal layers, ought to be written in

vector font. This is the only font the CAM Processor can work with.

Otherwise the board will not look the same as it is shown. Change the font

with the help of the command CHANGE FONT or use the option Always

vector font in the Layout Editor's Options/User Interface menu:

If activated, the Layout Editor shows all texts in vector font. This is the way

the manufactured board will look like.

Activating the sub-option Persistent in this drawing saves the setting in

the drawing file. If you send the layout file, for example, to the board house

you can be sure that the vector font will be displayed also at his system.

No real vector font:

The font check (Design Rules, Misc tab) recognizes text in a signal layer

which is not written in EAGLE's internal vector font although it is

displayed as vector font in the Layout Editor window. This situation arises

if the option Always vector font in the menu Options/User Interface is

active.

See error message No vector font for further details.

Off Grid:

The object does not fit onto the currently chosen grid.

This check can be switched on or off in the Design Rules' Misc tab. The

default setting is off, because as soon as trough-hole and surface-mount

parts are used together it's not easily possible to find a reasonable common

grid. The check is set off by default.

Overlap:

DRC reports this error as soon as two copper elements with different

signals touch each other.

Restrict:

A wire drawn in layer 1, Top, or 16, Bottom, or a via lies in a restricted area

which is defined in layer 41 or 42, t/bRestrict.

If restricted areas and copper objects are defined in a common Package,

the DRC does not check them!

Stop Mask:

If there are silkscreen objects drawn in layers 21, 25, 27 for components on

the Top layer, and 22, 26, and 28 for components on the Bottom layer

overlapping the area of a solder stop symbol generated in layer 29 and 30,

the DRC reports a Stopmask error.

You have to display the corresponding layers to activate this check!

Please keep in mind that this check always takes the vector font as basis for

177

6 From Schematic to Finished Board

the calculation of the required space. This is the font type the CAM

Processor uses for manufacturing data generation.

Width:

Minimum width violation of a copper object. Defined by Minimum Width

in the Design Rules (Sizes tab) or, if defined, by the track parameter Width

of a referring net class. The higher one of the given values will be taken for

this check.

Also the line width of vector font texts in signal layers will be checked.

Wire Style:

The DRC treats a line (wire) whose Style is LongDash, ShortDash or

DashDot in the same way as a continuous line. If a wire drawn with one of

these styles is laid as a signal, the DRC reports a Wire Style error.

For further investigations, net, part and pin lists can be output by

means of the EXPORT command or by various User Language

programs.

6.7 Multilayer Boards

You can develop multilayer boards with EAGLE. To do this, you use one or

more inner layers (Route2 to Route15) as well as the layers Top and Bottom

for the top and undersides. You display these layers when routing.

Before starting the routing of the layout you should be aware of the number

of signal layers to use, if vias should go through all layers, or if you have, due

to the complexity of the layout, to work with Blind, Buried or Micro vias. In

this case you really ought to contact your board manufacturer to inform you

about the possible structure of the board and the costs to be expected.

Inner Layer

Inner layers are used the same way as the outer layers Top and Bottom. They

can be filled with copper areas (polygons) as well.

Before using inner layers you must define them in the Design Rules, Layers-

Tab. More details can be found in the following sections and on page 146.

Supply Layers with Polygons and More than One Signal

Areas of the board can be filled with a particular signal (e.g. ground) using

the POLYGON command. The associated pads are then automatically

connected using Thermal symbols. The isolate value for the Thermal symbols

is specified in the Design Rules (DRC command, Supply tab). The width of

the connecting bridge depends on the line thickness with which the polygon

is drawn (see page 166). You can also specify whether or not vias are to be

connected through Thermals. The minimum clearances from objects carrying

other signals specified in the Design Rules are maintained (Clearance and

Distance tabs). Changes are shown in the layout when the polygon is next

computed (RATSNEST command).

178

6.7 Multilayer Boards

This way you can create layers in which several areas are filled with different

signals. You can assign different ranks (priorities) for the polygons. The rank

property determines which polygon is subtracted from others if they overlap.

Rank = 1 signifies the highest priority in the layout: nothing will be

subtracted from such a polygon. Rank = 6 signifies the lowest priority.

Polygons with the same rank are compared by the DRC.

Please read the notes regarding polygons in the section on Defining a Copper

Plane on page 164.

Do not choose the wire width for polygons too fine! This can lead to

huge amounts of plot data and problems for the manufacturing

process.

Resticted Areas For Polygons

For creating non-copper areas for polygons in inner layers, you can use a so-

called cutout polygon. Such a polygon, with the special fill style cutout,

defines an area which is subtracted from all other signal polygons in this

layer. A cutout polygon may be draw with any wire width, even 0. Compared

to signal polygons a cutout polygon does not cause huge data when creating

manufacturing data.

Signal polygons respect the wire width of the cutout polygon. The dotted line

of the contour is always visible, however does not occur in the manufacturing

data.

Multilayer Boards with Through Vias

This type should be preferred if possible. Vias go through all signal layers and

will be drilled at the end of the production process. The production costs are

relatively moderate.

Layer Setup

The settings concerning layer composition and number of signal layers are

made in the Design Rules, Layers tab, Setup. See page 146.

For through vias the setup is very simple. No considerations about thickness

of copper and isolation layers are necessary.

Simply join two layers by an asterisk (like 1*2 or 15*16) to one core and

combine several cores. This is symbolized by a plus character (like in

1*2+15*16). The isolation layer between two copper layers is called prepreg.

To express the possibility to have vias through all layers the whole expression

is set into parenthesis.

Examples:

4 layers: (1*2+15*16)

6 layers: (1*2+3*14+15*16)

8 layers: (1*2+3*4+13*14+15*16)

Here vias always have the length 1-16. They are reachable from all layers (see

also the help function for VIA).

179

6 From Schematic to Finished Board

Multilayer with Blind and Buried Vias

In high density boards it is often necessary to use Blind and Buried vias.

These kinds of vias don't connect all layers, but are only reachable from a

certain number of layers. How these layers are connected depends on the

manufacturing process of the board which has to be determined in the Layer

setup in the Design Rules.

Please contact your board house before starting your work! Check

which Layer Setup is suitable for your purpose and what the

manufacturing costs are.

Disambiguation

Core:

The non-flexible kernel which is coated with copper on one or on both sides.

Is represented by a * in the Layer Setup. For example 5*12: Layer 5 and 12

are the board's core.

Prepreg:

Flexible glueing or isolating layer which is used in the manufacturing process

of a multilayer board to press inner and outer layers onto each other.

Is represented by a + in the Layer Setup. 1+2 tells us that layer 1 is a prepreg

and combined with layer 2.

Layer Stack:

A pack of any number of layers consisting of cores and prepregs which are

handled together in the current step of production.

Buried Via:

The production process of this via does not differ from a through (normal)

via. The current layer stack will be drilled through completely. In the

following production steps the already drilled vias can be covered (buried) by

pressing further cores and prepregs on the current layer stack. If the via is

not visible on the completed board we call it a buried via.

This is represented by parenthesis, for example in 1+(2*15)+16 where the

Buried Via goes from layer 2 to 15.

Blind Via:

A Blind via connects an outer layer with any inner layer but doesn't go

through all copper layers. The speciality of a Blind via lies in the production

process. The current layer stack is not drilled all through. The drill hole has a

certain depth depending on the number of layers that should be allowed to be

connected with each other. Blind vias have to follow a given ratio of depth to

drill diameter. Please contact your board house to get information about this.

This ratio has to be defined in the Sizes tab as Min. Blind Via Ratio.

This is represented by brackets and the target layer marked by a colon before

or after the bracket. The example [3:1+2+3*14+15+16] allows Blind vias

from layer 1 to 3.

Blind vias may be shorter than defined. In this example you are allowed to

use vias from layer 1 to 2. The Autorouter is also allowed to use shorter Blind

vias.

180

6.7 Multilayer Boards

Micro Via:

The micro via is a special case of a Blind via. It has a maximum depth of one

layer and a very small drill diameter. See page 187.

Displaying Vias

It makes sense to set the layer color of layer 18, Vias, to the background color

(DISPLAY menu, Change, Color) if you are working with vias that have

different lengths and shapes. In doing so it is possible to recognize layer

affiliation.

Layer Setup

Combining cores and prepregs allows many variants. In the following section

some examples show the function of the Layer setup.

Please read this paragraph entirely. Even if you intend to design a four layer

board, for example, it is most advisable to read also all the other examples for

a better understanding.

4-Layer Board

Example 1:

Layers 1, 2, 15 and 16 are used.

Board structure: One core inside, outside prepregs.

Connections: 1-2 (blind vias), 2-15 (buried vias) and 1-16 (through vias)

The setup expression looks like this:

[2:(1+(2*15)+16)]

Explanation:

2*15

Layers 2 and 3 form the core.

(2*15)

Parenthesis allow buried vias from 2 to 15.

(1+(2*15)+16)

On both sides of the core copper layers are pressed on

with prepregs.

The outer parenthesis define continuous vias from 1-16.

[2:(1+(2*15)+16)]

In square brackets and separated by a colon blind vias are defined.

Here from layer 1 to 2.

The following image shows the related setup expression in the Layers tab of

the Design Rules.

Blind vias have to keep a certain ratio of via depth to drill diameter. For this

reason it is necessary to specify values for the layer thickness.

These values are given by your board house! You are supposed to contact it in

either case before starting the layout!

181

6 From Schematic to Finished Board

Type in the values in the Copper (thickness of copper layer) and Isolation

(thickness of isolation layer) fields as shown in the image. The total thickness

of the board is shown below the Copper and Isolation fields.

Example 2:

Layers 1, 2, 15, and 16 are used.

Board structure: One core inside, outside prepregs.

Connections: 1-2, 15-16 (blind vias), 1-16 (through vias)

Setup expression:

[2:(1+2*15+16):15]

Explanation:

2*15

Layers 2 and 3 form the core.

1+2*15+16

On both sides of the core copper layers are pressed on

with prepregs.

(1+2*15+16)

The outer parenthesis define through vias from 1-16.

[2:(1+2*15+16):15]

In square brackets and separated by a colon blind vias are defined.

Here from layer 1 to 2 and 16 to 15.

182

➢

Example 1: Layer Setup for a 4 layer Board

6.7 Multilayer Boards

➢

Example 2: Layer Setup for a 4 layer Board

6-Layer Board

Example 3:

Layers 1, 2, 3, 14, 15, and 16 are used.

Board structure: Two cores, prepregs outside.

Connections: 2-3, 14-15 (buried vias), 1-16 (through vias)

Setup expression:

(1+(2*3)+(14*15)+16)

Explanation:

(2*3)+(14*15)

Two cores with buried vias are pressed together.

1+(2*3)+(14*15)+16

This layer stack is covered with outer layers 1 and 16 which are

isolated with prepregs.

(1+(2*3)+(14*15)+16)

The whole expression in parenthesis defines through vias from 1-16.

183

6 From Schematic to Finished Board

➢

Example 3: Layer Setup for a 6 layer Board

The values for layer thickness for copper and isolation used in these

examples are fictive. Please contact your board house to get the allowed

values.

Example 4:

Layers 1, 2, 3, 14, 15, and 16 are used.

Board structure: One core, on each side two prepregs.

Connections: 3-14 (buried vias), 2-14 (blind vias in inner layer stack),

1-16 (through vias)

Setup expression:

(1+[14:2+(3*14)+15]+16)

Explanation:

2+(3*14)+15

The core with buried vias. One prepreg on each side.

[14:2+(3*14)+15]

Blind vias from layer 2 to 4.

1+[14:2+(3*14)+15]+16

On this layer stack a prepreg on each side is pressed on.

(1+[14:2+(3*14)+15]+16)

Parenthesis allow through vias from 1 to 16.

184

6.7 Multilayer Boards

➢

Example 4: Blind Vias in the inner layer stack

8-Layer Board

Example 5:

Layers 1, 2, 3, 4, 13, 14, 15, and 16 are used.

Board structure: Three cores, prepregs outside.

Connections: 1-3, 14-16 (blind vias), 2-3, 4-13, 14-15 (buried vias),

1-16 (through vias).

Setup expression:

[3:(1+(2*3)+(4*13)+(14*15)+16):14]

Explanation:

(2*3)+(4*13)+(14*15)

Three cores, each with buried vias, are pressed together and

isolated with prepregs.

1+(2*3)+(4*13)+(14*15)+16

Outer copper layers 1 and 16 which are isolated through prepregs

are pressed onto this layer stack.

(1+(2*3)+(4*13)+(14*15)+16)

Parenthesis allow through vias from 1-16.

[3:(1+(2*3)+(4*13)+(14*15)+16):14]

Blind vias from 1-3 and 16-14.

185

6 From Schematic to Finished Board

➢

Example 5: Layer Setup for an 8 layer board

Hints For Working With Blind, Buried, and Micro Vias

VIA command

Depending on the Layer setup vias can have different lengths. The parameter

toolbar of the VIA command shows all available lengths in the Layer box.

When routing manually (ROUTE command) EAGLE takes the shortest

possible via length in order to change layers. It is also possible that vias at the

same position are elongated.

The via length can be changed with the CHANGE VIA command. Select the

value from the according menu and click the via with the left mouse button.

Alternatively use the command line:

*:.-9

and a click onto the via changes the length from layer 2 to 15.

If the given via length is not defined in the Layer setup it will be elongated to

the next possible length or, if this is not possible, an error message will be

generated.

:C5C-;@-$09.B

places a via that belongs to the signal GND and reaches from layer 1 to 4 at

position (1.05 2).

186

6.7 Multilayer Boards

ROUTE Command

If you want to change the layer while laying-out the board, EAGLE always

takes the shortest possible via (CHANGE LAYER command; also in Follow-

me mode). It is also possible that a via at the same position is elongated

automatically.

If Micro vias are enabled in the Design Rules by setting a minimum

value for the drill diameter (Sizes tab, Min. Micro Via) and defining a

proper Layer setup, EAGLE sets a Micro via when routing from a

SMD and immediately changing to the next inner layer.

In Follow-me mode, however, EAGLE can't place Micro vias. The

Follow-me router is powered by the Autorouter engine and therefore

it has to follow its properties and restrictions.

Micro Via − A Special Case of Blind Via

In contrast to Blind vias that can reach several layers deep into the board the

Micro via connects an outer layer with the next inner layer. The drill

diameter of a micro via is relatively small. Presently the usual values are

about 0.1 to 0.05 mm.

For manufacturing reasons Micro vias, as Blind vias, have to follow a certain

Aspect ratio of depth to drill diameter. This ratio defines the maximum via

depth for a certain drill diameter.

The proper value can be learned from your board house.

Set this value in the Design Rules, Sizes tab, Min. Blind Via Ratio.

Assumed the board house demands the ratio as 1:0.5 you have to enter 0.5

for Min. Blind Via Ratio.

Additionally the Design Rule Check verifies the minimum drill diameter for

Micro vias given in Min. MicroVia. If this value is higher than the value for

Minimum Drill (default), micro vias won't be checked.

The diameter of micro vias is set in the Restring tab of the Design Rules.

If you change the layer from an outer to the next inner one while you are

routing a track out of a SMD, EAGLE automatically places a Micro via,

provided the Design Rules allow it.

The Autorouter can't set Micro vias!

6.8 Editing and Updating Components

Open Device/Symbol/Package

Depending on the Editor window you are currently working wit the context

menu of a component offers the entries Open Device/Symbol/Package. If

you select one of them, EAGLE tries to open the referring library file in the

corresponding editing mode. Now you can easily check all the objects the

187

6 From Schematic to Finished Board

Device/Symbol/Package consists of. And it is even possible to modify the

library definition.

In order to update your project with the modified library definition you have

to start a library update (menu Library/Update...)in schematic/board (see

next section)

Please be aware that changes in the libraries can affect a number of

different devices in the library file and therefore your future projects,

as well. Please act accordingly carefully!

In case EAGLE doesn't find the original library file, EAGLE prompts a

warning and cancels this action.

In this case there is a possibility of extracting the library definitions used in

your current project. File/Export/Libraries... starts the User Language

Program exp-lbrs.ulp that creates library files accordingly.

Updating Project (Library Update)

The UPDATE command allows components in a schematic diagram or a

layout to be replaced by components defined in accordance with the current

libraries. This function is of particular interest for existing projects. If, in the

course of development, the definitions of Packages, Symbols or Devices in the

libraries are changed, the existing project can be adapted to them.

The menu item Library/Update causes all the components in a project to be

compared with the definitions in the current libraries. If EAGLE finds

differences, the components are exchanged.

Those libraries on the path specified for Libraries in the Control Panel under

Options/Directories will be examined.

It is also possible to update components from one particular library. Type the

UPDATE command on the command line, stating the library, for instance as:

5!=

5'('8='!'!=K8'!=$!K

or select the library in the File dialog of the Library/Update... menu item.

In the case you want to replace parts from one library with parts from

another library you can use the command:

5!!K<!K$

Old-lbr-name represents the name of the library as shown by the INFO

command in the layout or schematic. New-lbr-name stands for the library

from which you want to take elements. You may add paths as well.

Please see the help function for more information.

In many cases you will be asked whether Gates, pins or pads should be

replaced according to name or according to position. This always happens if

library objects are renamed, or if their position (sequence) is changed.

188

6.8 Editing and Updating Components

If too many changes are made in the library at one time (e.g. pin names and

pin positions are changed) it is not possible to carry out an automatic

adaptation. In such a case it is possible either to carry out the modifications

to the library in two steps (e.g. first the pin names and then the pin

positions), or the library element can be given a new name, so that it is not

exchanged.

Changing a Device's prefix in the library does not update the part

names of already placed elements in your drawing.

If Forward&Back Annotation is active, the components are replaced in the

schematic diagram and in the layout at the same time.

You will find further information on the program's help pages.

After any library update, please carry out both an ERC on the

schematic and a DRC on the layout!

Individual components can, for instance, be updated with the aid of the ADD

command. If you use ADD to fetch a modified component from a library, you

will be asked whether all the older definitions of this type should be updated.

After the update you can delete the component that you just fetched. Again

here it is wise to carry out an ERC and a DRC after the update!

6.9 Differential Pairs And Meanders

Routing Differential Pairs

A Differential Pair consists of two signals that have the same name, but

different name extensions. One of the signals must have the extension _P, the

other one _N, as for example in CLOCK_P and CLOCK_N. The two signals

must belong to the same net class.

The following particularities apply:

As soon as you select an airwire of a Differential Pair with the ROUTE

command, both signals are routed in parallel. The distance between the two

signals and the wire and via sizes are always determined by the signals' net

class.

The option Auto set route width and drill in the menu Options/Set/Misc

does not affect differential pairs.

If you don't want to route both signals for the whole distance, you can drop

the second airwire with the Escape key.

The first mouse click with the active ROUTE command onto one of the

airwires of the differential pair decides about the starting point of the parallel

routing. Usually the pads or SMDs the airwires start from don't have the

necessary distance for parallel routing, so EAGLE draws traces from the

starting points to the current mouse cursor position, according to the current

wire bend style. Note that there may be cases where these wires overlap, so

189

6 From Schematic to Finished Board

please make sure you choose a proper point from where to start the actual

parallel routing. It can be wise to run a Design Rule Check in this area.

The distance between the target pads/SMDs will also be probably more than

the Differential Pair is routed with, so you should start the routing from this

side as well and define the ending point of the parallel routing, as you did

before at the starting point. If you route towards the wire end points of a

Differential Pair in a different layer, and the wires are fully aligned, the

proper vias will be generated automatically.

Differential Pairs can only be routed manually. The Follow-me

router and the Autorouter treat them like regular signals.

The special functions Shift + left click that places a via at the end point and

Ctrl + left click for defining an arc radius don't work in Differential Pair

mode. When you start routing at any point of a signal (with Ctrl + left click)

you will route the selected signal only, and not the Differential Pair the signal

might be part of.

Coordinates given in the command line while routing a Differential Pair form

a center line along which the actual signal wires are placed left and right with

the proper distance.

Meanders

Length Balance for a Differential Pair

In most cases the traces of a differential pair will have different lengths

although you tried to route them in parallel. The MEANDER command can

be used to balance the lengths of signals forming a differential pair. To do

this, activate the MEANDER command, click onto one of the differential pair

wires, and move the mouse cursor away from the selection point. The

190

➢

Differential Pair follows the mouse cursor

6.9 Differential Pairs And Meanders

distance from the initial selection point and the deflection of the mouse

determines the width and the height of the meander. If there is a difference

in the length of the two signals, and the current mouse position is far enough

away from the selection point, a meander shaped sequence of wires will be

drawn. The meander increases the length of the shorter signal segment.

An indicator attached to the mouse cursor shows the target length which is

the length of the longer signal segment, as well as the deviation in percent of

both signals from the target length.

If a single meander isn't enough to balance the lengths, you can add further

meanders at different locations.

Specifying a Certain Length

In case you want to specify a certain length for the Differential Pair signals,

you can type in the value, for example 9.5in, in the command line directly.

Type in the value, press the Enter key and click onto on of the Differential

Pair wires. Again, the position of the mouse determines the way the meander

looks like.

When meandering a differential pair with a given target length, the meander

first tries to balance the length of the two signal segments that form the

differential pair, and then increases the total length of both segments.

To reset the target length you can either restart the MEANDER command or

enter a value of 0 in the command line.

It's possible to do this for a segment of any signal, not only for

Differential Pairs.

Symmetric and Asymmetric Meanders

By default a meander is generated symmetrical, which means it extends to

both sides along the selected wire. If this is not what you need (either because

there is only space on one side, or because the longer one of the wires of a

differential pair shall not be elongated you can switch to asymmetric mode by

clicking the right mouse button. The actual mouse position will decide which

side of the wire the meander extends to. Move the mouse around to find the

proper position.

The value for Gap factor for meanders in differential pairs which can be set

in the Design Rules' Misc tab, determines the size of the gap between

meander's loops. Increasing the value results in bigger gaps between the

loops. The factor may have values from 1 up to 20. Default: 2.5

Length Tolerance Display

The value defined in Design Rules, Misc tab for Max. length difference in

differential pairs is used to select the color when displaying the length

deviations while drawing a meander. If the percentage is shown in green, the

respective segment lies within the given tolerance. Otherwise the percentage

is displayed in red. The default for this parameter is 10mm.Measuring signal

lengths

191

6 From Schematic to Finished Board

If you click on a signal wire with the Ctrl key pressed, the length of that signal

segment will be measured and displayed on the screen in a little indicator

near the mouse cursor. You can use this to measure the length of a given

signal segment and it as the target length for meandering an other segment.

If you do the measuring with Ctrl+Shift pressed, the maximum length of this

or any previously selected segments will be taken. This can be used to

determine the maximum length of several bus signals and then meandering

each of them to that length.

