Manual En

User Manual: Pdf

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

EASILY APPLICABLE GRAPHICAL LAYOUT EDITOR
Version 8.4
Manual
71023841
Copyright © 2017 Autodesk
All Rights Reserved
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.
© Copyright 1988-2017 Autodesk. All rights reserved worldwide.
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.
19
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.
20
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.
21
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.
22
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.
23
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.
24
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.
25
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.
26
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.
27
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).
28
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.
29
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.
30
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:

'(')"'!#$%$%'!
31
2 Installation
This
page
has been
left free
intentionally.
32
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).
33
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
34
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
35
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:
36
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.
37
3 EAGLE Modules and Editions
This
page
has been
left free
intentionally.
38
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.
39
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.
40
➢
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.
41
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.
42
➢
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.
43
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.
44
➢
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
sign in and use EAGLE with his account and entitlements. When starting
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.
45
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.
46
➢
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.
47
➢
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.
48
➢
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.
49
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.
50
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
51
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.
52
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.
53
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).
54
➢
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.
55
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