6.10 Assembly Variants

If you would like to have your project manufactured in different assembly

variants, EAGLE helps you in creating and managing them. Basically an

assembly variant offers the opportunity to have components not populated

on the board or to use components with different values or with different

technologies.

Creating Assembly Variants

As soon as you have finished your project, or at least the schematic, you can

define assembly variants. The default assembly variant (which is the

schematic/layout you just finished) should already contain all the

components which will be used in the different assembly variants. Based on

the default variant open the Assembly Variants dialog through the menu

entry Edit/Assembly variants.... This dialog shows all the components with

its name, value, technology, and the description of the device.

Click onto the New button in order to define an assembly variant. It will be

shown in the Assembly variants window then. Its name is visible in the title

bar. Below you find three columns: A check box, value, and technology.

If the check box is checked, the component will be populated. If you want it

not to be populated, uncheck it. If not populated, the component will be

crossed out in the schematic drawing. This indicates: not available in this

192

➢

Target length 5.125 inch: currently both signals have 93.3%

6.10 Assembly Variants

variant. Simultaneously in the Layout Editor all the objects representing the

silkscreen print for this element will be deleted.

If you would like to change the value of a component, click into the

appropriate field of the Value column, and type in the new value. By default,

all fields remain empty which means that there is no change compared to the

default assembly variant. You are allowed to alter the value of components

which have Value set on for the Device in the library. This setting is typically

used, for example, for resistors or capacitors.

If a component is defined in different technologies, you are allowed to change

it in the Technology column. If there is no technology defined, you can't

change it.

The image above shows besides the default assembly variant on the left with

its columns Name, Value, Technology, and Description two additional

variants. In Variante1 one component (C5) is not populated, some of the

components have altered values. In Variante2 two components will not be

populated. Cells without entry indicate that there are no changes compared

to the default assembly variant.

Click onto the name of the variant in the title bar of the table and it will be

shown in bold text. This indicates that this variant is currently selected. The

buttons Rename... and Delete... affect this variant now.

193

➢

Assembly variants window

6 From Schematic to Finished Board

After defining assembly variants, the action toolbar of the Schematic and

Layout Editor contain an additional selection combo box. The image above

shows Variant2 selected. Two components won't be populated. They are

crossed out in the schematic.

The commands ADD, CHANGE PACKAGE | TECHNOLOGY, REPLACE,

UPDATE and VALUE can only be used, if the default assembly variant is

active. That's the entry without name in the combo box of the action toolbar.

The EXPORT PARTLIST command creates data for the currently selected

assembly variant. If you use bom.ulp for creating the bill of materials, you

can choose the variant in the ULP's dialog. Unpopulated components will not

appear in the parts list.

Assembly Variants and CAM Processor

If you want to create manufacturing data with the CAM Processor be sure to

select the applicable assembly variant in the schematic before and save your

project. The board is also saved in this variant then and the CAM processor

can create data from this.

The information about assembly variants is available only in the

schematic. For boards without a schematic assembly variants are

not supported.

The recommended procedure is to set the variant in the schematic and save

schematic and board. Then run the CAM Processor.

194

➢

Action Toolbar with combo box for assembly variant

6.10 Assembly Variants

In boards without schematic it is possible to change the Populate option of

components via the CHANGE command or via the properties dialog.

6.11 Print Out Schematic and Layout

Schematic diagrams, boards and also library elements can be printed out

with the PRINT command.

Using DISPLAY you should first select the layers that you want to print.

The basic rule is: If you can see it in the editor, you will see it on the

print.

Exceptions to the rule above are:

Origin crosses for texts

Grid lines or grid dots

Polygons that can't be calculated by RATSNEST and therefore only

show their contours in the Layout Editor

Error polygons of the Design Rule Check

Settings of the Print Dialog

When the printer icon on the action toolbar is clicked, the PRINT dialog

opens.

195

➢

The PRINT window

6 From Schematic to Finished Board

The currently selected printer is shown at the top of the window in the

Printer line. The small button on the right, at the end of the line, can be used

to select another printer or activate one of the print-to-file options. If a

printer is selected, the button with the three dots ... leads you to the printer

properties.

In case you selected a print-to-file option the Output file line shows the path

to the output file. If you want to change it, click onto the … button.

Below these two lines you will find settings about Paper format, Orientation

and Alignment of your print. The … button in the Paper line allows you to

define a user-specific format, provided the selected printer supports this.

Alignment defines the location of the print-out on the paper. Changing this

will directly result in a modified Preview, if active.

In the Area line, you determine what to print: Window prints the drawing

window which is currently visible in the Editor window. Full on the other

hand, prints the whole drawing. In this case all drawing objects (displayed or

not) are relevant for the calculation of the resulting printing area.

Printing Options

Mirror inverts the drawing from left to right about the Y axis, Rotate turns it

90 degrees counter-clockwise, and Upside down turns it through 180

degrees. If both are activated, a rotation of 270 degrees is the result.

If the Black option is chosen, a black-and-white printout is made. Otherwise

the print will be either in color or gray scale, depending on the printer.

Solid causes each object to be entirely filled. If you want to see the different

filling patterns of the individual layers, then deactivate this option.

The Caption option switches the appearance of the title, printing date, file

name and the scale of the print on or off.

In the Scale section of the window the Scale factor specifies the scale of the

drawing. It may be in the range of 0.001 and 1000.

If Page limit is set to 0, the printer will use whatever number of pages is

needed to print the output at the selected scale. If a different value is

selected, EAGLE will adjust the scale of the drawing to fit it onto the stated

number of pages. This can mean that, under unfavourable circumstances, the

selected scale cannot be maintained.

Otherwise you have the possibility to select Page Limit 1, and a Scale factor

that would request more than one page for printing to get a maximum filling

of the page.

It is possible to select which sheets from a schematic diagram are printed

using the Sheets box. This only appears in the Schematic Editor. This

selection also determines which sheet is shown in the preview.

If you activate the option Hierarchy, all the module sheets for each module

instance used in the schematic will be printed with the corresponding part

names, net names and assembly variants.

The edges of the print can be defined with the aid of the four entry boxes

under Border. The values may be entered in mm or in inches. If you have

changed the values and want to use the printer driver's standard settings

again, simply enter a 0.

196

6.11 Print Out Schematic and Layout

Calibrate allows correction factors for the aspect ratio of the printout. This

allows linear errors in the dimensional accuracy of the print to be corrected.

The values can be specified in the range of 0.1...2.

Note concerning colored printing:

EAGLE always takes the white palette as basis for colored printouts.

If you are working with a black or colored background and using

self-defined colors, it is recommended to define these colors also for

the white palette. So the printer can use your colors, too.

If, when a layout is printed, the drill holes in the pads and vias are not to be

visible, select the No Drills option for the Display mode by way of the menu

item Options/Set/Misc.

Generating PDF files

If you want to generate a PDF file (resolution 1200dpi) from your drawing,

click onto the small selection button in the Printer line and choose the option

Print to file (PDF). Go to the Output file line then and specify path and name

of the PDF output file.

All texts that are not written in EAGLE vector font are searchable in the PDF

file by means of your PDF viewer.

Visibility and Sequence of Printed Layers

EAGLE prints its layers in a certain sequence, one over the other. If you are

using, for example, self-defined layers that are hidden by other layers in the

print-out, you can use a SET command option – SET Option.LayerSequence

– for bringing them into the foreground, or in general, for defining the layer

printing sequence. This affects printing into a PDF file, as well.

Details about this can be found in the help function of the SET command,

Help/Editor commands/SET.

The PRINT command can also be given directly on the command line, or can

be run by a script file. Information about the selection of options is available

on the help pages for PRINT.

6.12 Combining Small Circuit Boards on a

Common Panel

In order to save costs, it may be worth supplying, for example, a smaller

board to the board manufacturer in the form of a multiple board. So you can

have several boards made in one step.

You can reproduce the layout or combine different layouts to create a

multiple board with the GROUP, COPY and PASTE commands. Please note

that this will change the board's silk screen, since elements receive new

names, if a certain designator is already used in the board when pasting from

the buffer. If you don't need the silkscreen this does not matter. Otherwise a

User Language program can help. Panelize.ulp copies the texts written in the

layers 25 and 26 (t/bNames) into two new layers 125 and 126. When

combining the boards the names of the parts will change anyway, the copied

texts in those new layers however will remain unchanged.

197

6 From Schematic to Finished Board

Tell the board manufacturer that they have to take layers 125 and 126 instead

of the original layers 25 and 26 to generate the silkscreen from.

Procedure:

Load the board file.

Run panelize.ulp to copy name texts.

DISPLAY all layers.

Use GROUP to select all objects to be copied.

To select the whole layout you could also use GROUP ALL.

Click the COPY icon in order to put the group into the clipboard

Edit a new board file with File/New .

Use PASTE and place the layout as often as wanted. If necessary, it is

possible to specify an orientation for the group before fixing it.

Please make sure that the new board has the same set of Design Rules

as the original board file has. It is possible to export Design Rules into

a file (*.dru) and then import it into another board file (Edit/Design

rules menu, File tab).

Save the new board file.

Tell your board house that they have to use layers 125/126 instead of

25/26.

6.13 Consistency Lost between Schematic

and Layout

It is very important during the design that the content of the schematic and

the layout exactly correspond to allow for design congruency. Eagle uses a

Forward&Back annotation to perform this task. General information about

this can be found in the chapter about Forward&Back Annotation beginning

with page 103.

The interconnection between Schematic Editor and Layout Editor ensures

that both are in lock-step from a design standpoint automatically, provided

both files are always loaded at the same time. If you close one of them, either

the schematic or layout file, and continue your work in the remaining opened

file the consistency will be lost. EAGLE will not be able to transfer the

modifications into the other file. So differences will arise between Schematic

and Layout.

In case you close one of the two editor windows EAGLE prompts an eye-

catching yellow and black warning on top of the drawing area which tells you

that Forward&Back Annotation has been severed. Please reload the file

again.

In case you severed F&B Annotation intentionally, you can hide this warning

by clicking into the message area.

198

6.13 Consistency Lost between Schematic and Layout

EAGLE will prompt a similar warning as soon as you try to load a pair of

schematic/board files or a project which is not consistent.

Start the Electrical Rule Check (ERC) immediately. It compares both files

and reports differences in the ERC Errors window's Consistency Errors

branch. If you click onto one of these entries, EAGLE marks the affected

object in Schematic and Board, if possible.

Process each message and resolve the difference in the Schematic or in the

Layout Editor window, according to requirements. Finally you can mark the

entry in the list as done with the Processed button.

For establishing consistency again it can be helpful to use UNDO.

Launch the ERC every time a change has been made for design verification

and to get an overview of progress. All differences are cleared, if ERC reports

consistency. Now the Annotation will work again and the board and

schematic are again in lock-step with each other.

199

➢

Forward&Back Annotation severed!

➢

Consistency loss between Schematic and

Layout

6 From Schematic to Finished Board

➢

The differences are marked in both editor windows

Don't forget to save the files now and remember to leave both files loaded

simultaneously all the time.

Criteria For Consistency

There are some rules that have to be fulfilled in order to have consistency

between schematic and layout and the Forward&Back Annotation working.

In the following list there are mentioned the most important items:

Each component in the schematic has to have a corresponding

package in the layout and vice versa. Exceptions are supply symbols,

elements without contacts, and components with an attribute with

the name _EXTERNAL_ (for example for simulation symbols).

☞ Use ADD/DELETE/NAME commands for placing/deleting/

naming components

Corresponding components have to have the same values.

☞ Use the VALUE command in order to adjust the values.

For each connection of net and pin in the schematic there has to be

a corresponding connection with the same name of signal and

referring pad in the layout.

☞ Add the missing net with the NET command, missing signals in

the layout with the SIGNAL command, if necessary use NAME

to adjust signal/net names or DELETE for deleting connections.

Nets in the schematic and signals in the layout have to belong to

identical netclasses.

200

6.13 Consistency Lost between Schematic and Layout

☞ CHANGE CLASS or use the properties dialog of the net/signal

in order to adjust the net classes and their values for width,

clearance and drill.

Assembly variants in schematic and board have to be identical;

There must be the same number of variants and identic variant

names. Additionally the population options of the components have

to be the same.

☞ Use the VARIANT command for adjusting this

If there are attributes defined for components, the attribute name

and the attribute value have to be the same in schematic and board.

It is allowed to have additional attributes defined in the layout

editor which are not available in the schematic, but not vice versa.

☞ Check the ATTRIBUTE command

If there are attributes that are defined in the library, it might be

helpful to use the REPLACE command in order to replace such

components and update the attribute information.

The definition of the package in schematic and board has to be

exactly the same. There are different options in order to eliminate

such discrepancies:

☞ Use the REPLACE command in the layout editor in order to

exchange the package with a definition that matches the

package used in the schematic.

☞ Exchange of a whole device in the schematic editor with the

REPLACE command or replacement of the components with

a package definition used in the layout editor.

Please take care on attributes, as well (see above).

☞ Change the package variant , if any, with CHANGE PACKAGE

in the schematic editor.

If the libraries that contained the components originally used in your

schematic and layout are not available, it might be helpful to export the

library definitions from your drawing files (File/Export menu). Now it is

possible to modify the libraries, if necessary, and use the REPLACE

command.

Consistency Indicator

In the bottom right corner of the editor window you can see an indicator that

gives, depending on its color, information about consistency.

Gray F&B Annotation not possible

Only one file loaded

Yellow F&B Annotation not available

SCH and BRD have different names

Pink F&B Annotation not active

SCH and BRD are not consistent

Green F&B Annotation is active

SCH and BRD are consistent

201

6 From Schematic to Finished Board

The exclamation mark right of the consistency indicator remembers you that

the drawing is currently not saved.

202

➢

Consistency indicator

Chapter 7

The Autorouter

7.1 Basic Features

Any routing grid (min. 0.02 mm)

Any placement grid

Fully integrated into basic program

TopRouter with gridless routing algorithm, which can be preceded by

the Autorouter

BGA router for fan-out routing

Optional automatic selection of routing grid and preferred directions

in the signal layers

Support for multi-core processors to process multiple routing jobs

simultaneously

SMDs are routed on both sides

The whole drawing area can be the routing area (provided enough

memory is available)

The strategy is selected via control parameters

Simultaneous routing of various signal classes with various track

widths and minimum clearances

Common data set (Design Rules) for the Design Rule Check and the

Autorouter

Multilayer capability (up to 16 layers can be routed simultaneously,

not only in pairs)

Support of Blind and Buried vias

The preferred track direction can be set independently for each layer:

horizontal and vertical, true 45/135 degrees (important for inner

layers!)

Ripup and retry for 100 % routing strategy

Optimization passes to reduce vias and smooth track paths

Prerouted tracks are not changed

Serves a basis for the Follow-me router, a special operating mode

of the ROUTE command that allows automatic routing of selected

signals

203

7 The Autorouter

7.2 What Can be Expected from the

Autorouter

The EAGLE Autorouter is a "100%" router. This means that boards which, in

theory, can be completely routed will indeed be 100% routed by the

Autorouter, provided - and this is a very important restriction - the

Autorouter has unlimited time. This restriction is valid for all 100%

Autorouters whatsoever. However, in practice, the required amount of time

is not always available, and therefore certain boards will not be completed

even by a 100% Autorouter.

The EAGLE Autorouter is based on the ripup/retry algorithm. As soon as it

cannot route a track, it removes prerouted tracks (ripup) and tries it again

(retry). The number of tracks it may remove is called ripup depth which is

decisive for the speed and the routing result. This is, in principle, the

previously mentioned restriction.

In the Autorouter main dialog it is possible to choose a TopRouter variant. It

uses a gridless algorithm with topological approach. This algorithm

calculates first the course of the signals and then uses the optimization runs

of the traditional EAGLE Autorouter to meet the Design Rules. Typically, the

TopRouter requires significantly fewer vias than the traditional EAGLE

Autorouter. The user has the option to select both methods for a project and

eventually opt for one or the other routing result.

Those who expect an Autorouter to supply a perfect board without some

manual help will be disappointed. The user must contribute his ideas and

invest some energy. If he does, the Autorouter will be a valuable tool which

will greatly reduce routine work.

Working with the EAGLE Autorouter requires that the user places the

components and sets control parameters which influence the routing

strategy. These parameters must be set carefully if the best results are to be

achieved. They are therefore described in detail in this section.

7.3 Controlling the Autorouter

The Autorouter is controlled by a number of parameters. The values in the

current Design Rules, the net classes and special Autorouter control

parameters all have an effect.

The Design Rules specify the minimum clearances (DRC commands for

setting Clearance and Distance), the via diameter (Restring setting) and the

hole diameter of the vias (Sizes setting). The minimum track width is also

specified.

The net classes - if any are defined - specify special minimum clearances,

track widths and the hole diameters for vias carrying particular signals.

There is also a range of special cost factors and control parameters that can

be changed via the Autorouter menu. They affect the route given to tracks

during automatic routing. Default values are provided by the program. The

control parameters are saved in the BRD file when the layout is saved. You

can also save these values in an Autorouter control file (*.ctl). This allows a

204

7.3 Controlling the Autorouter

particular set of parameters to be used for different layouts. Neither Design

Rules nor the data for various net classes are part of the control file.

A routing process involves a number of separate basic steps:

Bus Router

Normally the bus router starts first.

It deals with signals which can be routed in the preferred direction with only

slight deviation in x and y direction allowed. The bus router takes only those

signals into consideration that belong to net class 0.

This step may be omitted.

Buses, as understood by the Autorouter, are connections which can

be laid as straight lines in the x or y direction with only a few

deviations.

It has nothing in common with buses in the meaning of electronics,

for example, address buses or the like.

Routing Pass

The actual routing pass is then started, using parameters which make a 100%

routing as likely as possible. A large number of vias are deliberately allowed

to avoid paths becoming blocked.

TopRouter

Select a routing variant with upstream TopRouter, and the traces will be laid

out with another routing algorithm, which tends to use less vias. Finally

routing and optimization follows in order to trim all the traces to comply

with the design rules.

Optimization

After the main routing pass, any number of optimization passes can be made.

The parameters are then set to remove superfluous vias and to smooth the

track paths. In the optimization passes tracks are removed and rerouted one

at a time. This can, however, lead to a higher degree of routing, since it is

possible for new paths to be freed by the changed path of this track.

The number of optimization passes must be specified before starting the

Autorouter. It is not possible to optimize at a later stage. Once the routing job

has been completed all the tracks are considered to have been prerouted, and

may no longer be changed.

Any of the steps mentioned above may be separately activated or deactivated.

205

7 The Autorouter

7.4 What Has to be Defined Before

Autorouting

Design Rules

The Design Rules need to be specified in accordance with the complexity of

the board and of the manufacturing facilities available. You will find a

description of the procedure and of the meanings of the individual

parameters in the section on Specifying the Design Rules on page 144.

Track Width and Net Classes

If you have not already defined various net classes in the schematic diagram

you now have the opportunity, before running the Autorouter, of specifying

whether particular signals are to be laid using special track widths, particular

clearances are to be observed, or whether certain drill diameters are to be

used for vias for particular signals. Please consult the help pages (CLASS

command) or the section on Specifying Net Classes on page 123 for

information about the definition of net classes.

If no special net classes are defined, the values from the Design Rules apply.

The value Minimum width in the Sizes tab determines the track width, the

values for minimum clearances/distances are taken from the Clearance and

Distance tabs. The diameter of vias is defined by the values in the Restring

tab.

Did you set values in the Design Rules and for net classes? In this

case the Autorouter follows the higher value.

Grid

The Design Rules determine the routing and placement grid. The minimum

routing grid is 0.02 mm, which is about 0.8 mil.

Placement Grid

Although the Autorouter does permit any placement grid, it is not a good

idea to place the components on a grid that is too fine. Two good rules are:

The placement grid should not be finer than the routing grid.

If the placement grid is larger than the routing grid, it should be set to

an integral multiple of the routing grid.

These rules make sense if, for example, you consider that it might be

possible, within the Design Rules, to route two tracks between two pins of a

component, but that an inappropriate relationship between the two grids

could prevent this (see diagram).

206

7.4 What Has to be Defined Before Autorouting

Routing Grid

Please note that the Autorouter grid has to be set in the AUTO command's

Autorouter Main Setup Window. This is not the same as the currently used

grid in the Layout Editor window that you have selected with the GRID

command.

Bear in mind that for the routing grid the time demand increases

exponentially with the resolution. Therefore select as large a grid as possible.

The main question for most boards is how many tracks are to be placed

between the pins of an IC. To answer this question, the selected Design Rules

(i.e. the minimum spacing between tracks and pads or other tracks) must of

course also be considered.

The result is:

The two grids must be selected so that component's pads are located

on the routing grid.

There are of course exceptions, such as with SMDs to which the opposite may

apply, namely that a position outside of the routing grid leads to the best

results. In any event the choice of grid should be carefully considered in the

light of the Design Rules and the pad spacing.

The example above may clarify the situation:

For the component on the left, the pads are placed on the routing grid. Two

tracks can be routed between two pads. The pads of the component in the

middle are not on the routing grid, and therefore only one track can be

routed between them.

On the right you see the exception from the rule shown for SMD pads, which

are placed between the routing grid lines so that one track can be routed

between them.

When choosing the grid, please also ensure that each pad covers at least one

grid point. Otherwise it can happen that the Autorouter is unable to route a

signal, even though there is enough space to route it. In this case the

Autorouter issues the message Unreachable SMD at x y as it starts. The

parameters x and y specify the position of the SMD pad.

207

➢

Track patterns with different placement grids

7 The Autorouter

The default value for the routing grid is 50 mil. This value is sufficient for

simple through-hole layouts. Working with SMD components demands a

finer routing grid.

Usual values are 25, 12.5, 10, or 5 mil.

Please remember that finer routing grids require significantly more

routing memory.

With the automatic grid selection option, the auto router determines at its

own heuristics suitable grid settings for each routing jobs.

Memory Requirement

The amount of routing memory required depends in the first place on the

selected routing grid, the area of the board and the number of signal layers in

which tracks are routed.

The static memory requirement (in bytes) for a board can be calculated as

follows:

)KV=H=&"x)KV"=!!8"x.

Space is also required for dynamic data, in addition to the static memory

requirement. The dynamic data require in a very rough estimate about 10%

up to 100% (in some cases even more!) of the static value. This depends

heavily on the layout.

Total memory requirement (rough approximation):

"&G8x@-$-$$.30B/K8&"2

This much RAM should be free before starting the Autorouter. If this is

insufficient, the Autorouter must store data on the hard disk. This lengthens

the routing time enormously, and should be avoided at all costs. Short

accesses to the hard disk are normal, since the job file on the hard disk is

regularly updated.

Try to choose the coarsest possible routing grid. This saves memory

space and routing time!

Layer

If you want to design a double-sided board, then select Top and Bottom as

route layers. You should only use the Bottom layer for a single-sided board.

In the case of inner layers, it is helpful to use the layers from the outside to

the inside, i.e. first 2 and 15 and so on.

In the case of boards that are so complex that it is not certain whether they

can be wired on two sides, it is helpful to define them as multilayer boards,

and to set very high costs for the inner layers. This will cause the Autorouter

to avoid the inner layers and to place as many connections as possible in the

outer layers. It can, however, make use of an inner layer when necessary.

These settings are made in the Autorouter menu (see page 210).

208

7.4 What Has to be Defined Before Autorouting

The autorouter shows the message Unreachable SMD in layer..., if a layer

that contains SMDs is not active. Clicking OK starts the autorouter

nevertheless. If you want to change the autorouter setup click Cancel.

Preferred Directions

For each routing job you can specify individually for each signal layer its own

preferred direction. With the new Auto setting the Autorouter will choose

different settings for preferred directions on its own.

If you want to set preferred directions manually, the following considerations

apply: On the two outside layers the preferred directions are normally set to

90 degrees from each other. For the inner layers it may be useful to choose

45 and 135 degrees to cover diagonal connections. Before setting the

preferred direction it is well worth examining the board (based on the

airwires) to see if one direction offers advantages for a certain side of the

board. This is particularly likely to be the case for SMD boards.

Please also follow the preferred direction when pre-placing tracks.

The defaults are vertical for the Top (red) and horizontal for the

Bottom (blue) layer.

Experience has shown that small boards containing mainly SMD components

are best routed without any preferred direction at all (set * in the Autorouter

setup). The router then reaches a usable result much faster.

Single sided boards should be routed without a preferred direction.

Restricted Areas for the Autorouter

If the Autorouter is not supposed to route tracks or place vias within certain

areas, you can define restricted areas by using the commands RECT,

CIRCLE, and POLYGON in the layers 41, tRestrict, 42, bRestrict, and 43,

vRestrict.

tRestrict: Restricted areas for Wires and Polygons in the Top layer.

bRestrict: Restricted areas for Wires and Polygons in Bottom

layer.

vRestrict: Restricted areas for Vias.

Such restricted areas can already be defined in a Device or Package (around,

for instance, the fixing holes for a connector, or for a flat-mounted transistor

under which there should not be any tracks).

Wires drawn in layer 20, Dimension, are boundary lines for the Autorouter.

Tracks cannot be laid beyond this boundary.

Typical application: board boundaries.

An area drawn in layer 20 can also be used as a restricted region for all

signals. It should, however, be noted that this area should be deleted before

sending the board for manufacture, since layer 20 is usually output during

the generation of manufacturing data.

Cutout polygons which are used, for example, in inner layers in order to keep

certain areas of signal polygons free of copper, are not recognized by the

Autorouter. It may happen that the Autorouter draws wires in such an area.

209

7 The Autorouter

Cost Factors and Other Control Parameters

All routing parameters are set in the Autorouter Variants dialog. They can be

modified separately for each routing variant.

The default values for the cost factors are chosen on the basis of our

experience in such a way as to give the best results.

The control parameters such as mnRipupLevel, mnRipupSteps etc. have also

been set to yield the best results according to our experience.

We want to emphasize, that we recommend working with the default values.

If you nevertheless do want to experiment with these parameters, please

consider the description of the cost factors in the following section. In the

case of many parameters even small alterations can have large effects.

7.5 The Autorouter Menu

When running the Autorouter with the AUTO command, the setup menu

appears first. All the necessary settings are made there.

Autorouter Main Setup

This is where you specify the layers that may be used for routing and which

preferred directions apply. Click in the appropriate combo box with the

mouse, and select the desired value.

Setting the preferred directions:

- horizontal

| vertical

/ diagonal at 45°

\ diagonal at 135°

* none

210

➢

Autorouter main setup: General settings

7.5 The Autorouter Menu

auto automatic setting

Setting Effort (Low, Medium or High) determines how many routing

variants can be created.

If the automatic grid selection is on, the auto router chooses its own values.

Turn off this option to choose your own suitable routing grid. There is the

opportunity to examine the (automatically) selected grid settings and modify

them later in the routing variants dialog.

Variant with TopRouter activates the new TopRouter that calculates the

layout with another routing algorithm. Typically, the computational effort is

larger, but usually provides smoother results with fewer vias.

The maximum number of running threads can be limited. The EAGLE

Autorouter supports the calculation of multiple Autorouter jobs at a time by

using multi-core processors. The indicated value depends on the number of

available processor cores. It may be useful to reduce the number of threads in

order not to occupy all processor cores with the EAGLE Autorouter.

You may use the Load... and Save as.... buttons to load a different parameter

set from an Autorouter control file (*.ctl) or to save the current settings for

further projects.

Select this by clicking the corresponding signal lines.

Clicking onto the Select button allows certain signals to be selected for

autorouting. Select these with a mouse click onto the respective airwires.

Then click on the traffic-light icon in the action toolbar in order to open the

second part of the Autorouter setup; the routing variants dialog. There you

can check the configuration of the routing jobs and change some settings

before the actual routing process begins.

It is, alternatively, possible to enter the signal names on the command line.

Examples:

:5

The signals VCC and GND will be routed.

The semicolon at the end of the line starts the Autorouter immediately. It is

alternatively possible to click on the traffic-light icon.

If you type in the command line

Z:5

all signals except VCC and GND will be routed.

You may use wildcards for the signal selection, as well. Allowed is

*which matches any number of any characters.

?which matches exactly one character.

[…] which matches any of the characters between the brackets,

for example [a-f], for all characters from a to f.

Routing Variants Dialog

Click Continue... and a number of different routing variants are calculated,

The Routing Variants Dialog opens.

211

7 The Autorouter

Here you can modify the parameter set of each variant or delete or add

variants in the list. Each parameter set corresponds to the known Autorouter

parameter set from the previous versions of EAGLE.

The calculation of the individual routing variants (routing jobs) is started

from this dialog.

Depending on the settings EAGLE shows a number of routing options for the

board. Click the Start button and the Autorouter starts processing the routing

variants.

If you would like to check and maybe adjust the individual routing

parameters before, click the >> button.

In the advanced options dialog you can review and modify the routing

parameters. Click Duplicate or Delete, in order to copy or delete the selected

variant.

The parameters grouped in the sections Layer costs, Cost factors and

Maximum can be set individually for each pass (Busses, Route, Optimize 1-

4). For more information, see the following section.

You can insert additional optimization passes by clicking the Add button in

the last optimization run.

The Autorouter starts for all the signals that have not yet been laid out by

clicking on the OK button.

212

➢

Autorouter: List of Routing Variants

➢

Autorouter Variants: List and Parameter settings

7.5 The Autorouter Menu

The Cancel menu button interrupts the AUTO command without storing any

changes.

You are not allowed to make any changes to the parameters, if you want to

restart an interrupted routing job. Use the Continue existing job check box to

decide whether you want to continue with an existing job, or whether you

want to choose new settings for the remaining unrouted signals.

➢

Autorouter Main Setup: Restarting an

interrupted job

The Autorouter's work can be undone by the UNDO command.

7.6 How the Cost Factors Influence the

Routing Process

Values between 0..99 are possible for each cost factor (cfxxx), but the full

range is not useful for all parameters. Sensible values are therefore given

with each parameter.

The control parameters (mnxxx) accept values in the range 0..9999.

Reasonable figures are also provided under each parameter.

The parameter can be set by the Autorouter Setup Menu. The settings for

Route and the Optimize passes can be configured separately. The menu is

split into three sections, Layer Costs, Costs, Maximum.

213

7 The Autorouter

➢

Autorouter: Parameter for Route

The following section shows the available parameters and their effects. The

names of the parameters are the same as they would be used in an

Autorouter control file *.ctl. Details about this can be found in Parameters of

a Control File beginning with page 221.

Layer Costs

cfBase.xx: 0..20

Base costs for one step on the corresponding layer. Recommendation:

outside layers (Top, Bottom) always 0, inside layers greater than 0.

Costs

cfVia: 0..99

Controls the use of vias. A low value produces many vias but also allows the

preferred direction to be followed. A high value tries to avoid vias and thus

violates the preferred direction. Recommendation: low value for the routing

pass, high value for the optimization.

cfNonPref: 0..10

Controls following of the preferred direction. A low value allows tracks to be

routed against the preferred direction, while a high value forces them into

the preferred direction.

If cfNonPref is set to 99, track sections can only be placed in the preferred

direction. Only select this value if you are certain that this behaviour is really

wanted.

cfChangeDir: 0..25

Controls how often the direction is changed. A low value means many bends

are allowed within a track. A high value produces virtually straight tracks.

214

7.6 How the Cost Factors Influence the Routing Process

cfOrthStep, cfDiagStep

Implements the rule that the hypotenuse of a right-angled triangle is shorter

than the sum of the other two sides. The default values are 2 and 3. That

means that the costs for the route using the two other sides are 2+2, as

against 3 for the hypotenuse. These parameters should be altered with great

care!

cfExtdStep: 0..30

Controls the avoidance of track sections which run at an angle of 45 degrees

to the preferred direction, and which would divide the board into two

sections. A low value means that such sections are allowed while a high value

tries to avoid them. In combination with the parameter mnExtdStep you can

control the length of these tracks. If mnExtdStep = 0, each grid step at 45

degrees to the preferred direction causes costs that are defined in parameter

cfExtdStep. Choosing for example mnExtdStep = 5 allows a track to run five

steps at 45 degrees without any additional costs. Each further step causes

costs defined in cfExtdStep.

In this way, 90 degree bends can be given 45 degree corners. Settings like

cfExtdStep = 99 and mnExtdStep = 0 should avoid tracks with 45 degree

angles.

This parameter is only relevant to layers which have a preferred direction.

Recommendation: use a lower value for the routing pass, and a higher value

for the optimization.

cfBonusStep, cfMalusStep: 1..3

Strengthens the differentiation between preferred (bonus) and bad (malus)

areas in the layout. With high values, the router differentiates strongly

between good and bad areas. When low values are used, the influence of this

factor is reduced. See also cfPadImpact, cfSmdImpact.

cfPadImpact, cfSmdImpact: 0..10

Pads and SMDs produce good and bad sections or areas around them in

which the Autorouter likes (or does not like) to place tracks. The good areas

are in the preferred direction (if defined), the bad ones perpendicular to it.

This means that tracks which run in the preferred direction are routed away

from the pad/SMD. With high values the track will run as far as possible in

the preferred direction, but if the value is low it may leave the preferred

direction quite soon.

It may be worth selecting a somewhat higher value for cfSmdImpact for

densely populated SMD boards.

cfBusImpact: 0..10

Controls whether the ideal line is followed for bus connections (see also

cfPadImpact). A high value ensures that the direct line between start and

end point is followed. Only important for bus routing.

215

7 The Autorouter

cfHugging: 0..5

Controls the hugging of parallel tracks. A high value allows for a strong

hugging (tracks are very close to each other), a low value allows for a more

generous distribution. Recommendation: higher value for routing, lower

value for the optimization.

cfAvoid 0..10

During the ripup, areas are avoided from which tracks were removed. A high

value means strong avoidance.

Not relevant to the optimization passes.

cfPolygon 0..30

If a polygon has been processed with the RATSNEST command and therefore

is displayed as a filled area before you start the Autorouter, every step within

the polygon is associated with this value. A low value makes it easier for the

Autorouter to route traces inside the polygon area. The probability, however,

that the polygon is broken into several pieces is higher. A higher value causes

the Autorouter to make fewer connections inside the polygon.

If a polygon is in outline mode and not processed by RATSNEST before you

start the Autorouter, it won't be taken into consideration at all. cfPolygon

does not play a role for such polygons.

Maximum

mnVia 0..30

Controls the maximum number of vias that can be used in creating a

connecting track.

mnSegments 0..9999

Determines the maximum number of wire pieces in one connecting track.

mnExtdSteps 0..9999

Specifies the number of steps that are allowed at 45 degrees to the preferred

direction without incurring the value of cfExtdStep.

See also page 283.

262

8.3 Defining a Complex Device

The Connect Command

This must be the most important step in the library definition. CONNECT

assigns each pin to one ore more pads. The way in which nets in the

schematic diagram are converted into signal lines in the layout is defined

here. Each net at a pin creates a signal line at a pad. The pin assignment for

the 541032 is specified in the data sheet. Check the connects in the library

with care. Errors that may pass unnoticed here can make the layout useless.

Select the J version from the Package list and click the CONNECT button.

The connect window opens.

➢

CONNECT dialog

The list of pins is on the left, and the pads are in the center. Click onto a pin-

entry, and select the associated pad. Both entries are now marked. You join

them with the connect button. This pair now appears on the right, in the

Connection column. Join each pin to its pad in accordance with the data

sheet. Finish the definition by clicking OK.

Please note that in our example the Gates are named A, B, C, and D while

they are named 1, 2, 3, and 4 in the data sheet.

263

➢

The pin assignment for the

packages

8 Component Design Explained through Examples

Define the connections for the second Package version, FK, in the same way.

Select the version, and click the Connect button. The usual dialog appears in

the connect window. Proceed exactly as described above.

Please note that six pads are not connected in this version. They are left over

in the Pad column. Finish the process by clicking OK.

There is now a green tick to the right of both Package variants, and this

indicates that connection is complete. This is only true when every pin is

connected to a pad.

It is not possible to connect several pins with a common pad!

A Device may contain more pads than pins, but not the other way

around!

Pins with direction NC (not connected) must be connected to a pad,

as well!

In the section 8.5 beginning with page 268 is explained how to use

the Append button of the Connect dialog in order to connect one pin

with more than one pad.

Defining Technologies

As noted above, the 541032 is to be used in two different technologies AS and

ALS. By including a * as a placeholder in the Device name we have already

taken the first step towards this. In the schematic diagram the code for the

chosen technology will appear instead of the *. The data sheet shows that

both technologies are available in both Packages.

Select the J Package from the list on the right of the Device Editor window.

Then click onto Technologies in the description box. The technologies

window opens. Define the technology in the New line, and confirm the entry

with OK. When the entry has been completed, the AS and ALS entries are

activated with a tick.

Close the window by clicking OK again.

Select the FK version from the Package list. Click onto Technologies in the

description box again. You will now see that AS and ALS are available as

selections in the technologies window. Activate both of these by clicking into

the small box to the left, so that a tick is displayed. Finish the definition by

clicking OK.

264

➢

Technologies for package

variant J

8.3 Defining a Complex Device

The technologies available for the selected Package version are now listed in

the description area of the Device Editor.

Specifying the Prefix

The prefix of the Device name is defined simply by clicking on the Prefix

button. IC is to be entered in this example.

Value

The setting of value determines whether the VALUE command can be used

to alter the value of the Device in the schematic diagram and in the layout.

On: You are allowed to change the value in the schematic (for example

for resistors). Defining the value is necessary to specify the part.

Off: The value will be generated from the Device name which can

include technology and Package variant name (e.g. 74LS00N).

Even if Value is set Off, it is possible to change the value of a component after

confirming a warning message.

If you change the initial value and decide to use another Technology or

Package variant later with CHANGE PACKAGE or CHANGE TECHNOLOGY,

the user-defined value will remain unchanged.

Independently from the Value settings mentioned above, it is allowed to

define an attribute with the name VALUE and assign any attribute value.

This attribute value will be finally used in schematic and board.

Description

Click onto Description in the description box. You can enter a description of

the Device in the window which now opens. Use typical terms that you might

apply for a keyword search. The search facility of the ADD command in the

schematic diagram will also search through this text.

You can use HTML text. The syntax is described in the help system under the

keyword HTML Text.

The description can look like this:

QK?9;-01.Q'K?

QH?

U))H!.H)&"=GM+)["'5=M"

V$

265

8 Component Design Explained through Examples

Save

This completes definition of the Device set. If you have not already saved the

library, please do it at this stage!

8.4 Supply Voltages

Component Power Supply Pins

The components' supply pins are to be given the direction Pwr in the Symbol

definition. The pin name determines the name of the supply signal. Pins

whose direction is Pwr and which have the same name are automatically

wired together (even when no net line is shown explicitly). Whether the pins

are visible in the schematic diagram or are fetched by means of a hidden

Symbol is also not relevant.

Invisible Supply Pins

We do not want as a rule to draw the supply connections for logic

components or operational amplifiers in the schematic. In such a case a

specific Symbol containing the supply connections is defined. This can be

demonstrated with the example of a 7400 TTL component:

You first define a NAND gate with the name 7400, and the following

properties in the Symbol Editor:

The two input pins are called I0 and I1 and are defined as having direction

In, Swaplevel 1, visible Pin and function None.

266

➢

Device Editor: 54*1032A.dev

8.4 Supply Voltages

The output pin is called O and is defined with direction Out, Swaplevel 0,

visible Pin, and function Dot.

Now define the supply gate with the name PWRN, and the following

properties:

The two pins are called GND and VCC. They are defined with direction Pwr,

Swaplevel 0, function None, and visible Pad.

Now create the 7400 Device in the Device Editor:

Specify the Package with PACKAGE (which must already be present in the

library) and use PREFIX to specify the name prefix as IC.

Use the ADD command to place the 7400 Symbol four times, with Addlevel

being set to Next and Swaplevel to 1. Then label the Gates as A, B, C and D

with the NAME command.

The Addlevel of Next means that as these Gates are placed into the

schematic, they will be used in that sequence, i.e., the sequence in which they

were fetched into the Device.

Then place the PWRN Symbol once, using Addlevel Request and Swaplevel 0.

Name this Gate P.

Addlevel Request specifies two things:

267

➢

NAND Symbol 7400 (European

Representation)

➢

Power gate

8 Component Design Explained through Examples

The supply gate will only be fetched into the schematic if requested,

i.e. with the INVOKE command. The ADD command will only be able

to place NAND gates.

The supply gate will not be included when names are allocated to the

schematic. Whereas an IC with two Next Gates appears in the

schematic as something like IC1A and IC1B, an IC with one Next Gate

and one Request Gate will only be identified as IC1.

So use the CONNECT command to define the housing pads to which the

supply pins are connected.

Pins with the Same Names

If you want to define components having several power pins of the same

name, let's suppose that three pins are all to be called GND, then proceed as

follows:

set pin direction Pwr for each power pin

name these pins GND@1, GND@2, and GND@3

Only the characters in front of the "@" are visible in the schematic, and the

pins are treated as if they were all called GND. In the board the referring

pads are connected with airwires automatically.

8.5 One Pin – Multiple Pads Connections

You are allowed to connect one pin with several pads belonging to a common

signal. This can be done with the help of the Append button in the connect

dialog window.

First mark one pin and one pad in the connect dialog as usual and click onto

the Connect button. The pin/pad connection now appears in the Connection

column.

In order to add a further pad to this connection first mark the connection,

then select the pad in the Pad column, and click onto the Append button.

Repeat this for further pads, if necessary. The names of the pads appended

now are displayed in the Connection column.

EAGLE knows two different ways of creating multiple pad connections:

As soon as you establish a multiple pad connection, a special icon is

displayed in the Connections column, located between Pin and Pad list. It

informs you about the mode: All or Any. Click onto the icon to toggle.

All: All pads must be connected with traces. In the Layout editor you

will see all pads connected with airwires you have to route.

Any: Only one of the pads will be connected by an airwire and has to

be routed. In the routing process it is up to you which pad you

want to connect with a trace. In this mode internal connections

of a device can be realized.

Further information can be found in the help, Editor

Commands/CONNECT.

268

8.6 Supply Symbols

Supply symbols, such as might be used in the schematic for ground or VCC,

are defined as Devices without a Package. They are needed for the automatic

wiring of supply nets (see page 126).

The following diagram shows a GND symbol as it is defined in one of the

supplied EAGLE libraries.

Note that when defining your own supply symbols, the pin and the Device

name need to agree.

The pin is defined with direction sup and has the name GND. This specifies

that the Device containing this Symbol is responsible for the automatic

wiring of the GND signal. The text variable for the value (>VALUE) is chosen

for the labeling. The Device also receives the name GND. Thus the label GND

appears in the schematic, since by default EAGLE uses the Device name for

the value.

It is very important that the labeling reproduces the pin names, since

otherwise the user will not know which signal is automatically connected.

The pin parameter Visible is therefore set to off, since otherwise the placing,

orientation and size of the pin name would no longer be freely selectable.

Directly labeling with the text GND would also have been possible here. With

the chosen solution however, the Symbol can be used in various Devices

(such as for DGND etc.).

269

➢

Connect: One pin is connected to three pads in Any mode

8 Component Design Explained through Examples

➢

Supply symbol for GND

The Supply symbol has no Package assigned!

As has been explained above, the Device receives the name of the pin that is

used in the Symbol. The corresponding Device is defined with Addlevel Next.

If you set Value to off you can be sure that the labeling is not accidentally

changed. On the other hand, you have more flexibility with Value set to on.

You can alter the label if, for instance, you have a second ground potential.

You must, however, then create explicit nets for the second ground.

Quick guide to define a Supply Symbol:

Create a new Symbol in the library

Place the pin, with direction Supply

Pin name corresponds to the signal name

Set Value placeholder

Create a new Device

Device name is signal name

Package assignment not necessary

270

8.7 Attributes

You are allowed to define, additionally to >name and >value, further

properties, the so-called attributes. It's possible to define attributes for each

technology and Package variant in the Device editor. This chapter will guide

you through the process of defining attributes with the help of an example.

Therefore open the library 74xx-us.lbr and save a copy of it with Save as... in

an arbitrary directory. We don't want to change the original library for this.

Edit the Device 74*05.

Define Attributes

Let's define some attributes for the Package variant N, which is the DIL14

Package. Therefore click onto entry DIL14 (Variant N) in the Package list on

the right-hand side of the Device Editor window. Now click the ATTRIBUTE

command icon in the menu bar or onto the text Attributes in the

description window below the representation of the Device. The following

Attribute window will appear.

This dialog initially shows the Technologies available for the Package variant

N. Clicking the New button opens the New Attribute window. Please enter,

for example, Height for the attribute's name and 0.16in for the attribute's

value. The line below determines whether it is allowed to modify the value of

the attribute (variable) or not (constant) in the drawing. Select constant in

our example here.

Now you have still to define for which Technologies the attribute should be

valid: for the currently selected one only (current) or for all. Select all here.

271

➢

Attributes' dialog

➢

Defining the Height Attribute

8 Component Design Explained through Examples

Click the OK button and the new attribute is shown in the list now.

Let's define a second attribute that should have different values for the

Technologies. Click the New button in the Attributes' dialog again. Enter the

following parameters:

Name: Distributor Value: Smith, variable Technologies: all

Click OK now. A further column for the Distributor attribute is shown. All

technologies have the Smith entry.

Attribute names are written in upper case letters automatically!

But in our example the LS technology has to be distributed by Miller

exclusively. Click into the field of the Distributor attribute that belongs to the

LS technology.

➢

The Distributor field for LS is selected

Click onto the Change button now. The window for changing the properties

of the attribute opens. Set the following options:

Name: Distributor Value: Miller exclusively, constant Technologies:

current

Click the OK button, and the exception for the LS technology is defined. This

value can not be altered in the Schematic/Layout.

The Change dialog allows three possibilities in the Technologies field:

current, same, all. This means that the currently changed properties will be

valid for the currently selected (current), for all the technologies with the

same attribute value as the currently selected (all with same value) , or for

all technologies.

Finally let's define a further attribute for remarks. This attribute will have no

initial value and will be variable. So we can use it in the Schematic or in the

Layout, if necessary.

Therefore click again the New button in the Attributes dialog and make the

following settings:

Name: Remarks Value: -, variable Technologies: all

272

8.7 Attributes

Click OK. The attributes window looks like this now:

Attributes with a fixed value are colored gray in the table.

The definition of attributes for the Package variant N is finished now. Click

OK to close the Attributes window now. The attributes are shown in addition

to Technologies in the Device Editor window.

If you like to define attributes, for example, for the Package variant D (SO14),

click onto the entry in the Package list of the Device Editor window and

proceed as described above for variant N.

It's also possible to define attributes via the command line or with the help of

a Script file. Please take a look into the help function about the ATTRIBUTE

command for details.

Display Attributes

If you would use the Device 74*05 without further changes in the Schematic

or Layout Editor, it would bring along its attributes and their values. The

attributes are not visible in the drawing and can be check with the

ATTRIBUTES command.

Information about how to display attributes in Schematic or Layout can be

found on page 129 in this manual.

Placeholders in Symbol and Package

Already in the library you may define whether an attribute will be displayed

together with the Device in the Schematic or the Package in the Layout.

Simply write a placeholder text in the Symbol or Package with the TEXT

command. Such a placeholder text begins with the > character, as it is with

>name and >value. For our example attributes we defined above, you have to

write:

?5="&=K)&

?*=(&

?J"

273

➢

All the Attributes for 74*05, Variant N

8 Component Design Explained through Examples

Place this text at a suitable location in the Symbol or Package Editor and

select a proper layer for each text. It doesn't matter if you write it with upper

or lower case letters.

As soon as you add a part with pre-defined attribute placeholder texts and set

a value for an attribute in Schematic and Board respectively, the attribute's

value will be displayed at the placeholder text's location.

These texts can be separated from the Device/Package with the SMASH

command. From then on the Display property of the Attribute dialog takes

effect. The possible options are Off, Value, Name, or Both.

See page 129 for details about display options of attributes.

8.8 External Devices without Packages

A so-called External Device can be used to represent components or objects

that need to appear in the schematic but are not part of the board design.

There can be additional components, measurement equipment, cables,

mounting materials and so on. It could be used for testing or simulating

purposes, or for an electric schematic, as well.

An external device is created in the library the same way as any other

component. The symbol may have pins of any direction. Create the Device

and ADD the symbol(s) as usual.

For marking the device as an external device create an attribute with the

name _EXTERNAL_. This attribute has to be created in the library; creating

the attribute in the schematic won't work! The attribute's value doesn't

matter.

An external device is no longer treated as external as soon as you assign a

package. In this case you have to CONNECT all the pins with pads.

8.9 Labeling of Schematic Symbols

The two text variables >NAME and >VALUE are available for labeling

Packages and schematic Symbols. Their use has already been illustrated.

There are two further methods that can be used in the schematic: >PART

and >GATE.

The following diagram illustrates their use, in contrast to >NAME. The

Symbol definition on the left, the appearance in the schematic diagram on

the right.

In the first case all the symbols are labeled with >NAME. In the second case,

the symbol of the first gate is labeled with >PART and >GATE, the other

three with >GATE only.

274

8.10 More about the Addlevel Parameter

The Addlevel of the Gates that have been fetched determines the manner in

which these Gates are fetched into the schematic, and under what conditions

it can be deleted from the schematic.

Summary

Next: For all Gates that should be fetched in sequence (e.g. the NAND Gates

of a 7400). This is also a good option for Devices with a single Gate. The ADD

command first takes unused Next-Gates from components which exist on the

current sheet before "opening" a new component.

Must: For Gates which must be present if some other Gate from the

component is present. Typical example: the coil of a relay. Must-Gates

cannot be deleted before all the other Gates from that component have been

deleted.

Can: For Gates which are only used as required. In a relay the contacts may

be defined with Addlevel Can. In such a case the individual contacts can be

specifically fetched with INVOKE, and can later be deleted with DELETE.

Always: For Gates which as a general rule will be used in the schematic as

soon as the component is used at all. Example: contacts from a multi-contact

relay, of which a few are occasionally left unused. These contacts can be

removed with DELETE, provided that they were defined with Addlevel

Always.

Request: For supply gates of components.

The difference from Can is: A Device with exactly one Next-Gate and a

Request-Gate will be named, for example IC1. The Gate name does not

appear in the name of the part in the schematic. The Request-Gate's name,

however will consist of Prefix+Number+Gate name, for example, IC1P.

275

➢

Labeling of a schematic symbol

8 Component Design Explained through Examples

Relay: Coil and First Contact must be Placed

A relay with three contacts is to be designed, of which typically only the first

contact will be used.

Define the coil and one contact as their own Symbols. In the Device, give the

coil and the first contact the Addlevel Must. All the other contacts are given

the Addlevel Can.

If the relay is fetched into the schematic with the ADD command, the coil

and the first contact are placed. If another contact is to be placed, this can be

done with the INVOKE command. The coil cannot be deleted on its own. It

disappears when all the contacts have been deleted (beginning with those

defined with Addlevel Can).

➢

Relay with one coil and three contacts

Connector: Some Connection Pins can be Omitted

A PCB connector is to be designed in which normally all the contact areas are

present. In some cases it may be desirable for some of the contact areas to be

omitted.

Define a Package with 10 SMDs as contact areas, giving the SMDs the names

1 to 10.

➢

Package of a circuit board connector

Now define a symbol representing one contact area. Set visible to Pad, so

that the names 1 to 10, defined in the Package, appear in the schematic.

276

8.10 More about the Addlevel Parameter

➢

Connector symbol for the

Schematic

Then fetch the Symbol ten times into a newly created Device, setting the

Addlevel in each case to Always, and use the CONNECT command to create

the connections between the SMDs and the pins. When you now fetch this

Device into a schematic, all the connections appear as soon as it is placed.

Individual connections can be removed with DELETE.

➢

After ADD, all the connections are visible in the

schematic

Connector with Fixing Hole and Restricted Area

A connector is to be defined having fixing holes. On the solder side (bottom),

the Autorouter must avoid bringing tracks closer to the holes than a certain

distance.

277

8 Component Design Explained through Examples

The drill holes are placed, with the desired diameter, on the Package using

the HOLE command. The drilling diameter can be retrospectively changed

with CHANGE DRILL.

The forbidden area for the Autorouter/Follow-me router is defined in layer

42, bRestrict, using the CIRCLE command. For reasons of representational

clarity the circle is shown here with a non-zero width. Circles whose width is

0 are filled. In this case it has no effect on the Autorouter, since it may not

route within the circle in either case. These forbidden areas are also taken

into account by a polygon in layer 16, Bottom.

8.11 Defining Components with Contact

Cross-References

If you have to design a component that consists of a coil gate and several

contact gates for an Electrical Schematic, for example an electro-mechanical

relay, you can define the contact symbols with a placeholder text that will

generate cross-references for components. The contact overview in the

Schematic will show the cross-references then.

For a proper display of the contact cross-references in the Schematic, please

stick to the following rules for Symbol, Device, and Package definition.

Define Symbol

For defining an electro-mechanical relay you have to use one Symbol for the

coil and one or more Symbols for the contacts.

Please note the following rules for the contact symbols:

The center of the contact symbol should be located at position (0 0)

Arrange the pins in vertical direction, i.e. they are pointing up or

down

278

➢

Fixing holes with restricted areas

8.11 Defining Components with Contact Cross-References

In order to get automatically generated cross-references, use the

TEXT command to define the placeholder text >XREF and place it.

The text should be written in layer 95, Names, like >NAME and

>VALUE.

There are no special rules for the coil symbol. The placeholder text >XREF

is not needed here.

Define Device

Our electro-mechanical relay consists of multiple Gates: one Gate for the coil

and several Gates for the contacts. The placement of the Gates in the Device

Editor has to follow some rules. Otherwise the presentation of the cross-

references in the Schematic would not be optimal.

The origin of the first contact gate should be located at the

x-coordinate 0. The lower pin of the Gate should be located

completely in the positive coordinates range. The y-coordinate is

typically 0.1 inch.

Each further contact gate is placed to the right of the first one at the

same y-coordinate (the same height).

The distance between the contact gates in the Device Editor finally

determines the distance of the contacts in the graphical

representation of the contact cross-references in the Schematic. The

contact gates will be rotated by 90° and aligned vertically one by one

there.

The coil gate may be placed anywhere in the Device drawing. The

Addlevel for this Gate must be Must.

The representation of the contact cross-references shows all Gates that come

with the >XREF text. The cross-references consisting of sheet numbers and

column/row coordinates will be shown on the right of the Gates, if you placed

a drawing frame defined with the FRAME command on the Schematic's

sheets.

All other texts defined in the Symbol are not visible in the cross-reference

representation.

Define Package

Due to EAGLE's library structure and in order to avoid error messages you

have to define a Package, as well. This can be a simple dummy Package that

simply has the same number of Pads as number of Pins in the Device.

Select the Package with the New button in the Device Editor and assign Pins

with Pads with the CONNECT command.

8.12 Drawing Frames

It may be true that drawing frames are not components, but they can be

defined for schematics as Devices with neither Packages nor pins. Such

Devices in EAGLE's frames library contain a Symbol consisting merely of a

frame of the appropriate size, and a documentation field, which is also

defined as a Symbol.

279

8 Component Design Explained through Examples

A drawing frame is defined with the FRAME command. This command can

be found in the Draw/Frame menu.

The parameter toolbar offers settings for the number of columns and rows

where you can define how your drawing should be fielded. A positive value

for columns labels the frame from the left to the right, beginning with 1, for

rows from top to bottom, beginning with A. Negative values inverse the

direction of the labelling. The following four icons determine on which

position the labelling of the frame shall be visible.

The position of the drawing frame is fixed by two mouse clicks or by typing

the coordinates of its corners in the command line.

Columns and Rows can be used to determine a Device's or a net's position,

for example with the help of an ULP, or to have cross-references calculated

automatically (see LABEL command).

Is the frame already defined but you want to change its properties?

Then use the CHANGE command with its options Border, Rows and

Columns to determine the frame's position of the labelling and its number of

rows or columns.

Due to the special nature of the frame object, it doesn't have a

rotation of its own!

The FRAME command is also available in Schematic or Board. But it

is common practice to define a drawing frame in the Library.

The library frames.lbr also contains documentation fields you can use

together with a frame. Of course you are allowed to draw your own.

The text variables >DRAWING_NAME, >LAST_DATE_TIME and >SHEET

are contained, as well as some fixed text. The drawing's file name, date and

time of the last change appear at these points together with the sheet number

in the schematic (e.g., 2/3 = sheet 2 of 3).

In addition, the following variables are available:

>PLOT_DATE_TIME contains the date and time of the last printout,

>SHEETS shows the total number of sheets in the schematic,

>SHEETNR shows the current sheet number.

All of these text variables can be placed on the schematic, and (with the

exception of >SHEET/S/NR) on the board.

The frame is defined in the Device with Addlevel Next, and the

documentation field with Addlevel Must. This means that the documentation

field cannot be deleted as long as the frame is present.

280

➢

Parameter toolbar of the FRAME command

8.12 Drawing Frames

There are frames defined as Packages available for the Layout Editor which

can be placed even if there is a consistent schematic/layout pair. These

frames don't have any electrical significance because they are defined

without pads or SMDs.

The variable >CONTACT_XREF has a special meaning for Electrical

Schematics. The position of this text, which is not displayed in the Schematic,

determines the reserved area for the representation of the contact cross-

references. More details about this can be found in the help function in the

section Contact cross-references.

8.13 Components on the Solder Side

SMD components (and leaded ones too) can be placed on the top or bottom

layers of a board. For this reason EAGLE makes a set of predefined layers

available which are related to the top side (Top, tPlace, tOrigins, tNames,

tValues etc.) and another set of layers related to the bottom side (Bottom,

bPlace etc.).

SMD components are always defined in the layers associated with the top.

In the board, a component of this sort is moved to the opposite side with the

MIRROR command . Therefore click onto the component with the

mouse or enter the component's name in the command line. This causes

objects in the Top layer to be reflected into the Bottom layer, while all the

objects in the t.. layers are reflected into the corresponding b.. layers.

If one of the commands ADD, COPY, MOVE, or PASTE is active the

component can be mirrored by clicking the middle mouse button.

8.14 Components with Oblong Holes

If the board manufacturer has to mill oblong holes, you have to draw the

milling contour of oblong holes in a separate layer. Usually this is layer 46,

Milling.

The milling contour for components that need oblong holes can be drawn

with LINE (and possibly ARC) with a very fine wire width near or even 0 in

the Package Editor. Take a pad that has a drill diameter which lies inside the

milling contour, or SMDs, for example in Top and Bottom layer, as basis for

the oblong hole.

281

➢

Text variables in the documentation field

8 Component Design Explained through Examples

In case of a multilayer board you should draw a LINE in the used inner layers

at the position of the oblong holes so that it covers the milling contour and

leaves a kind of restring around the opening.

Please inform your board manufacturer that they have to take care on the

milling data drawn in this layer. Also tell them whether they should be

plated-through or not.

Any other cut-outs in the board are drawn in the same way:

Use a separate layer, typically layer 46, Milling, and draw the

milling contours. Tell your board manufacturer that they have to

take care with this information and make special note.

8.15 Arbitrary Pad Shapes

If you have to define a package with solder areas that can't be achieved with

the default pad shapes, you have to draw an arbitrary pad shape. This can be

done with the help of a polygon or with additional wires. As soon as the

center of the pad or SMD is inside the polygon's area or a wire begins at the

center of a pad, it is recognized as a part of the PAD/SMD.

The typical way to draw an arbitrary pads shape is:

Place a PAD or SMD

Use POLYGON to draw the final pad shape

- For a SMD typically in Layer Top

- For a PAD you have to draw the final shape in all the layers you plan

to use (Top, Bottom, Inner layers...)

The PAD/SMDs center must be inside the polygon's area. Otherwise

that polygon is not recognized as a part to the pad. Use a reasonable

wire width for the polygon, which fulfils the Design Rules.

The alternative to POLYGON is LINE

Start the wire in the origin of the PAD/SMD. You have to draw this

area in any signal layer you plan to use. Please use a reasonable wire

width, which fits to the Design Rules.

Check the solder stop mask

Mask data will be generated for the PAD/SMD area only. Display

layers 29, tStop and 30, bStop. If you want to have the area not

covered by solder stop lacquer, draw it manually in the appropriate

layer(s).

Check the cream frame (solder paste mask)

Display layers 31, tCream and 32, bCream for this. As we agreed upon

defining packages always on the top side of a board, the layer we have

to check is 31, tCream. Mask data will be generated automatically for

the SMD area only. If this is not what you would like to have, simply

draw the mask manually. Keep in mind that it is possible to switch off

automatic generation of mask data in the SMD properties (Cream

on/off).

Further conditions for drawing arbitrary pad shapes can be found in the help

function about the PAD or SMD command.

282

8.15 Arbitrary Pad Shapes

If a pad with arbitrary shape is not connected to a signal, the DRC

will report a Clearance error, because the polygon or wires that

define the arbitrary shape can't be recognized as a part of a signal.

8.16 Creating New Package Variants

Most components are manufactured in various Package variants. Supposed

you do not find the appropriate Package for a certain Device in one of the

libraries, it is very easy to define a new Package.

To describe this procedure clearly we want to come back again to our

example Device 541032A from paragraph 8.2.

The third Package variant to be designed here only serves as an

example for practice and does not meet the specifications of the

manufacturer!

Please notify the explanations concerning this topic, in particular if the

appropriate Package already exists in the current library beginning with page

262.

Package from Another Library

In the most favourable case you can use an already existing Package from

another library. The easiest way to define the new Package variant is to use

the PACKAGE command directly in the Device Editor.

Being in the table of contents view of your library, click onto the Add

package… button at the bottom of the Packages column, then the Import...

button in the opened dialog. Now the Import Package window pops up. It’s

similar to the ADD dialog. From here search for the wanted package, or in

case you already know where to find it, select it from the libraries list. With

the Manage libraries button you can add further libraries, or in case you

want to have less libraries in the list, drop libraries from it.

In case there is already a package with the same name in your library, it will

be updated with the imported package automatically.

Open the library (here: my_lib.lbr from paragraph 8.2) that contains the

Device you want to define the new Package variant for. For example, by the

menu File/Open/Library of the Control Panel.

Click the Edit-a-Device icon and select the Device 54*1032A from the menu.

The Device Editor opens.

Defining the Package Variant

The new variant should be named Test. The Package must have a minimum

of 14 pads because both Gates together have 14 pins. As an example, we take

the SO14 Package from the smd-ipc.lbr library.

The import is done as described above from the Table of Contents of the

library with Add package… and Import.

283

8 Component Design Explained through Examples

Alternative import options:

If Control Panel and Library Editor window are arranged side by side, select

the SO14 Package and Drag&Drop it into the opened Library Editor window.

After releasing the mouse button you will be asked for the new Package

variant name. Enter it and confirm it by clicking OK. The new variant is now

shown in the Package list.

It is also possible to define the Package variant in the Device Editor directly

with the PACKAGE command.

Type in the command line:

4+-;,"=H$!K

Or include the path (if necessary):

+-;,!!K"=H$!K

If the path contains spaces include the path name in single quotes, for

example:

C+-;,=&(H""=H$!KC

Now on the lower right of the Device Editor window a new entry for the

Package SO14 and the variant name TEST appears.

On the left a black exclamation mark on yellow ground is shown which

indicates that there are no connections between pins and pads defined yet.

➢

Device Editor: List of Package

Variants

The PACKAGE command copies the complete Package definition into

the current library and makes available the new variant with the

given name for the Device.

284

8.16 Creating New Package Variants

If you decide to erase a newly defined variant, you can do this with

the UNDO function (as far as possible) or by using the context menu

of the Package entry (right mouse click, Delete entry).

Connect Command

Click the Connect button now. The Connect window opens. Connect pins with

pads by clicking on the pin and pad entries belonging together as described

in paragraph 8.2.

It is also possible to adapt the pin/pad connections from an already existing

Package variant. In our example the assignment does not differ from the

DIL14 Package. Therefore select the entry DIL14 from the Copy from: combo

box.

After clicking OK the CONNECT command is finished.

Defining Technologies

The Device 54*1032A is available in two technologies (ALS and AS). These

still have to be set up for the new Package variant.

Select the Package variant Test from the list on the lower right of the Device

Editor window. A click onto Technologies in the description field opens a

window. Click the New button and set up technology ALS with a following

click onto OK, and AS again with a following click onto OK. Both entries are

shown with a tag now. A further click onto the OK button closes the window

again.

Save

The definition of the Package variant is finished. Now it is time to save the

library.

Using a Modified Package from Another Library

If there is no appropriate but a similar Package available in another library

you should import or copy the Package into the current library first, then

modify it, and use it afterwards as new variant for the Device.

Import the Package

We want to use a Package named SOP14 from the smd-ipc.lbr library here.

This Package should get a new name, MYSOP14, in the library my_lib.lbr.

Add Package and Import

Open your library and click onto Add package… in the Table of Contents

view. Now select Import and choose the package SOP14 from smd-ipc.lbr

from the libraries list.

Copy From the Control Panel

As an alternative to the import option:

First of all open a Library Editor window with the library that should contain

the new Package (File/Open/Library). It is not necessary to

select a certain editing mode. Now switch to the Control Panel (e. g. Window

285

8 Component Design Explained through Examples

menu) and expand the Libraries branch of the tree view. Choose the library

which contains the requested Package and select it. On the right half of the

Control Panel a preview of the Package is visible now.

If the Control Panel and the Library Editor window are arranged in a way

that both windows are visible you can move the Package into the Library

window by keeping the left mouse button pressed. After releasing the mouse

button (Drag&Drop) the Library Editor will be in the Package editing mode.

The Package is shown there.

Alternatively you could use a right mouse click to open the context menu of

the Package entry in the tree view. Select Copy to Library now. The Library

Editor needs not to be visible.

Now the Package can be modified. The Package name is adopted from the

source library. To change the Package name use the RENAME command.

Using the COPY command

For the friends of command lines:

Type in the command line of the Library Editor window (it does not matter

which editor mode is active) the following:

+6+-;,"=H$!K76+-;

Or with the whole path:

+6+-;,!!K"=H$!K76+-;

If the path contains spaces use single quotes for it, for example:

+6C+-;,*"=H$!KC76+-;

The Package Editor window opens and the Package can be modified as

needed.

Don't forget to save the library.

Defining the Variant

We want to define a further variant for our example Device. Switch to the

Device editing mode, for example, by the menu Libraries/Device. The Edit

window opens. Select the entry 54*1032A. Click OK to open the editor

window.

Use the New button to define a new variant. Select the Package MYSOP14 in

the selection dialog and enter, for example, TEST2 as variant name. After

clicking OK a new entry is shown in the Package list.

To complete the definition execute the CONNECT command and define

Technologies (as described in the previous paragraph) now.

8.17 Defining Packages in Any Rotation

Components can be defined in any rotation with a resolution of 0.1 degrees in

the Package Editor. Usually the Package is defined in normal position first

and rotated afterwards as a whole. The definition of Packages has been

already explained in this chapter. Here we only want to elaborate on the

rotation of Packages.

286

8.17 Defining Packages in Any Rotation

Packages can be defined in any rotation! Schematic Symbols can be

rotated in 90-degrees steps only!

Rotating a Package as a Whole

To come back to the example of this chapter, please open the library

my_lib.lbr and edit the Package LCC-20.

Display all layers with DISPLAY ALL to make sure you have all objects

rotated. Now use GROUP ALL to select everything.

Use the ROTATE command to rotate the group:

Now click with the left mouse into the Angle box of the parameter toolbar

and type in the requested angle. Then use a right mouse click into the group

to define the rotation point.

The Package is shown now in the given angle.

Alternatively you can work with the command line:

+..$9@?00B

rotates, for example, the previously selected group 22.5° further around the

point (0 0). The > sign (right angle bracket) within the parenthesis for

coordinates causes the rotation of the whole group (as a right mouse click at

the point (0 0) would do).

Packages with Radial Pad Arrangement

It is possible to work with polar coordinates to place pads or SMDs in a radial

arrangement. Set a suitable reference point, for example, in the center of the

Package with the MARK command first. The command line shows now

additional information about the cursor position.

Values marked with an R are relative values referring to the previously set

reference point. The leading P indicates polar values referring to the

reference point.

Example:

Three pads are to be placed on the circumference of a circle with a radius of

50 mm. The center of the part is at position (0 0).

577

74@00B

5C-C@900B

5C.C@90-.0B

5C1C@90.;0B

Depending on the used pad shape it may be useful to place the pads rotated

(for example for Long pads or SMDs).

287

➢

Package Editor: Relative and Polar Coordinates Display

8 Component Design Explained through Examples

It is possible to enter the angle directly in the parameter toolbar or in the

command line while the PAD or SMD command is active.

Example:

577

74@00B

5C.C+-.0@90-.0B

8.18 Library and Part Management

Copying of Library Elements

Within a Library

The easiest way is to do this in the Table of Contents of the library.

Each object has a context menu that offers a Duplicate entry. You will

be asked for a new name for the new Device/Symbol/Package then.

Alternatives:

If you want to use a Symbol or a Package which already exists in a related

manner for a Device definition you can copy it within the library with the

commands GROUP, COPY, and PASTE. Afterwards it can be modified as

requested.

The following sections explain every single step with the help of an example

Package taken from linear.lbr.

Open Library

Use the menu File/Open/Library in the Control Panel to open the library

linear.lbr or select the entry Open from its context menu of the tree view's

expanded Libraries branch.

Edit Existing Element

Open the Edit window with Library/Package and select the Package DIL08.

After clicking OK it is shown in the Package Editor window.

Use DISPLAY to show all layers.

Draw a frame around all objects to be copied with GROUP or type

GROUP ALL in the command line.

Now click the COPY icon. The group will be copied into the clipboard.

Define New Element

Click the Edit-a-package icon in the action toolbar.

Enter the name DIL08-TEST in the New field of the Edit window and

confirm with OK.

Click the PASTE icon followed by a click at the drawing's reference point. The

Package will be placed.

Now it can be modified as requested.

288

8.18 Library and Part Management

It is possible to COPY and PASTE with coordinates in order to move a group

by a certain value in the coordinates system. This may be valuable for

elements that have been drawn in the wrong grid. Syntax:

+6@00B

@-00B

The group will be moved by a value of 10 (grid units) in x direction.

This procedure can be applied to Symbols too!

From One Library into Another

Most convenient way to import an object is in the Table of Contents view of

the library by clicking the Add Device…, Add Package…, or Add Symbol...

button and choose the Import… option in the dialog window.

There are alternative options to import Devices, Packages, and Symbols:

Devices

If there is a proper Device or Device set that you want to use in your current

library you can copy it in different ways.

In the Control Panel:

Move (with Drag&Drop) the requested Device set from the Control Panel's

tree view into the opened Library Editor window. The complete Device set

with Symbol(s) and Package(s) will be copied and newly defined.

As an alternative you could use the entry Copy to Library in the context

menu of the Device entry.

289

➢

Import Package from Table of Contents view of a Library

8 Component Design Explained through Examples

With the COPY command:

Type, for example,

+6A9-10,A9-%%$!K

or with the whole path

+6A9-10,!!KA9-%%$!K

in the command line, the Device 75130 from library 751xx.lbr is copied into

the currently opened library.

If the path contains spaces use single quotes for it, for example:

+6CA9-10,*A9-%%$!KC

If the Device should be stored in the current library under a new name

simply enter it, like here:

+6A9-10,A9-%%$!KA9-10

Symbols

Symbols can be copied similar to Devices. Either by Drag&Drop from the

Control Panel into the open Library Editor window or with the help of the

contex menu entry Copy to Library.

You can also use the COPY command, for example:

+6=$"8,H$!K=<

Packages

The procedure to copy Packages is nearly the same as to copy Devices.

Either move (with Drag&Drop) the requested Package from the Control

Panel's tree view into the opened Library Editor window. The complete

Package will be copied and newly defined in the current library. As an

alternative you could use the entry Copy to Library in the context menu of

the Package entry.

Or use the COPY command. Type, for example,

+65->,A9-%%$!K

in the command line, the Package DIL16 from library 751xx.lbr is copied into

the currently opened library. If the library is not in the current working

directory you have to enter the whole path, as for example, in:

+65->,!8!KA9-%%$!K

If the path contains spaces use single quotes for it:

+6C5->,5*8!KA9-%%$!KC

If the Package should be stored in the current library under a new name

simply enter it directly in the command line:

+65->,!8!KA9-%%$!K5->

The Package is stored with the new name DIL16NEW now.

If you want to copy a Package that already exists with the same name in the

target library the Package will be simply replaced.

290

8.18 Library and Part Management

If the Package is already used in a Device and the position or the name of one

or more pads/SMDs changes, EAGLE prompts a message in which mode the

pads/SMDs are to be replaced. This procedure can also be cancelled. The

Package remains unchanged then.

If the enumeration and position of the pads are unchanged but the order is,

EAGLE will ask you for the appropriate update mode. Depending on your

selection the pin/pad connections of the Device may change (see CONNECT

command).

➢

Requesting the Update Mode

Composition of Your own Libraries

The previously mentioned methods to copy library elements make it very

easy to compose your own libraries with selected contents.

Provided the Control Panel and the Library Editor window are arranged in a

manner that both are visible on the screen at the same time, it is very easy to

make user-defined libraries while browsing through the library contents in

the Control Panel. Simply use Drag&Drop or the context menu Copy to

Library of the current Device or Package.

Removing and Renaming Library Elements

The easiest way to remove or rename library objects is in the Table of

Contents view in the Library Editor. Simply right-click onto the

object to be removed or renamed and select the appropriate entry in

the context menu.

Devices, Symbols, and Packages can be removed from a library with the

REMOVE command. Defining a new library element can't be cancelled by

UNDO.

Example:

You would like to remove the Package named DIL16.

Open the menu Library/Remove.... A dialog window opens where you can

enter the name of the element to be deleted.

This can be done also at the command line:

7+:5->

291

8 Component Design Explained through Examples

Packages and Symbols can be removed only if they are not used in one of the

library's Devices. In this case the message Package is in use! or Symbol is in

use! appears. Remove the corresponding Device first or delete the particular

Package or Symbol in the Device (set).

Would you like to change the name of an element in your library? Then use

the RENAME command.

Switch to the Package editing mode so that the element that should be

renamed is shown first and open the menu Library/Rename. A dialog

window opens where you can enter the new name of the element.

This can also be done at the command line:

75->5->

The Package DIL16 gets the new name DIL-16.

The Device, Symbol, or Package name may also be given with its extension

(.dev, .sym, .pac), for example:

7+:5->$

In this case it is not necessary to switch to the related editing mode before.

Update Packages in Libraries

As already mentioned in the section Copying of Library Elements it is

possible to copy Packages from one library into another one. An already

existing Package is replaced in that case.

Each library contains Packages which are needed for Device definitions. In

many libraries identical types of Packages can be found. To keep them

uniform over all libraries it is possible to replace all Packages of a library with

those of another library with the help of the UPDATE command. An existing

Package with the proper name will be replaced by the current definition.

If you have, for example, special requirements for Packages you could define

them in a custom-built Package or SMD library. The UPDATE command

could transfer them to other libraries.

Therefore open the library to be updated and select Library/Update.... Now

select the library which you want to take the Packages from.

Having finished the update EAGLE reports in the status bar:

Update: finished - library modified!

If there was nothing to replace: Update: finished - nothing to do.

It is also possible to use the command line for this procedure.

If you want to update your library with Packages from, for example,

ref-packages.lbr, type:

5VHJ"$!K

To transfer Packages from different libraries, type in one after another:

5VHJ"$!K!$!K""H=!$!K

To update a single Package, type in the Package name:

5+-;,VHJ"

292

8.18 Library and Part Management

The extension .lbr is not necessary. You may also use the whole library path.

See page 290 for further information.

293

8 Component Design Explained through Examples

This

page

has been

left free

intentionally.

294

Chapter 9

Preparing Manufacturing Data

Data output for board manufacturing is made with the help of the CAM

Processor. PCB manufacturer usually work with drill data in Excellon format

and plot data in Gerber format. How to generate such data and which data

you have to pass on to your PCB manufacturer will be explained in this

chapter.

A lot of PCB manufacturers generate these data with EAGLE by themselves.

In such a case you have to pass on the board file only and you need not care

about data generation. You will find links to such firms on our Internet

pages.

With the help of pcb-service.ulp you will be directed to element14.com and

may have an offer of partners from Farnell/Newark for manufacturing your

printed circuit board. Based on your layout and the Design Rules, key

parameters for manufacturing, like board size, minimum drill size, and so on

are determined.

Your design should be complete and have passed a DRC successfully. By

clicking onto the link in the ULP dialog window you will be directed to the

quote site of element14, where these parameters will be transferred, as well

(login necessary). With a few steps you get a quote for manufacturing your

board.

If, however, your board maker is not set up to process EAGLE board files

directly, you will have to supply them with a set of files. What will be required

will be discussed in the following sections.

Additional useful User Language Programs (ULPs) are available on the web.

They can be used, for example, for the generation of glue mask data, for the

calculation of milling contours, or for data regarding automatic mounting

and testing equipment.

9.1 Which Data do we Need for Board

Manufacture?

The PCB manufacturer requires specific information pertaining to each step

in the manufacturing process of your board. This special information is

described in a file containing plot and / or drilling information.

For example, one file for each signal layer, for the silkscreen, for the solder

stop mask, the cream frame, for a gold application, for a glue mask (for SMT

devices), or for milling data regarding cut-outs in the board.

295

9 Preparing Manufacturing Data

Double-sided boards with parts on top and bottom side require a silkscreen

on both sides, or in case of SMT devices, a cream frame or a glue mask for

each side.

Additionally the board manufacturer needs drilling data in a separate file.

If you want a milled prototype board, milling contours have to be calculated

first, and generated in a specific data format for fabrication milling

machines.

If you want to have the parts automatically mounted, you need additional

files in appropriate data format that depict centroid and rotational angular

information.

A bill of materials or a legend for the drill symbols can be helpful, too.

Gerber Plot Data

All PCB manufacturers use Gerber format. There are two options of Gerber

format available, Extended Gerber format, also known as Gerber RS-274X

(in short RS-274X), which is the most commonly used today in industry.

The CAM Processor offers this device option as GERBER_RS274X.

It may be the case that the PCB manufacturer works with the second option

RS-274D. This will require the generation of data with the devices

GERBERAUTO and GERBER of the CAM Processor.

Gerber data (RS-274D) basically consist of two parts:

The so-called Aperture file or Wheel file, a special tool table, and the plot

data that contain coordinates and plotting information for the Gerber plotter.

Please inquire which format your PCB manufacturer prefers. The

more convenient to use is Extended Gerber, RS-274X.

GERBER_RS274X

This device generates files in Extended Gerber format (RS-274X) where the

aperture table is integrated in the output file. Simply generate Gerber files

with the GERBER_RS274X device and pass them on to your board

manufacturer. This is the most efficient and easiest way to generate Gerber

data.

The Extended Gerber device GERBER_RS-274X has a resolution of

1/100,000 of an Inch (data format: 2.5, inch).

Alternatives:

GERBER_RS274X_24 1/10.000 inch, data format 2.4, inch

GERBER_RS274X_26 1/1.000.000 inch, data format 2.6, inch

GERBER_RS274X_33MM 1/1000 mm, data format 3.3,

GERBERAUTO and GERBER

The prior RS-274D format works with a separate aperture file which is

necessary to generate all Gerber files you will need for board manufacturing.

296

9.1 Which Data do we Need for Board Manufacture?

First you have to generate the aperture table (wheel file) with

GERBERAUTO. This file is a tool table which defines the shape and the size

of the Gerber plotter's apertures (tools). This table must contain the whole

aperture definition we need for generating all Gerber files that describe the

board.

For generating the Gerber files with the GERBER device, we refer to the

previously generated aperture file, made with GERBERAUTO.

GERBER and GERBERAUTO have a resolution of 1/10.000 of an Inch.

Exceptions are the devices GERBERAUTO_23 and GERBER_23. They have

a lower resolution of 1/1,000 of an Inch (data format 2.3, inch).

Drill Data

The generation of drill data is very similar to the generation of plot data.

Typical formats used in industry are Excellon or Sieb&Meyer 1000 or 3000.

They are supported by the CAM Processor. The most common one is

Excellon.

The simplest case is to generate one common drill data file for all drill holes.

If you have to distinguish plated from non-plated drill holes, two drill data

files must be generated. EAGLE differentiates between plated drills of Pads

and Vias in layer 44, Drills, and non-plated holes in layer 45, Holes, which

are placed by the HOLE command.

If you have to generate drill data for a multilayer board that uses Blind and

Buried vias with different via lengths that result in different drilling depths,

the CAM Processor takes care on this automatically. For each via length it

generates a separate drill data file.

Further information about this can be found in chapter 9.5 from page 310 on.

EXCELLON

Using this device the CAM Processor generates a drill file that contains the

drill table and the drill coordinates. This file format is the most common in

the industry and will be recognized by most board manufacturers.

The default resolution of the EXCELLON device is 1/100,000 of an Inch, no

leading zeros (data format: 2.5, Inch).

Alternatives:

EXCELLON_24 1/10.000 inch, data format: 2.4, inch

EXCELLON_26 1/1.000.000 inch, data format: 2.6, inch

EXCELLON_33MM 1/1.000 mm, data format: 3.3, mm

EXCELLON_RACK

This device can be used, if your board manufacturer insists on two separate

files. A drill table (rack file) and the drill data file. This was default in prior

EAGLE versions. Default data format is 2.4, Inch.

In the first step one has to generate the drill table in the Layout Editor with

the help of the User Language program drillcfg.ulp, and refers to this drill

table when generating drill data with the CAM Processor. The board

manufacturer gets two files then, drill data and drill table.

297

9 Preparing Manufacturing Data

If you have to distinguish between plated and non-plated drillings you have

to supply one drill table and two drill data files (one for layer Drills, one for

layer Holes).

SM1000 and SM3000

These devices generate drill data in Sieb&Meyer 1000 or in Sieb&Meyer

3000 format. SM1000 has a resolution of 1/100 mm, SM3000 1/1000 mm.

Data output is exactly the same as it is with EXCELLON_RACK. First you

have to generate the drill table with drillcfg.ulp, then use the CAM Processor

to generate drill data.

Further Drill Data Devices

The CAM Processor supports two further devices for drill data generation.

GERBDRL generates Gerber drill code. Here we need a separate drill table

(RUN drillcfg.ulp), as it is with EXCELLON_RACK.

SMS68 is a further drill data device that generates a HPGL code.

Prototype Manufacture With a Milling Machine

With the help of various User Language programs you can generate outline

data for milling a prototype board.

outlines.ulp

A simple example for contour data calculation is outlines.ulp. Start it with the

RUN command. Select the layer for which outline data shall be generated,

define the diameter of the milling tool (Width), and select the output file

format (Script or HPGL) in the ULP's dialog window.

The Script file containing the outline data can be imported into EAGLE with

the SCRIPT command. Thus it's possible to visualize the calculated contours

in the Layout Editor. You can even modify them, if necessary.

Finally, the milling data output is made with the CAM Processor. Select the

layer where the contours are to be drawn in and use, for example, the HPGL,

the PS (Postscript) or one of the Gerber devices for the output.

Further information can be found in the help function, Outline data.

mill-outlines.ulp

Another User Language program that calculates outline and drill data is mill-

outlines.ulp. It offers various configuration parameters. Simply start it with

the RUN command in the Layout Editor. Consult the ULPs integrated help

function for details.

This ULP exports for example CNC or HPGL formatted data or generates a

Script file which can be imported into the layout again. The milling contours

can be viewed, or even modified, if required. Generate the milling data with

the CAM Processor and one of its devices, like Gerber, HPGL or PS then.

Film Generation Using PostScript Files

A high-quality alternative to Gerber is the data generation for PostScript

raster image recorders. The exposed film serves as master for board

manufacturing.

298

9.1 Which Data do we Need for Board Manufacture?

With the PS driver, the CAM Processor generates files in PostScript format.

These files can be processed directly by appropriate service companies (most

of which operate in the print industry).

For PostScript recorders the Width and Height parameters should be set to

very high values (e.g. 100 x 100 inches), so that the drawing is not spread

over several pages.

For generating Postscript files you have to select the proper layers, the same

way it is performed for Gerber data generation. Use these files for the

generation of your artwork at your particular PCB subcontractor.

Films that relate to the bottom side are usually output in mirrored form

(Mirror option in the CAM Processor). In doing so the coating of the foil

rests directly on the copper layer of the board which is to be exposed.

The EPS driver generates Encapsulated PostScript files. They can be

processed with Desktop Publishing programs.

Printing on a Film

For boards of limited complexity, one can use a laser or ink jet printer and

print on a transparent foil with the PRINT command. This method is used,

for example, by hobbyists and results in a shorter fabrication time and a less

expensive board fabrication process.

The layers that are displayed in the Layout Editor while printing will appear

on the film. Check the options Black and Solid in the print dialog.

The drills of pads and vias are visible on the printout. This will allow an easy

visual indication of where you have to drill manually on the board.

Experience shows that the opening of a pad or a via should not be too big to

allow for a good centering of the drill bit. This issue can be solved with the

help of an User Language program, named drill-aid.ulp. Start it before

printing, and let it draw a ring inside each pad and via in a separate layer.

The inner diameter of this ring can be defined and is usually set to 0.3mm. Of

course, you have to display this additional layer for printing on the film.

Data for Pick-and-place Machines and In-circuit

Testers

EAGLE includes some ULPs which create data for various automatic

placement machines and in-circuit testers that are typically used by PCB

manufacturers.

The description of an ULP can be viewed in the User Language Programs

branch of the tree view of the Control Panel by selecting one of the ULP

entries with the mouse. The describing text appears on the right side of the

Control Panel window. It's also possible to edit the ULP file with a text editor.

The description usually is written in the file header.

ULPs for pick-and-place data (selection):

mount.ulp Generates one file with coordinates of

the centered part origins

mountsmd.ulp Centered origins for SMT devices; one file for

top and one file for bottom side

299

9 Preparing Manufacturing Data

ULPs for circuit tester (selection):

dif40.ulp DIF-4.0 format from Digitaltest

fabmaster.ulp Fabmaster format FATF REV 11.1

gencad.ulp GenCAD format for Teradyne/GenRad

in circuit tester

unidat.ulp UNIDAT format

Execute the RUN command in the Layout Editor window to start the

particular ULP.

Documentation

Many documentation items can be generated with the aid of User Language

programs. Note also the wide range of programs that are made available on

our web server. The bom.ulp, the program for generating a bill of materials,

has been used as a basis for lots of user-contributed ULPs.

Parts List

The parts list can be created by bom.ulp. Start it from the Schematic Editor,

using the RUN command. The Bill Of Material window with the parts

summary opens first.

➢

bom.ulp: Dialog window

is possible to import additional information from a database file into the

parts list (Load), or to create a new database with its own properties such as

manufacturer, stores number, material number or price (New).

You can obtain further details about the current version of the ULP by

clicking the help button.

300

9.1 Which Data do we Need for Board Manufacture?

A simple parts list can also be created from a board or schematic by

means of the EXPORT command (Partlist option).

Drill Plan

Printing a drill plan enables you to check the drill holes and their diameters.

It shows an individual symbol for each diameter of hole, via, and pad used in

your design. EAGLE uses 19 different symbols: 18 of them are assigned to a

certain diameter; one (Æ) appears, if no symbol has been defined for the

diameter of this hole. The symbols appear in layer 44, Drills, at the positions

where pads or vias are placed, and in layer 45, Holes, at the positions where

holes are placed.

The relation between diameters and symbols is defined through the Layout

Editor's Options/Set/Drill dialog.

The buttons New, Change, Delete and Add can be used to create a new table,

to modify certain entries, delete them or to add new ones.

The Set button extracts all the hole diameters from the layout and

automatically assigns them to a drill symbol number. The values of Diameter

and Width determine the diameter and line thickness of the drill symbol on

the screen and the printout.

The image above shows that drill symbol 1 is assigned to a drill diameter of

0.01 inch. In the following image you can see how the related symbol drawn

in layer 44, Drills, or 45, Holes, looks like. The symbol number 1 looks like a

plus character (+).

The dill symbol assignment is stored in the user-specific file eaglerc.usr

(.eaglerc for Linux and Mac).

301

➢

Configuration of the drill symbols

9 Preparing Manufacturing Data

Drill Legend

Documenting the drill symbol assignment is quite simple with the help of a

handy User Language program named drill-legend.ulp.

In the first step we let EAGLE generate the drill symbol assignment for the

current layout with the Set button in the Options/Set/Drill Symbols menu.

Now we start drill-legend.ulp. It draws a table with the proper drill symbol

assignment and the drill symbols at their positions in the board in the newly

generated layer 144. For printing, it can be helpful to display layer 20,

Dimensions, additionally.

If you want to delete this all, simply use GROUP and DELETE in layer 144.

Assembly Variants

The CAM Processor basically generates data for the assembly variant, the

board is saved with. The status bar of the CAM Processors shows the

assembly variant as soon as the board file is loaded.

If you have to create data for another assembly variant, we recommend to

select this variant in the schematic editor and save schematic and board in

this variant. Now start the CAM Processor again.

If you prefer to the CAM Processor from a Command Prompt window or a

Terminal window (eagle -X) you have to specify the command line option -A

in order to select the assembly variant. Information about these options can

be found in the Appendix beginning with page 325.

9.2 Rules that Save Time and Money

Each layer should without fail be uniquely identified (e.g. CS for

Component Side, BS for Bottom Side).

302

➢

Assignment of the drill

symbols

9.2 Rules that Save Time and Money

It may be wise to use fiducial or crop marks which can be defined in

layer 49, Reference. This will allow easy alignment of PCB generated

films for both inspection and fabrication. When generating

manufacturing data, this layer has to be active additionally with all

signal layers. Please contact you board manufacturer concerning this

matter. Fiducials can be found in marks.lbr. A minimum of three

fiducials or crop marks (three corners) is required for proper film

alignment reference.

For cost reasons you should, if at all possible, avoid tracks that narrow

to below 8 mil.

Usually the contour of the board is drawn in layer 20, Dimension. But

it is also possible to draw angles at the corners to delimit the board in

each signal layer. Please contact your board manufacturer what they

prefer.

If your board has milled edges, please contact your board

manufacturer to clarify in which layer these contours have to be

drawn. See also page 309.

You should always leave at least 2 mm (about 80 mil) around the edge

of the board free of copper. This is especially important for multilayer

boards to avoid internal shorts between these layers.

In the case of supply layers on multilayer boards, which are plotted

inverse, you do this by drawing a wire around the edge of the board.

This will act as a copper keep-out in this area.

Please take care of the wire width for polygons. It should not be set

too fine or even 0. These reduced wire widths result in huge file sizes

and can lead to problems for board manufacturing, as well.

As already mentioned in the section of the TEXT command, texts in

copper layers ought to be written in vector font. So you can really be

sure that the text on your board looks the same as it does in the

Layout Editor window.

To play safe, you could activate the options Always vector font and

Persistent in this drawing in the Options/User Interface menu before

passing on your board file to the board manufacturer.

For the sake of completeness we want to point out here again that all

questions concerning layer setup, layer thickness, and drill diameter

for multilayer boards with Blind, Buried, or Micro vias have to be pre-

examined.

Supply an informational text file to your PCB manufacturer that

contains information about specific features in the board. For

example, information about used layers, milling contours, and so on.

This saves time and avoids trouble.

9.3 Quick Guide for Data Output

The CAM Processor provides an automated job mechanism aiding in the

creation of the output data for a board. It is possible to generate all data by a

single mouse click.

303

9 Preparing Manufacturing Data

The Control Panel's tree view (CAM Jobs branch) lists all jobs and shows a

brief description.

If you are not yet familiar with the use of the CAM Processor, please scroll

back to the chapter about The CAM Processor on page 84. There you will

learn about the basic operation of the CAM Processor.

The pre-defined jobs gerb274x.cam and gerber.cam are designed for

a two layer board which has components on the top side only. They

will generate files for the signal layers, the silk screen for the

component side, and the solder stop mask for top and bottom.

Job gerb274x.cam

This job can be used to generate manufacturing data in Extended Gerber

format.

Proceed as follows:

Start the CAM Processor, for example, with the CAM Processor icon

in the Layout Editor or with the File/CAM Processor menu.

Load the board into the CAM Processor (File/Open/Board) if it was

not loaded automatically during the start sequence.

Load the pre-defined job gerb274x.cam with the File/Open/Job

menu.

Now click Process Job. EAGLE generates five files, one by one,

automatically which you have to pass on to the board manufacturer.

Each Gerber file contains the aperture table and the respective plot

data.

The following files will be generated:

%N.cmp Component side

%N.sol Solder side

%N.plc Silk screen component side

%N.stc Solder stop mask component

side

%N.sts Solder stop mask solder side

%N.gpi Info file, not needed here

%N is the placeholder for the board file name without its extension.

304

9.3 Quick Guide for Data Output

If other layers are also to be generated, e.g. silkscreen for the bottom side, or

a solder cream mask, the Gerber job can be extended with modifications as

required. Extending the job is discussed later in this chapter.

Job excellon.cam

The easiest way to generate drill data is to use the pre-defined CAM job

excellon.cam, used with the CAM Processor a file that contains drill data and

the respective drill table will be generated automatically. This job does not

distinguish between the layers Drills and Holes. Both will be output into a

common file. Usually all drillings will be plated-through then.

Proceed as follows:

Start the CAM Processor (for example File/CAM Processor menu) in

the Layout Editor.

Load the board into the CAM Processor (File/Open/Board), if it has

not been loaded automatically during the start sequence.

Load the pre-defined job excellon.cam, e.g. with File/Open/Job.

Execute the job with a mouse click on Process Job. Drill data output

starts now.

Excellon.cam does not distinguish between plated-through drills and

non-plated-through holes!

The following files will be generated:

%N.drd Drill data

%N.dri Info file, for board

manufacturer,

if required

305

9 Preparing Manufacturing Data

➢

CAM Processor: Generate drill data with the excellon.cam

job

The default unit for the drill table is inch. If the drill table would be preferred

in Millimetres the device definition can be changed in the file eagle.def. More

details concerning this can be found in the section Units for aperture and

drill tables, beginning with page 320.

Excellon.cam can be used for multilayer boards, as well as for those with

Blind, Buried or Micro vias. In this case several drill data files will be

generated. See chapter 9.5 for details.

Job gerber.cam

If your board manufacturer can not handle Extended Gerber format and

expects Gerber data with a separate aperture file, use the job gerber.cam.

These files can be created with the devices GERBERAUTO and GERBER and

generates data in RS-274D format.

How to proceed:

Start the CAM Processor, for example, with the CAM Processor icon

in the Layout Editor or with the File/CAM Processor menu.

Load the board into the CAM Processor (File/Open/Board) if it was

not loaded automatically during the start sequence.

Load the pre-defined job gerber.cam with the File/Open/Job menu.

Now click Process Job. EAGLE automatically generates six files which

you have to pass on to the board manufacturer. Five Gerber plot files

and one common aperture table.

In the first step an aperture table %N.whl is generated. Two messages

appear, which you confirm with OK.

306

9.3 Quick Guide for Data Output

The left message is generated by the entry in the Prompt field, and

reminds you to delete the temporary file %N.$$$ created when generating

the aperture table after the job is done.

The message on the right advises you that more than one signal layer are

active at the same time. Normally only one signal layer is active while

output is generated. However, when generating the wheel, all the layers

need to be active at the same time to form a common aperture table for

the Gerber output.

The following files will be subsequently output:

%N.whl Aperture file (Wheel)

%N.cmp Component side

%N.sol Solder side

%N.plc Silk screen component side

%N.stc Solder stop mask component side

%N.sts Solder stop mask solder side

%N.$$$ Temporary file, please delete it

%N.gpi Info file, not needed here

9.4 Which Files do I Need for my Board?

The previous part of this chapter told you a lot about the basics of data

generation and how to use pre-defined job files for default two layer boards.

In this section you will find a summary of files usually generated for board

manufacturing.

Files List

The output files of the CAM jobs differ in their file extensions. You are, of

course, free to use unequivocal names of your own.

The CAM Processor allows the use of some placeholders for the generation of

output file names. Usually the output file name consists of the name of the

board file plus a special file extension. For the board file name without

extension we use the placeholder %N. Write, for example, in the Output File

307

➢

Messages in gerber.cam

9 Preparing Manufacturing Data

field: %N.cmp. This will be expanded with the name of the layout file that is

loaded plus the extension (here: boardname.cmp).

In the following table %N also stands for the name of the currently loaded

board file that is used to generate manufacturing data from.

File name Selected layers Description

Signal layers

❑%N.cmp 1 Top, 17 Pads, 18 Vias Component side

(top)

❑%N.sol 16 Bottom, 17 Pads,

18Vias Solder side (bottom)

Inner layers

❑%N.ly2 2 Route2, 17 Pads, 18

Vias

Inner layer 2

❑%N.ly3 3 Route3, 17 Pads, 18

Vias

Inner layer 3

..... ..... .....

❑%N.l15 15 Route15, 17 Pads,

18 Vias

Inner layer 15

Silk screen

❑%N.plc 21 tPlace, 25 tNames,

possibly 20

Dimension(*)

Silk screen

component side

❑%N.pls 22 bPlace, 26 bNames

possibly 20

Dimension(*)

Silk screen solder

side

Solder stop mask

❑%N.stc 29 tStop Solder stop

component side

❑%N.sts 30 bStop Solder stop solder

side

Cream frame (for SMT devices)

308

9.4 Which Files do I Need for my Board?

❑%N.crc 31 tCream Cream frame

component side

❑%N.crs 32 bCream Cream frame solder

side

Milling contours for openings, oblong holes...

❑%N.mill 46 Milling (**) Plated milling

contours

❑%N.dim 20 Dimension (**) Non-plated milling

cont.

Finishing mask (e.g. gold coating)

❑%N.fic 33 tFinish Finishing

component side

❑%N.fis 34 bFinish Finishing solder side

Glue mask (for larger SMT devices)

❑%N.glc 35 tGlue Glue mask

component side

❑%N.gls 36 bGlue Glue mask solder

side

Drill data

❑%N.drd 44 Drills, 45 Holes All drillings

Distinguishing plated from non-plated drillings

❑%N.drd 44 Drills Plated drillings

❑%N.hol 45 Holes Non-plated drillings

(*) Please check with your board manufacturer whether you have to output

the board contour in layer 20 in a separate file or you are allowed to combine

it with those layers.

(**) If there are additional milled edges in the board, you should contact

your board manufacturer and ask them which layers they prefer for milling

contours.

309

9 Preparing Manufacturing Data

Placeholders for Output File Name Generation

%D{xxx} xxx stands for a string that is inserted

only into the data file name

%E file extension of the loaded file, without

the '.'

%H home directory of the user

%I{xxx} xxx stands for a string that is inserted

only into the Info file name

%L layer range for blind&buried vias

%N name of the loaded file without path and

extension

%P directory path of the loaded Board or

Schematic file

%% the character '%'

These placeholders must be written in upper case letters!

Hints Concerning File Extensions:

cmp stands for component side, the upper side of the board, sol for the solder

(bottom) side. It makes sense to choose the first two letters according the

active layers. The third one can be c or s for belonging to component or

solder side.

Of course you are free in naming your files in any manner you wish!

Please ensure when defining a job that the extensions of the output

files are unique and therefore distinguishable.

9.5 Peculiarities of Multilayer Boards

In case of boards with inner layers one has to know how these layers are

defined in order to generate proper manufacturing data. Is it an inner layer

that contains tracks and polygons, as it is in Top or Bottom layer? Or is it a

supply layer that can be identified by the $ character in front of the layer

name?

Inner Layers

Inner layers are treated the same as the outer signal layers. Together with the

signal layer, the layers Pads and Vias have to be actived.

310

9.5 Peculiarities of Multilayer Boards

If the Layer Setup allows Blind and Buried vias, the combination of one

signal layer and the Vias layer outputs only those vias that belong to this

signal layer.

If there is only the Vias layer active (no signal layer), the CAM

Processor will output all vias of the board!

Drill Data for Multilayer Boards With Blind and Buried

Vias

The CAM Processor generates one drill data file for each via length for a

layout that uses Blind and Buried vias.

The drill data file extension .drd is expanded by the via length specification.

If there are, for example, vias from layer 1 to 2, the output file extension will

be .drd.0102.

The layer specification can be moved to another position with the help of the

wildcard %L. Writing, for example, in the File box of the CAM Processor %N.

%L.drd results in an output file named boardname.0102.drd.

Pads and trough-hole vias will be written into an output file with extension

.drd.0116. If you placed holes (HOLE command) in the layout and the Holes

layer is active for output, the CAM Processor writes this data also into the file

with extension .drd.0116.

Pass on all these files to your board manufacturer.

Provided you did not use the EXCELLON device which combines drill table

and drill coordinates in a common file, your board house additionally needs

the rack file name.drl which is generated by drillcfg.ulp.

9.6 Set Output Parameters

This section describes the setting of the parameters in the CAM Processor for

the output of a board or a schematic.

Load the schematic or board file from the CAM Processor's File/Open menu,

and set the parameters.

The CAM Processor window is divided into sections (Output, Job, Style,

Layer, Offset and so on). Some sections, like Emulate, Tolerance, Pen or

Page, are used by and therefore displayed with certain devices only.

311

9 Preparing Manufacturing Data

➢

CAM Processor: Solder side section of the gerber.cam

job

Output:

Select the driver for the desired output device or output format in the

Device combo box.

Enter the output path and file name in the File field or simply click

onto the File button and use its dialog.

If you want to output a file on a particular drive, place the drive

identifier or, if appropriate, the path in front of the file name ending.

For instance, under Windows, d:\%N.cmp would place the file

boardname.cmp in the root directory of drive D. This also applies to

the Linux version, so that, for example, /dev/hdc2/%N.cmp, would

place the file on drive hdc2.

%H can be used as wildcard for the Home directory, %P for the loaded

file's directory path.

If output is to go directly to a plotter, enter the name of the print

queue that is connected to the corresponding computer interface in

UNC notation, e.g. \\Servername\Plottername.

Depending on the chosen device it may be asked for Wheel (aperture

table) or Rack (drill table). Select path and file by clicking the button.

Layer selection:

Select the layers that should be output into a common file by clicking

the appropriate layer number.

Click the menu Layer/Deselect all to uncheck all the layers first.

Layer/show selected displays only the currently selected layers.

Some devices (like HPGL or certain plotter devices) allow you to select

a color or pen number in an additional column.

312

9.6 Set Output Parameters

Style:

Mirror: Mirrors the output.

It can be useful to mirror all outputs that refer to the bottom

side of the board.

Rotate: Rotates the output by 90 degrees.

Upside down: Rotates the output by 180 degrees.

When combined with Rotate, the drawing is rotated

by a total of 270 degrees.

Pos. Coords.: Avoids negative coordinate values for the output.

The drawing will be moved near the coordinate's axis,

even if it is already in the positive coordinates range.

Negative values can lead to errors with a lot of devices!

This option should be set on always by default.

Switching it off, transfers the coordinate values from

the Layout Editor unchanged.

Quickplot: Draft output which shows only the outlines of objects.

This option is available for certain devices, like HPGL

and various plotters.

Optimize: Activates the optimization of the drawing sequence for

plotters. Should be set on by default.

Fill Pads: This option is always set on. Only the devices PS and

EPS allow you to switch off this option. The drill holes

for pads will be visible on the output (as it is with the

PRINT command).

Job:

If you are on the way to define a CAM job that consists of several

sections it is useful to name them. In the Section line, it is possible to

enter a section name which will be shown also in the tab above.

If, for example, you assign the section name Wheel: Generate

Aperture File, only the title Wheel is visible as a tab name. The

additional description can be read in the section line. The colon ends

the title in the tab.

In case you wish to display a message box on the screen before

executing this section, enter special message text in the Prompt field.

For example: Please insert a new sheet of paper! The output does not

continue until confirmation of this message.

Offset:

Define an offset in x and y direction.

The values can be given in Inches or Millimetres, for example, 15mm

or 0.5inch.

Tolerance:

Tolerances for Draw and Flash apertures are necessary for devices

that use an aperture file, like GERBER or GERBER_23. Usually one

allows a tolerance of 1% in all fields.

This is necessary to compensate small rounding errors that can arise

during the conversion from mm to inch values and vice versa as the

aperture table is generated.

313

9 Preparing Manufacturing Data

Devices for drill data generation that use a separate drill table (rack

file) invoke a Drill entry. A tolerance of ± 2.5% is enough to

compensate for rounding errors that possibly can arise during the

conversion from mm to inch.

Emulate:

If an aperture with the exact value is not available in the aperture file,

you can allow Aperture emulation. The CAM Processor is allowed to

use smaller drawing apertures for emulation. Plotting time and costs

will increase, and therefore you should try to avoid aperture

emulation.

Arcs with flat endings (CHANGE CAP FLAT) are always emulated for

Gerber output, which means that they are drawn with small lines.

Arcs with round endings (CHANGE CAP ROUND), however, not.

If your layout contains objects that are rotated in any angle, you

have to activate aperture emulation. Certain pad shapes must be

drawn with a smaller round aperture.

Page:

Define the Height and Width of the sheet you want to plot on. Values

are in Inches by default. Values can also be given in Millimetres, like

297mm.

Pen:

The Diameter of the plotting pen is given in here. The value has to be

in Millimetres.

For plotters that support adjustable pen Velocity you can define a

value given in cm/s (centimetres per second). No value here results in

a default value given by the plotter.

Sheet:

Select the sheet of the schematic you want to output.

9.7 Automating the Output with CAM

Processor Jobs

Defining a New CAM Job

A Job consists of one or more sections that allow you to generate a full set of

manufacturing data with only a few mouse clicks. A section is a group of

settings, as described above in the Set Output Parameters chapter, which

defines the output of one file.

Define a job as follows:

Start the CAM Processor.

No job is loaded at first, unless there is a file called eagle.cam in the

cam directory or an existing job is called up automatically by an

EAGLE project file.

314

9.7 Automating the Output with CAM Processor Jobs

If has not already been done, load the board file which you want to

define the job for (also possible for schematics).

It is best that you load an existing job, for example gerb274x.cam,

through the CAM Processor's File/Open/Job menu.

Save this job under a new name with File/Save job... So the original

job file remains unchanged.

Click the Add button.

The currently active section with all its parameter settings is copied

now.

Enter a new descriptive text in the Section line.

If you wish to get a message shown before executing this section,

enter a specific text prompt in the Prompt line.

Set all parameters now:

Device, the layers for the output, the output File, a Scale factor, if

needed, the Style options (Mirror, Rotate, Upside down...).

Define further sections in the same way using different names.

Very important: First use Add to create a new section, then set the

parameters.

Delete a section, if needed, by clicking the Del button.

Save all the sections of your new job as a job file under a name of your

choice with File/Save job...

All the sections of the job will be executed automatically one after another if

you click the Process job button. One specific (the currently shown) section

will be executed if you click the Process section button.

The Description button allows a descriptive text of the CAM job that will be

displayed in the Control Panel.

Extending gerber.cam Job for Multilayer Boards

The gerber.cam job can be used as the basis of the job for multilayer boards.

It must simply be extended for the additional inner layers.

Example:

You want to output the files for a board with SMD components on the top

and bottom sides. The board has two additional inner layers. Layer 2 and

layer 15 which is named VCC.

You need silkscreen prints for the upper and lower sides, solder stop masks,

and masks for the solder cream for both sides.

Before you start to change the CAM job you should save the job under a new

name through the File/Save job as.. menu.

Proceed as described in the previous section. The CAM job then contains the

following sections:

Output

file

Selected layers Description

315

9 Preparing Manufacturing Data

*%N.$$$

1, 2, 15, 16, 17, 18, 20,

21, 22, 25, 26, 29, 30,

31, 32

Generate wheel

file .whl

* modified layer

selection

%N.cmp 1 Top, 17 Pads, 18 Vias Component side

%N.ly2 2 Route2, 17 Pads, 18

Vias Inner layer 2

%N.l15 15 VCC, 17 Pads, 18

Vias Inner layer 15

%N.sol 16 Bottom, 17 Pads,

18Vias Solder side

%N.plc 21 tPlace, 25 tNames,

20 Dimension

Silkscreen

component side

%N.pls 22 bPlace, 26 bNames

20 Dimension

Silkscreen solder

side

%N.stc 29 tStop Solderstop mask

comp. side

%N.sts 30 bStop Solderstop mask

solder side

%N.crc 31 tCream Creamframe comp.

side

%N.crs 32 bCream Creamframe solder

side

Check once more whether all the necessary layers for the creation of the

aperture table are active in the first section. The output file generated in the

first section cannot be used. For this reason, the file boardname.$$$ should

be deleted.

For inner layers, you always have to activate the layers Pads and

Vias!

Error Message: Apertures Missing

If the error message APERTURES MISSING – NO PLOTFILE HAS BEEN

PRODUCED appears after starting the modified CAM Job, the Gerber info

file boardname.gpi contains information about the reason of the problem.

The error could possibly be not all apertures were defined or some could not

316

9.7 Automating the Output with CAM Processor Jobs

be found in the table due to missing tolerance settings.

Ensure all used layers were activated in the Generate a Wheel file section?

It could also be the case that there are parts placed in any angle with pads

that don't have a round shape in the layout. You have to activate the aperture

emulation then to have a successful file creation.

Gerber Info Files

The CAM Processor generates for each Gerber plot file created an additional

Gerber info file with the extension .gpi. This text file informs you about used

apertures, the data format of the Gerber device, about possible aperture

emulations or tolerances, and so on.

If you define a job for Gerber output with data files that use the extensions

proposed in the table above, the info file will be overwritten with each

succeeding section.

If your board manufacturer or your plot service wants to have these

additional information files (they are typically not necessary), use the

%I{xxx} placeholder as follows:

For Output File enter %N.xxx%I{.info}

Here %N stands for the board name, xxx stands for any characters for the file

extension, %I{.info} generates an additional extension .info for the Gerber

info files.

The output files generated will look like this:

Gerber file: boardname.xxx

Info file: boardname.xxx.info

Example:

The board myboard.brd is loaded. The File field contains %N.cmp

%I{.info}. The output file is called myboard.cmp, and the info file is

named myboard.cmp.info.

The files will be written into the same directory as the board file is.

Drill Data Generation with Separate Rack File

If you prefer drill data in another data format, for example Sieb&Meyer 1000

or 3000 (SM1000, SM3000) or the Excellon format with a separate rack file

(EXCELLON_RACK), a drill table is required first.

Define a Drill Configuration (Rack) File

This file is usually created by drillcfg.ulp (RUN command) started directly in

the Layout Editor window and will be named boardname.drl.

It is of course also possible to define a drill table with the aid of a text editor.

For data generation enter the table's path and file name in the CAM

Processor's Rack field.

Example of a drill configuration file:

0-0$0-0

0.0$0->

010$01.

0;0$0;0

090$090

0>0$0A0

317

9 Preparing Manufacturing Data

All dimensions are given here in inches. It is also possible to enter the values

with their unit, e.g. 0.010in or 0.8mm. Comments in drill configuration files

may be used and are identified by a semicolon, which may stand at the start

of a line or be preceded by a space.

Define Job for Drill Data Output

Start the CAM Processor

Load the predefined job excellon.cam, e.g. with File/Open/Job.

Change the output Device to EXCELLON_RACK, SM1000 or

SM3000 and check the parameters. Layers 44, Drills, and 45, Holes,

must be selected only. No other layers! Use the Layers/show selected

menu to get a summary of the active layers.

☞ If you want to have separate files for plated and non-plated

drillings, select here Layer 44, Drills, only and insert a further section

that outputs layer 45, Holes, in a separate file with the Add button

after the following item.

Check with your board manufacturer to see if this is the method they

prefer.

After changing the output device the CAM Processor requires a Rack

file as a tool guide. Type in .drl or click the Rack button and choose

the path to your rack file in the file dialog.

☞ In the event you wish to distinguish plated and non-plated holes:

Add a new section which outputs only layer 45, Holes, into a second

drill file with modified file name. Possibly .hol for holes.

Save the job file via File/Save job with a new name.

A tolerance of ± 2.5% should be allowed for drill diameter selection in

order to compensate rounding errors that possibly can arise during

the conversion from mm to inch and vice versa in the drill table.

Drill Info File

The file name.dri is generated with each drill data output. It contains the list

of used tools and further information about the data format.

If the error message DRILLS MISSING – NO PLOTFILE HAS BEEN

PRODUCED appears, the info file contains information which drill diameter

could not be found in the drill table. Add the missing diameter in the drill

table with a text editor or check the given values for tolerances.

The info file is written into the same directory as the output file. You may

send this file to your PCB manufacturer, if requested.

9.8 Device Driver Definition in eagle.def

Output device drivers are defined in the eagle.def text file. Here you will find

all the information that is needed for the creation of your own device driver.

The best way is to copy the block for an output device of the same general

category, and then alter the parameters where necessary.

318

9.8 Device Driver Definition in eagle.def

The file eagle.def can be found in the eagle/bin directory.

Creating Your Own Device Driver

Please use a text editor that does not introduce any control codes into the file.

Example 1: Gerber(auto) device, Millimetre

/77112

8H(&!X

\KH(&H!X\

=&\0-P000000600000050.\

"&\P000000600000050.70.\

"P.9;00

"6.9;00

(!\\

7M\PY0>6Y0>50.\@%38B

5<\PY0>6Y0>50-\@%38B

E!"(\PY0>6Y0>501\@%38B

=&"

5=!";

H&)\Y"\@H&)B

V\!]=!V\

\\

\=&E&1$1\

\=&=&"-'-000\

\5&7K"!)&\

\^)HH""=\

\+V!J\

\\

/+77112

,7711

\=&()&G<(! !G\

(!\\M="""Z

)&H&)\5Y\@H&))KB

E="&H&)-0

7%H&)=F.$0

Example 2: EXCELLON Device, Output with Leading Zeros

[EXCELLON-LZ]

Type = DrillStation

Long = "Excellon drill station"

Init = "%%\nM48\nM72\n"

Reset = "M30\n"

ResX = 10000

ResY = 10000

;Rack = ""

DrillSize = "%sC%0.4f\n" ; (Tool code, tool size)

AutoDrill = "T%02d" ; (Tool number)

FirstDrill = 1

BeginData = "%%\n"

Units = Inch

Decimals = 0

Select = "%s\n" ; (Drill code)

Drill = "X%06.0fY%06.0f\n" ; (x, y)

Info = "Drill File Info:\n"\

"\n"\

" Data Mode : Absolute\n"\

319

9 Preparing Manufacturing Data

" Units : 1/10000 Inch\n"\

"\n"

Units in the Aperture and Drill Table

When automatically generated with the GERBERAUTO driver, the aperture

table contains values in inches.

This is also the case for the drill table which is automatically written into the

drill data file with the output device EXCELLON.

If your PCB manufacturer insists on mm units for aperture sizes and drill

diameters, you can achieve this by altering the GERBER or GERBERAUTO

respectively for the EXCELLON driver.

Use a text editor that does not introduce any control codes to edit the

eagle.def file, look for the line

/2

/+2

and add/edit in this section the lines

=&"

5=!";

In order to change the drill table units look for the line

/P+2

and change:

=&"(

=&"

9.9 Gerber Files for Photoplotters with Fixed

Aperture Wheels

This section goes into more detail on the definition of the aperture table.

Some board manufacturers may perhaps still be using a Gerber plotter that

works with a fixed aperture wheel. In such a case it is necessary to adapt the

aperture table to the restricted facilities of the Gerber plotter. Files for

Gerber photoplotters with fixed aperture wheels are generated with the

GERBER driver. It is essential to confer with your photoplot service ahead of

time, so as to adjust EAGLE to the available apertures. The aperture table has

to be defined manually.

There are various types of apertures. They differ in size and shape. The most

common are circle, octagon, and square. The drawing aperture (Draw) used

for tracks is normally a round aperture.

You must specify the aperture configuration before you can generate files for

a fixed aperture wheel photoplotter. To do this, enter the configuration file

for apertures name.whl e.g. with the EAGLE Text Editor, and then load this

file into the CAM Processor by clicking the Wheel button after selecting the

GERBER device driver (see Set Output Parameters beginning with page 311).

320

9.9 Gerber Files for Photoplotters with Fixed Aperture Wheels

Defining the Aperture Table (Wheel)

The CAM Processor distinguishes Draw apertures from Flash apertures. The

first type is used to draw objects (e.g. tracks). The second type is used to

generate symbols (e.g. pads) by a light flash. Only if draw apertures are

defined can the plotter draw lines. Therefore, if the plotter doesn't

distinguish between draw and flash apertures, you must additionally define

round or octagonal apertures as draw apertures.

The following apertures are available:

Name Dimension

5< =&

) =&

_) !&(

+& =&

&! !&(P%<=&(6

+M! =&P%=&6

Use of aperture shapes in the CAM Processor:

5< <"<=")!&"H&)"

) <")H"M="

_) <""_)H"375"M="

+& <"&!H"M="<=&(

 &("P6="="

&! <"&!"75"

+M! <"H"<=&(=[&P

 6="="

Aperture configuration file example:

50.0)0$00;

5011)0$09O

509."_)0$09O

5-09M!0$0O0%0$010

5-0-&!0$0A9%0$0>0

5--0<0$00;

5---<0$009

The D code determines the tool number, then follows the aperture shape

after at least one blank character, then the dimensions are defined. All values

default to inches, unless a unit is added, for example 0.010in or 0.8mm.

Comments are marked with semicolons at the beginning of a line, or with a

semicolon following a blank character.

Aperture Emulation

If objects exist in a drawing which is not compatible with the available

aperture sizes, it is possible to emulate the desired dimensions by selecting

the Emulate Apertures option. The CAM Processor then selects smaller

apertures to emulate dimensions which are not matched by aperture sizes.

Emulation results in longer plot times and higher film costs, so it should be

avoided whenever possible.

The file name.gpi indicates which apertures are emulated.

321

9 Preparing Manufacturing Data

This

page

has been

left free

intentionally.

322

Chapter 10

Appendix

10.1 Layers and their Usage

In Layout and Package Editor

-H J"3&H"=

.)&. !8

1)&1 !8

;)&; !8

9)&9 !8

>)&> !8

A)&A !8

#)&# !8

O)&O !8

-0)&-0 !8

--)&-- !8

-.)&-. !8

-1)&-1 !8

-;)&-; !8

-9)&-9 !8

->X J"3KX"=

-A" "@&()((!B

-#:=" :="@&()(!!!8"B

-O)& =!="@)KKK"B

.05="= )&!="@=!"V(!"BB

.-&! =!J"3&H"=

..K! =!J"3KX"=

.1&+==" +=="3&H"=@&)&$B

.;K+==" +=="3KX"=@&)&$B

.9&" M=H=&3&H"=@H&7B

.>K" M=H=&3KX"$@H&7B

.A&:!)" H&:3&H"=

.#K:!)" H&:3KX"=

.O&&H !"&H"J3&H"=@$)&$B

10K&H !"&H"J3KX"=@$)&$B

1-& !3&H"=

1.K !3KX"=

11&E=="( E=="(3&H"=

1;KE=="( E=="(3KX"=

19&!) !)"J3&H"=

1>K!) !)"J3KX"=

1A&"& "&L)"&&=VG3&H"=

1#K"& "&L)"&&=V$3KX"=

1O&4H)& "&=&"VH&"3&H"=

;0K4H)& "&=&"VH&"3KX"$

;-&"&=& "&=&"VHH3&H"=

;.K"&=& "&=&"VHH3KX"=

;1M"&=& "&=&"VM="

;;5=!!" )G&()((!"

;9*!" )G(!"

323

10 Appendix

;>7=!!= 7=!!=

;A7")" 7")"

;#5)& 5)&G

;OV VJ"

9-&5) 5&=!&H"H=&

9.K5) 5&=!KX"H=&

In Schematic, Symbol, and Device Editor

O07)!" 7)!="&"H&"

O-&" &"

O.)""" )"""

O1=" GH=&"V"8K!"<=&(=G!=VG

O;8K!" (H"VH&"

O9" "VH&"8K!"

O>:!)" :!)"'H&&8H"

OAV =G!=VG'(=&"

O#)= )==!="V"8K!!=&

B*!"&=!"<=&(&(==&=&(="!8$

(8)"&H!"&=G"&()&)&$

Layers can be used with their names or their numbers. Names can be

changed with the LAYER command or in the DISPLAY menu. The functions

of the special layers remain.

If you want to create your own layers, please use layer numbers above 100.

Use the DISPLAY menu to create new layers (New button) or type the

LAYER command on the command line. If you want to create, for example,

layer 200, Remarks, type in:

6.00J"

To set up color and fill style of this layer use the DISPLAY command.

10.2 EAGLE Files

EAGLE uses the following file types:

Name Type of le

$K 8)&

$"( (G

$!K =K8

$K! 5"=!J !

$)!H ")

$" =H& !

$&%& %& !@!"&(")`%"B

$) 5"=)!"

$&! &!H&V&()&)&

$H )&)&H&! !

$LK )&)&LK

$Kaa J)H !VKN ="(=

 &()&)&

$ 7""LK

$KR% J)H !V5@%-$$OB

$"R% J)H !V*@%-$$OB

$!R%  J)H !V@%-$$OB

$KRR  )&GKJ)H !V5

$"RR  )&GKJ)H !V*

$!RR )&GKJ)H !V

EAGLE for Linux only creates and recognizes lower case

characters in file endings!

324

10.3 EAGLE Options at a Glance

In order to output manufacturing data, for instance, with the CAM Processor,

EAGLE can be started directly from a terminal window under Linux and

Mac, or from a console window under MS Windows.

Since Windows programs give up their connection to the console they have

been started from, you can use the file eaglecon.exe (located in the eagle\bin

subdirectory of your installation) if you want to run the CAM Processor from

a batch file.

This version of EAGLE is exactly the same as the eagle.exe, except that it

doesn't disconnect from the console.

Type eaglecon -? for a list of CAM Processor options.

The following options are permitted:

 ""K!8M=&

 %)&=M

5%%% 5<&!@0$--0YB

%%% 5=!!&!@0$--0YB

E%%% E!"(&!@0$--0YB

D )HH""""HH&"

+D +HG=FHM&

%%% !XH@!8HB

%%% 5=!!J !

%%% =H& !

%%% GV! !

%%% H&)<(! !

P %)&7""

D "=GM=&"

%%% 5M=@bV!="&B

 )!&H&)"

VD E=!!H"

(%%% (=(&@=(B

 7=)&H)&

%%% +)&H)& !'(!

H%%% =&@B

_ U)=JH!&

 &&)&H)&O0"

"%%% !V&

M%%% M!=&8

) &&)&H)&-#0"

<%%% <=&(@=(B

%%%% +["&P@=(B

8%%% +["&6@=(B

Where:

xxx "&"VV)&(&3$$ !"<=&(-W=!

)K"<=&(-s$

%H!"-W'(')"'!'HL&'H&)$<(!

-s-$.9

-5V)!&VHG="[

+ 5V)!&VHG="

%H! H&))!G

D=X

H&))!G[

E!HG"@$$BK)"<=&()&HG&(CC(&

 H&))!G3=)&H)&

5 =&!M!)"

V&(=""=3&(M!)HH!="&=&(=G3

+"== "H"=GM&!3

-GM&!$

325

10 Appendix

50$-0 L)"&"&(<&!&-0Y

5D0$-50$09L)"&"&(<&!&D-0Y9Y

Notes on the individual options:

-A Specify the name of an assembly variant

Start the CAM Processor (-X) with this option in order to generate

data for a special assembly variant. If you do not use -A, EAGLE

creates data for the default variant.

-C Execute a command

After loading an EAGLE file the given command will be executed in

the Editor window's command line. See also help function,

Command Line Options.

-D Draw Tolerance (0.1 = 10 %):

Default: 0

-E Drill Tolerance (0.1 = 10 %):

Default: 0

-F Flash Tolerance (0.1 = 10 %):

Default: 0

-N Suppress messages:

This option suppresses warnings or other information in the console

window (DOS box, Linux console). Thus CAM jobs run without

interruption. Default: off

-O Route-Optimizing:

With this option the route-optimizing for the plotter can be turned

on and off. Default: on

-P Plotter Pen (layer=pen):

If you use a color pen plotter, you can determine which layer is to be

drawn in which color. Example: -P1=0 -P15=1

-R Drill Rack File:

With this option you define the path to a file with the drill

configuration table.

-S Script File:

When opening the editor window, EAGLE executes the eagle.scr

file.

This option allows a different name or directory to be selected for

the script file. The script file is not read by the CAM Processor.

-U User Settings File:

This option can be used to define the location of the eaglerc file

where EAGLE stores user settings. The file can have any name.

In case you are working with EAGLE beta versions and you want to

keep things separate from the official releases, you should start

EAGLE with this option.

-W Aperture Wheel File:

This option defines the path to the wheel file which should be used.

-X Calls command line version of the CAM Processor

326

10.3 EAGLE Options at a Glance

-c Positive Coordinates:

If this option is set the CAM Processor creates data without negative

coordinates. The drawing is moved to the zero-coordinates. This

option can be turned off with the option -c-. Please be careful with

this option, especially if you use mirrored and rotated drawings,

because negative coordinates normally cause problems. Default: on

-d Device:

This option determines the output driver. eagle -d? displays a

list of the available drivers

-e Emulate Apertures:

If this option is selected, apertures that do not exist are emulated

with smaller apertures. Default: off

-f Fill Pads:

This option can only work with generic devices like Postscript.

Default: on for all devices

-h Page Height (inch):

Printable region in the y-direction (in inches). The Y direction is the

direction in which the paper is transported. See also -w.

-m Mirror Output:

Default: off.

-o Output File Name

-p Pen Diameter [mm]:

EAGLE uses the Pen-diameter measurement to calculate the

number of lines required when areas are to be filled. Default: 0

-q Quick Plot:

Generates a draft or fast output, which only prints the frames of

the objects. Default: off

-r Rotate Output:

Rotates the output by 90 degrees. Default: off

-s Scale Factor:

Those devices which cannot change their scale-factor (in the

menu of the CAM Processor), have a scale factor of 1. Default: 1

-u Rotate Output by 180 degrees:

In combination with -r+ one can rotate by 270 degrees. Default: off

-v Pen Velocity in cm/s:

This option is for pen plotters supporting different speeds. To select

a plotter's default speed, use a value of 0. Default: 0

-w Page Width (inch):

Printable area in x direction. See also -h.

-x Offset X (Inch):

This option can be used to move the origin of the drawing.

Default: 0

-y Offset Y (Inch):

Default: 0

Example for starting eaglecon.exe

327

10 Appendix

Gerber data for solder (bottom) side of a board:

!$%-X-d.A;P-o$HK$K--A-#

Gerber data for component (top) side of a board:

!$%-X-d.A;P-o$"!K$K->-A-#

Gerber data for silk screen top side:

!$%-X-d.A;P-o$H!K$K.0.-

Gerber data for solder stop mask component side:

!$%-X-d.A;P-o$"&K$K.O

Gerber data for solder stop mask solder side:

!$%-X -d.A;P-o$"&"K$K10

Gerber data for solder cream mask top:

!$%-X-d.A;P-o$K$K1-

Drill data in Excellon format:

!$%-X-dP+o$!K$K;;;9

Gerber data generated with an older Gerber device with separate aperture

file for the solder side of a board. Draw apertures may have a negative

tolerance up to 10 %.

!-X-dK-WH&)$<(!-oK$"!-D0$-

$KHM=KX

All parameters have to be written in a common line!

Paths that include space characters must be set into double quotes!

10.4 Configuration of the Text Menu

With the help of a script file (e.g. menu.scr) you can configure your own text

menu.

R7)&)H

R

R(="="%H!&(&"(<"(<&"&)HH!%

R)3=!)=")K)"!=""$

7C/"=!=J..$H2(S

!)"=!=J$)!H!I

(G)"=!=J$)!H

TC

C=S

7&=S

E==0$-I

"=-

TI

H=!S

E===(0$00-I

"==(0$-

TI

+=+I

+[=+[

TC

C5="H!8S

H5="H!8H":="5=I

X5="H!8&":="5=I

!H!S

328

10.4 Configuration of the Text Menu

H5="H!8&!5=I

X5="H!8K!5=

T

TC

C---C

CE=&=<E=&C

5!&7MCC=&U)=&



The backslash \ at the end of a line shows that a command continues in the

next line. Here the MENU command runs from the first line after the

comment to the last line.

The pipe sign | has to be used if a command within braces { } is followed by

another command.

The MENU command can handle small images as shown in the example

above with designlink22.png. The images are expected to be in the eagle/bin

folder by default. It is also possible to use a path with the image name.

10.5 Text Variables

Text variable Meaning

?7 H&@M&)!!8D&B-B

?: H&M!)'&8H-B

? H&.B

? &.B

?7+5 7)!@!8)!"(&"B

?* (&)KV=)=&==&(V

V3V%H!-'11B

?**5 ((!=V&("(&"=HG

?*+ (&)K=(=(=!"(G=&(VV

?*+'?*+

?* &!)KV"(&"1B

?*+ &!)KV"(&"=!)=&()!"(&"

?* )&"(&)K1B

?*+ )&"(&)K=!)=&()!"(&"

?76: V""K!8M=&

?57 5<=

?57 =V&(!"&= G

?+57 =V&(H!&G

-B+!8VHJ"8K!

.B+!8V"8K!

1B+!8V"8K!=)=&=

All texts starting with the character >, will be interpreted as placeholder texts

for attributes. See ATTRIBUTE command.

10.6 Options for Experts in eaglerc

The user-specific file eaglerc.usr for Windows and .eaglerc for Linux and Mac

stores various settings defined during the work with EAGLE. Among them

you find some expert settings that can be adjusted in this file directly. The

most important of them are listed here.

Since version 5.2 it is possible to change these parameters with the help of

the SET command in the command line. Please see the help function about

the SET command for details.

329

10 Appendix

CAM Processor – Suppress Drills/Holes Warning

If you want to suppress the warning that you should activate the Drills and

the Holes layer for generating Drill data, write the following line in the

eaglerc file

=$$5=!!"*!")&\0\

Change Component Value Warning

Some users don't want the warning message about a part not having a user

definable value, so this warning can be disabled by appending the line

=$&*""5 K!:!)\0\

to the file.

Consistency Check

In order to handle Board/Schematic pairs that have only minor

inconsistencies, the user can enable a dialog that allows him to force the

editor to perform Forward&Back Annotation, even if the ERC detects that

the files are inconsistent. This can be done by appending the line:

$!!<"+M="="&8(J\-\

PLEASE NOTE THAT YOU ARE DOING THIS AT YOUR OWN

RISK!!!

If the files get corrupted in the process, there may be nothing

anybody can do to recover them. After all, the ERC did state that the

files were inconsistent!

Delete Wire Joints

If you absolutely insist on having the DELETE command delete wire joints

without pressing the Ctrl key, you can append the line

$5!&$=W=&"=&()&&!\-\

to the file.

Device Name as Value for all Components

Some users always want to use the device name as part value, even if the part

needs a user supplied value. Those who want this can append the line

($$$!<8""5M=":!)\-\

to the file.

Disable Ctrl for Radius Mode

If you don't like the special mode in wire drawing commands that allows for

the definition of an arc radius by pressing the Ctrl key when placing the wire,

you can add the line

$=$&!E=)"7\-\

to the file. This will turn this feature off for all commands that draw wires.

330

10.6 Options for Experts in eaglerc

Group Selection

Since the context menu function on the right mouse button interferes with

the selection of groups, a group is now selected with Ctrl plus right mouse

button. If you want to have the old method of selecting groups back, you can

add the line

+HG$!&!E)H!G&%&7)\-\

to the file. This will allow selecting groups with the right mouse button only

and require Ctrl plus right mouse button for context menus.

Load Matching File Automatically

If you have a board and schematic editor window open and load another

board (or schematic) in one of these windows, and if that other drawing has a

matching schematic (or board), EAGLE asks whether that other drawing

shall also be loaded. By setting

+HG$)&7&(=5<=E=!\-\

this query will be suppressed.

Name of Net, Busses, Signals and Polygons

If a net consists of more than one segment, the NAME command by default

acts only upon the selected segment. In order to rename the entire net set

$$G&85V)!&\-\

This parameter also applies to busses.

If a signal contains a polygon, and the NAME command is applied to that

polygon, by default only the polygon gets renamed. Setting

$$G=!85V)!&\-\

makes the NAME command act upon the entire signal by default.

Open Project

The automatic opening of the project folder at program start (or when

activating a project by clicking onto its gray button) can be disabled by

appending the line

&!!$:=<$)&+HL&E!\0\

to the file.

Panning Drawing Window

Panning can be done with the Ctrl button (as in previous versions) by writing

&V$"&!E=\-\

into the file. Note, though, that the Ctrl key is now used for special functions

in some commands, so when using these special functions (like selecting an

object at its origin in MOVE) with this parameter enabled you may

inadvertently pan your drawing window.

Polygon Edges as Continuous Lines

If you don't like the way unprocessed polygons display their edges (as dotted

lines), you can add the line

+HG$5<H""!8"G))"\-\

The edges of polygons will be displayed as continuous lines then.

331

10 Appendix

Reposition of the Mouse Cursor

Normally EAGLE does not automatically position the mouse cursor.

However, if you prefer the cursor to be repositioned to the point where it has

been before a context menu in the drawing editor was opened, add the line:

+HG$H"=G7)")"N&%&7)\-\

Units in Dialogs

The automatic unit determination in dialog input fields can be controlled by

appending the line

&V$V=&\%\

to the file, where "x" can be

"0" for automatic unit determination (default)

"1" for imperial units

"2" for metric units.

10.7 Error Messages

When Loading a File

Restring smaller than in older version

In EAGLE version prior 4.0 the pad diameter has been fixed in the Package

definition. Due to the given values in the Design Rules the pad diameters

have changed.

Please check and, if required, change the Restring settings. Run the Design

Rule Check in any rate to recognize possible clearance errors.

Library objects with the same names

The Text Editor shows this message if you attempt to load an older file (BRD

or SCH) that contains different versions of a library element. In this case it

added @1, @2, @3... to the names of the Devices so that they can be

identified.

332

➢

Pad diameter changed

10.7 Error Messages

This message can also appear if you use COPY and PASTE commands.

Pad, Via Replaced with a Hole

In older versions of EAGLE it was possible to define pads in which the hole

diameter was larger than the pad diameter. This is no longer permitted.

If you attempt to load a library file that was created with an earlier version

and that contains such a pad, the following message appears:

The pad or via is automatically converted into a hole, provided it is not

connected by CONNECT to a pin in one of the library's Devices.

If there is pad that has a connection to a pin (it is defined in the library), the

following message appears:

333

➢

Update report: Objects with the same name

➢

Update report: Via replaced with hole

10 Appendix

In that case the Library file must be manually edited in order to correct the

pad. Then you can update the board file with the new library definition.

Skipped unsuitable objects

If this message is shown, while you are loading a file or copying objects with

COPY and PASTE from one file into another, the data structure contains

objects that do not belong to the current file type and can't be displayed. For

example, a text or rectangle that has a non-orthogonal angle and is placed in

a user-defined layer (above 100) in the Layout editor which should be pasted

into a schematic. The Schematic editor doesn't allow non-orthognal angles

and therefore can't display such an object.

This message could be prompted as well, if the file's origin is one of the first

EAGLE versions. The file can be used without problems nevertheless. The

data structure is cleaned up automatically while loading it.

Can't Update File

If this message appears when loading an EAGLE file that was made with a

version earlier than 2.60 it is necessary first to convert the file.

The program update26.exe, which is located in the eagle/bin directory, is

used for this purpose.

334

➢

Update report: Pad replaced with a hole

➢

Update error: File older than version

2.6

10.7 Error Messages

Copy the file that is to be converted into the directory containing both

update26.exe and the file layers.new. Then open a DOS window under

Windows, and change into this directory. Type the command:

)H&.>&=$%&

The file is converted, after which it can be read by the new version of EAGLE.

If the conversion is successful, the message in the DOS box is: ok...

If the message Please define replacement for layer xxx in layers.new should

appear, it means that you have defined your own layers in

layout/schematic/library.

Because of the new layer structure used since version 2.6, a new layer

number (greater than 100) must be assigned.

This requires you to edit the file layers.new using a simple text editor,

adding, for example, a new layer number as the last line of the file.

If, for instance, you have used layer 55, and want to give it number 105,

enter:

99-09

In a Library

Package/Symbol is in use

If a Package or Symbol is already used in a Device, no pads or pins which are

already referenced to a pin or pad with the help of the CONNECT comand,

may be deleted . In such a case EAGLE shows the following messages:

But it is allowed to CHANGE or NAME such pins or pads. It's also possible to

add further pins/pads with the PIN or PAD/SMD command and you are

allowed to DELETE pins/pads which are not referenced via the CONNECT

command.

This message also appears, if you try to remove the whole Package/Symbol

from the library with the REMOVE command. You have to delete the whole

Device or the Package variant or symbol in the Device before.

In the CAM Processor

Polygon may cause extremely large plot data

This message appears, if you selected a layer in the CAM Processor which

contains a signal polygon in the layout whose line thickness is less than the

resolution of the selected output driver (Device).

335

➢

Error while editing Package or

Symbol

10 Appendix

In order to avoid unnecessary large plot files you should assign a higher value

to the polygon's line width (CHANGE width).

In the Free or Standard Edition

Can't perform the requested action

This message is shown if the limits of a smaller Edition are exceeded. This

can be the case, for example, if you want to place a part outside the Layout

size limits, if you want to start the Autorouter, or set parameters for the

Follow-me router, although there are parts outside the Layout limits, or you

want to define a not allowed inner layer.

336

➢

Polygons with width 0

➢

Free/Standard limits

Index

3D board 167

3D package assignment 234

Action toolbar 50, 53

Addlevel 267

Always 275, 277

Can 275

Must 275, 276

Next 275

Request 275

Airwire 26

Calculate 76

Display/hide 76

Alias 97

Deleting 98

ALIGN 22, 69

Alpha blending 108

Alt-X 45, 64

Aperture 320

Aperture File 296

Attributes

Defining 61, 127, 271

External device 274

For elements 127

Global 127

Search 116

VALUE 265

Automatic Naming 99

Autorouter 76

Backup 218

Blind vias 180

Bus router 205

Continue existing job 213

Control file, ctl 221

Control parameter 213

Controlling 204

Cost factors 213

Cutout polygon 209

Design rules 206

Effort 211

Features 203

Hints 222

Information 218

Interruption 218

Layer selection 208

Load settings 211

Log file 220

Memory requirement 208

Menu 210

Micro via 217

Min. distance, clearance 206

Min. routing grid 203

Module 33

Multilayer board 208

Net classes 206

Optimization 205

Placement grid 206

Polygon 216

Polygons as supply 217

Preferred direction 209, 210

Restarting 213

Restricted area 209

Ripup/Retry 216

Routing grid 207

Routing pass 205

Save settings 211

Select signals 211

Single-sided boards 222

Smds and supply layer 222

Status display 218

TopRouter 205

Track width 206

Unreachable Smd 207, 209

Background color 108

Backup files 47, 324

Beep 110

BGA Autorouter 76

Bill of material 300

Blind via 26

Blind via ratio 147

Blind, Buried via 180

Bmp file 101

Board

Arrange components 156

Attributes, global 158

Contour detection 155

Creating 153

Cut-out 282

337

Index

Cutouts 156

Design Rules 144

Draw outline 154

Flip View 20

Layer setup 146

Lock component 71

Multilayer 178

Multiple board 197

Placement grid 154

Prior considerations 143

Quotation 295

Routing manually 161

Board Manufacture 295

Buried via 26

Bus

End automatically 111

Naming 124, 331

CAM Job

Define drill job 318

Description 315

Excellon.cam 305

Extending gerber.cam 315

gerb274x.cam 304

gerber.cam 306

Output parameter 311

CAM Processor 84

Assembly variants 302

Choose pen number 312

Component side 308

Cream frame 309

Creating device driver 319

Drill data 297, 309

EPS output 299

Error: Apertures missing 316

Error: Drills missing 318

Extremely large plot data 335

File extensions 310

Fill Pads 313

Finish mask 309

Glue mask 309

HPGL 102

Inner layer 308

Job 314

Load job file 85

Milling contours 309

Plotter 312

Pos. Coords. 313

PostScript 298

Prompt 307

Save time and money 302

Section name 313

Silk screen 308

Solder stop 308

Start 53, 84

Start from batch 325

Tolerance 313

UNC notation 312

Vias 311

Caption 196

Circle

Filled 278

Clearance 147

Cmd key 91

Color

Background 49

Settings 107

Command

Activating 87

Language 91

Line 51, 87

Parameters 52

Text menu 328

Toolbar 51

Commands

ADD 57, 70, 82, 241

ALIGN 22, 69

ARC 60, 74

ASSIGN 62, 89, 105

ATTRIBUTE 61, 75, 83

AUTO 76

AUTO BGA 76

BOARD 53, 154

BUS 60, 124

CHANGE 57, 70, 83, 237

CIRCLE 60, 74, 91, 94

CLASS 62, 123

CLOSE 62

CONNECT 83, 242, 263

COPY 56, 69, 286

CUT 62

DELETE 57, 69

DESCRIPTION 80, 83

DIMENSION 61, 75

DISPLAY 55, 67, 97

DRC 76, 173

EDIT 62, 79, 116

ERC 62, 76, 130

ERRORS 77, 174

EXPORT 63, 91, 100

FRAME 63, 280

FUSIONSYNC 167

GATESWAP 58, 242

GRID 53

GROUP 56, 68

338

Index

HELP 51

HOLE 75, 88, 278

INFO 55, 66, 148

INVOKE 59, 118

IPROBE 20

JUNCTION 61, 121

LABEL 61, 121

LAYER 63, 324

LINE 59, 73

LOCK 71

MAKESPICE 20

MAPTOMODEL 20

MARK 55, 68, 287

MEANDER 72, 190

MENU 63, 105

MIRROR 56, 68, 88, 158, 281

MITER 59, 71

MODULE 61

MOVE 56, 68, 88

NAME 58, 71, 82

NET 60, 120

OPEN 63

OPTIMIZE 72

PACKAGE 63, 83, 284

PAD 80, 235

PASTE 57, 69, 133

PIN 95, 238

PINSWAP 58, 70

POLYGON 60, 74, 164

PORT 62

PREFIX 83, 243

PRINT 64, 195

QUIT 64

RATSNEST 76

RECT 60, 74

REDO 54

Remove 79

REMOVE 64, 116, 291

Rename 79

RENAME 292

REPLACE 58, 70, 160

RIPUP 73, 163

ROTATE 56, 69, 157, 287

ROUTE 72, 161

RUN 53

SCRIPT 53, 100

SET 64, 105, 329

SHOW 55, 66

SIGNAL 75

SIM 20

SIMOPTOGGLE 20

SLICE 59, 72

SMASH 58, 71, 118, 158

SMD 80, 235, 253

SOURCESETUP 20

SPLIT 59, 72

TECHNOLOGY 64, 83, 264

TEXT 60, 73

UNDO 54

UPDATE 64, 188, 292

USE 53, 245

VALUE 58, 71, 83, 243

VARIANT 64

VIA 75, 88, 186

VPPROBE 20

VPROBE 20

WINDOW 53

WRITE 65

Component

Add from library 57

Attribute 127

Changing Technology 161

Copying by Drag&Drop 289

Create symbol 238

Creating 82, 229

Cross-reference 278

Description 237

Editing 187

External 274

Keepout 237

Labeling 236

Lock 71

Name 236

On both sides 158

On bottom side 235, 281

Output list 101

Package editor 237

Placement grid in board 154

Prefix 243

Replace device 160

Replace package 159

Replacing 58

Rotation 156

Searching 116

Separate name/value 58, 71

Update 187

Value 58, 71, 236

Without package 274

Configuration

Commands 104

eagle.scr 111

eaglerc, eaglerc.usr 113, 329

Location of eaglerc 326

of EAGLE 104

User interface 105

Connector 276

Consistency

Check 62, 76, 104, 130

Indicator 201

Loss of c. 198

Contact cross reference

>CONTACT_XREF 122

339

Index

>XREF 278

Context menu 43, 88

Configure 105

Control Panel 39

Options menu 46

Search in tree 46

Control parameters 213

Coordinates

Display 51, 55, 68

Entering 93

Modifier 94

Polar 94, 287

Relative 94, 287

Select group 94

Copper plane 164

Copying SCH/BRD 132

Core 26, 180

Cost factors 213

Cream mask 152

Cross reference

For contacts 122, 278

For nets 61, 121

Specify format 122

Ctrl key 91

Current units 95

Cursor appearance 49

Cutout-Polygon 179

Data output 84

Date/time stamp 280

Delete

All signals 101

Wire bend 70

Design Block 42, 58

Add to drawing 58

Live DRC 20

Design Blocks 134

Design Rule Check 26, 76

Approve errors 175

Correcting errors 173

Fonts 153

Meaning of errors 175

Restricted areas 153

Show errors 77

Wire styles 178

Design Rules 42, 144

Clearance 147

Definition 76

Layer setup 146

Options 145

Restring 148

Designlink interface 119

Desktop Publishing 299

Device 26

Assign Package 242

Attributes 271

Build Device Set 260

Copying 289

Creating 241

Delete 78

Description 244

Driver 319

Editing 79, 81

External 274

Gate names 242, 261

Open/Edit 187

Placeholder in name 261

Prefix 243

Remove from LBR 291

Rename 78

Replacing 58, 160

Technologies 264

Value on/off 83, 243

Device Set 26

Differential Pair 189

Dimensioning 75

Directories 46

Distance 147

Documentation 40, 300

Export image 101

Print 236

Documentation field 280

Drag&Drop 39

Draw lines 59

Drawing area

Alias 98

Display last 54

Panning 54

Drawing frame 116, 279

Drawing name 280

DRC 26

See Design Rule Check 173

Drill 26

Diameter 278

Display 110

Legend 302

Non-plated 297

340

Index

Plan 301

Plated 297

Symbols 301

Drill data 297

Blind/buried vias 311

Configuration file 317

drillcfg.ulp 317

Error: Drills missing 318

EXCELLON 297

EXCELLON_RACK 317

Info file 318

Leading zeros 319

Multilayer boards 311

Rack 317

Separate rack file 317

SM1000 298

SM1000/SM3000 317

SM3000 298

Tolerance 318

Units 320

Dxf data export 102

eagle.def 318, 320

eagle.epf 114

eagle.scr 111

eaglecon.exe 325

eaglerc, eaglerc.usr 113, 326, 329

ECAD/MCAD

Synchronise 167

Edition

Premium 34

Standard 36

Electrical Rule Check 26, 62, 130

Approve errors 131

Electrical schematic 278

Electrical Schematic 122

Elongation 150

Encapsulated PostScript 299

Environment variable 47

ERC 26

Error messages

CAM Processor 335

Correcting 173

DRC - Meaning of 175

File prior version 2.60 334

In a library 335

Loading a file 332

excellon.cam 318

Exclamation mark 202

Exit program 45

Expert options 329

Export

Libraries 102

Export data 99

Fiducials 303

File

Backup 324

Edit 62

Import 134

Load SCH/BRD query 331

New 44

Open 45, 53

Print 53

Save 53

File Locking 47

Film Generation 298

Fixing hole 277

Follow-me Router 27, 223

Font

Checking 153, 177

No vector error 177

Persistent in drawing 48

Typeface 60, 73

Vector 48

Forbidden area 161

Forward&Back Annotation 27, 104

Consistency indicator 201

Consistency lost 198

Function keys 62, 89, 105

Fusion 167

Gate 27, 261

Hidden supply 118

Name 261

Place particular 59

Gateswap 125

Gerber

Extending gerber.cam 315

341

Index

Fixed aperture wheel 320

Units 320

Gerber device

RS-274D 296

RS274X 296

Gerber output

Aperture configuration 321

Aperture types 321

Arc 314

Draw aperture 321

Emulate aperture 314

Emulation 321

Error: Apertures missing 316

Flash aperture 321

GERBER 306

gerber.cam 306

GERBERAUTO 306

Info files 317

Messages gerber.cam 306

Resolution 296

Wheel 320

Wheel, example file 321

Gestures 49

GND symbol 269

Graphic format 101

Graphics data

Import 103

Grid 95

Alias definition 97

Alternative grid 96

Check 153

Menu 96

Min. visible size 111

Pad placement 234

Group

Default action 111

Define 56, 68

Move 56

Move to sheet 56

Rotate 287

Help function 50, 51

Hierarchical Schematic 137

Hierarchy

Part names in Layout 142

History function 88

Hole 27

Diameter 278

Min. diameter 147

HOME variable 47

Hyperlinks

In descriptions 244

Icons

Scale size 49

5.6 Import 99

ACCEL-ASCII 100

In-circuit tester 299

Inner layer 178

Installation 29

Invalid Polygon 176

Job 306, 314

Junction

Set automatically 111

Keepout 176, 237

Language setting 31

Layer

Abuse 176

Alias definition 97

Available 105

Creating 63

Display/hide 55, 67

Hide unused 105

Inner 178

Qty. of signal layers 146

Setup 146, 179, 181

Single layer mode 163

Stack 27, 180

Thickness 147, 181

Usage 323

342

Index

Layout Editor 33, 65

Layout Editor

Add Design Block 70

Description 154

Length Balance 190

Length tolerance 191

Library

3D package 77, 230

Attributes 271

Composition of your own 291

Copy elements 288

Copying by Drag&Drop 289

Create new 247

Description 245

Device creating 241

Device without package 274

Export 102

Extracting 188

Important comments 26

List contents 100

Managed libraries 41, 229

My Managed Libraries 233

Open 63

Output script file 101

Package creating 234

Package variants 262

Remove element 291

Rename element 292

Search for elements 116

Summary 40

Symbol creating 238

Table of contents 78

Update 188

Update Package 292

Updating older files 30

URN 229

Use 41, 53

Library Editor 77

License

New Installation 29

License information 40, 45

Line 28

Type 73

Logo import 103

Magnetic pads 163

Managed Libraries 229

Meander 190

Configure Text menu 328

Contents parameter menu 106

Menu bar 50

Merge SCH/BRD 132

Message

Automatic confirmation 107

Micro Via

Definition 27, 187

Restring, diameter 148

Set in SMD 187

Milling

Contour 281

Cutout in board 156

Prototype board 298

Milling machine 298

Module 27

Prefix for instance 139

Module instance 27

Port 140

Module sheets

Order 139

Modules

Assembly variants 142

Mounting hole 75, 277

Mouse click 93

Right click 94

Mouse keys 65

Mouse wheel zoom 49

Multi-channel device 134

Multilayer boards 178

4-Layer 181

6-Layer 183

8-Layer 185

Blind, Buried vias 180

Through vias 179

Via display 181

Name

Automatic naming 99

Forbidden characters 99

Length 99

Net 27

Connection point 61

Cross reference 61, 121

Naming 331

343

Index

Net classes 123

Netlist 101

Netscript 101

Object

Move 56, 68

Properties 55, 66

Show properties 49

Oblong holes 281

Obstacle Avoidance 27

Offset 142

ONLINE status 40

Output

Drawing 63, 64

Image 101

Package 27

3D 230

Arbitrary pad shape 282

Assigning 242

Changing 159

Copying 288

Creating new variant 283

Delete 78

Delete variant 285

Description 237

Editing 79

Import 285

In use 335

New 80

Open/Edit 187

Radial pad arrangement 287

Remove from LBR 291

Rename 78, 292

Rename variant 262

Replacing 70

Rotation 286

Search for P. 116

Update in LBR 291

Variants 262

Pad 27

Appearance in Editor 151

Arbitrary shapes 282

Aspect ratio 150

Automatic naming 99

Change shape 238

Diameter 235

Diameter in inner layer 149

Display name in board 110, 249

Display signal names 110

First 150, 248

Form 150

Layer color 151

Magnetic pads 163

Oblong hole 281

Offset pad 150

Radial arrangement 287

Restring, Diameter 148

Shapes 248

Solder stop mask 152

Stop flag 248

Thermals flag 152, 248

Palette 108

Panelize boards 197

Panning 54

Parameter toolbar 50, 52

Parts list 101, 300

Paste buffer 62

PASTE DBL 58, 70

Path specifications 46

Pbm file 101

PDF output 197

Pgm file 101

Photoplotters 320

Pick-and-place data 299

Pin 27

Automatic naming 99

Connection point 120, 240

Direction 239

Function 238

Inverted signal 258

Labeling 239

Length 239

Name 240

Orientation 238

Properties 238

Same names 268

Superimposed 132

Swap 58, 70

Visible 239

Pin/Pad connection 242, 263

Pin/Pad list 101

Pinswap 125

Placeholder

For attributes 273

>CONTACT_XREF 122, 281

344

Index

>DRAWING_NAME 280

>GATE 274

>LAST_DATE_TIME 280

>MODULE 329

>NAME 240, 274

>PART 274

>PLOT_DATE_TIME 280

>SHEET 280

>SHEET_HEADLINE 329

>SHEET_TOTAL 329

>SHEETNR 280

>SHEETNR_TOTAL 329

>SHEETS 280

>SHEETS_TOTAL 329

>VALUE 240, 274

Placeholder texts 329

Plated-through hole 75

Png file 101

Polar coords. 287

Polygon

Calculation on/off 110

Cutout 74

Invalid 166

Isolate 165

Naming 331

Orphans 166

Outline mode after Ratsnest 166

Pour 165

Rank 165

Restricted area 179

Spacing 165

Thermal connector width 166

Thermals 166

Width 165

Port 27

Direction 140

Eigenschaften ändern 141

Export bus 140

Port definition 140

PostScript 298

Power supply 126

Ppm graphic file 101

Prefix 83

Premium edition 34

Prepreg 27, 180

Print out

Date/time 280

Drawing 195

Options 196

Page limit 196

PDF file 197

Printing 64

Project

Close 45

Create new 43, 113

Directory 46

Edit Description 43

File, eagle.epf 113

Mangement 43

Open recent p. 45

Prototype Manufacture 298

Rack file 28, 317

Ratsnest 28

Relative coords. 287

Relay 276

Repetition points 93

Restricted area 161, 277

Cutout polygon 74

For components 237

Inner layer 165, 179

Restring 28, 148

RGB value 107

Roundness 150

Rubber band 26

Schematic

Checking 130

Create sheet 53

Creating 115

Delete sheet 64

Draw nets 120

Drawing frame 116

Duplicate section 132

Editor 33

Global attributes 127

Grid 116

Hierarchical sch. 137

Merge different 133

More than one sheet 132

New sheet 116

Points to note 132

Remove sheet 53

Sheet preview 51

Sheet preview on/off 132

Sort sheets 132

345

Index

Various supply voltages 126

Script files 100

Comments 100

defaultcolors.scr 109

Syntax 90

Search in Libraries 116

Select factor 111

Selecting objects 65

Sheet

Delete 116

Max. number of 33

New 116

Sorting 51, 132

Signal 28

Differential Pair 189

Display name 162

Length 190

Measuring length 191

Silkscreen 236

Single layer mode 163

SLICE 72

SMD

Arbitrary shapes 282

Automatic naming 99

Cream flag 254

Define size 253

Parameter 235

Placement 253

Round shape 253

Roundness 150

Solder cream mask 152

Solder stop mask 152

Stop flag 254

Thermals flag 152, 254

Snap length 111

Solder cream mask 152

Special characters 99

SPICE Simulation 20

Standard edition 34

Status line 51

Stop frame 152

Superimposed pins 132

Supply

Addlevel for gates 275

Autorouting supply layer 217

Invisible pins 266

Layer with polygons 178

Symbol 28, 126, 269

Various voltages 126

Voltages 266

Swaplevel 58, 125, 240

Symbol 28

Copying 288

Creating 238

Delete 78

Description 241

Editing 79, 80

In use 335

Labeling 274

New 81

Open/Edit 187

Power supply 259

Remove from LBR 291

Rename 78

Technologies 264

Technology

Changing 161

Termination

Of command 54

Text

Alignment 60

Bar over text 99

Change size 60, 73

Editor 86

Font 60, 73

HTML text 237

In copper layer 303

Inverted in copper layer 73

Menu 63, 105, 328

Min. visible size 111

Ratio 236

Separate from component 158

Special characters 99

Spin flag 156

Upside down 157, 249

Variables 280, 329

Vertical t. 49

Thermal symbol

In polygon 166, 178

In supply layer 151

Tif graphic file 101

Title bar 50

TopRouter 205

Trace

Display signal name 110

Track

Bend mode 164

Decompose 163

346

Index

Delete all 70

Min. width 147

Set width automatically 111

Smooth wire bends 163

Tree view

Extended mode 45

Update 46

Undo buffer 110

Undo/redo

list 54

Unsmash texts 71

Update

designlink-lbr.ulp 120

User gudance 49

User Guidance 51

User interface 48

User Language 28, 103

User Language Program

bom.ulp 300

Calculate milling contour 298

designlink-order.ulp 119

dif40.ulp 300

drill-legend.ulp 302

drillcfg.ulp. 311

dxf.ulp 102

fabmaster.ulp 300

gencad.ulp 300

List of all 43

mill-outlines.ulp 298

mount.ulp 299

mountsmd.ulp 299

outlines.ulp 298

pcb-service.ulp 295

Start ULP 53

unidat.ulp 300

Value

Placeholder text in package 249

Placeholder text in symbol 258

V. for Device 265

V. is always Device name 330

Warning 330

Variable

$EAGLEDIR 47

$HOME 47

Variant

Creating new 283

Delete 285

Using modified one 285

Vector font 48

Checking 153

Keep legacy vector font 48

New vector font 48

Via 28

Appearance in Editor 151

Blind 180

Blind via ratio 147, 187

Buried 180

Diameter display with INFO 148

Diameter in inner layer 149

Display length 110

Layer color 151

Length 186

Limit 152

Micro via 181, 187

Restricted area 161

Restring, Diameter 148

Shape in inner layer 150

Solder stop 152

Thermal symbol 151

Wheel file 28

Wheel mouse 49

Legacy wheel mode 49

Window

Fetch into foreground 90

Menu 49

Number 49

Store position 49

Wire 28

Bend mode 164

Style 73

Xbm graphic file 101

Xpm graphic file 101

XREF label 122

347

Index

ZZoom factor limit 49

Zoom in/out 53

348

Manual En

Navigation menu

Versions of this User Manual:

Views

Navigation