Eagle Guide
User Manual:
Open the PDF directly: View PDF 
.
Page Count: 12
Autodesk Eagle CAD Guide
Evan Peterson
September 23, 2018
Contents
1 Introduction 2
1.1 WhatisaPCB................................ 2
1.2 EagleIntro .................................. 2
1.3 EagleInstallation............................... 2
2 Libraries 2
2.1 CreateLibrary ................................ 3
2.2 LibraryPart:Symbol ............................ 3
2.3 Library Part: Footprint . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
2.4 LibraryPart:Device............................. 5
3 Schematic 6
3.1 Schematic: Adding Parts . . . . . . . . . . . . . . . . . . . . . . . . . . 6
3.2 Schematic:Wiring .............................. 7
3.3 Schematic: Error Checking . . . . . . . . . . . . . . . . . . . . . . . . . 7
4 Board Layout 8
4.1 BoardLayout:Layers ............................ 8
4.2 Board Layout: Arranging . . . . . . . . . . . . . . . . . . . . . . . . . . 8
4.3 Board Layout: Routing . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
4.4 Board Layout: Polygons . . . . . . . . . . . . . . . . . . . . . . . . . . . 10
4.5 Board Layout: Silkscreen . . . . . . . . . . . . . . . . . . . . . . . . . . 11
4.6 Board Layout: Error Checking . . . . . . . . . . . . . . . . . . . . . . . 11
4.7 Board Layout: Exporting . . . . . . . . . . . . . . . . . . . . . . . . . . 12
1
1 Introduction
1.1 What is a PCB
A printed circuit board (PCB) is used to mechanically support and electrically con-
nect various electrical components. A PCB is designed and manufactured based on how
you want to connect the components then the components are soldered to the PCB.
In its most basic form a PCB consists of a center substrate (typically fr4) with a
layer of copper traces on the bottom and top. Pads are portions of the copper layer that
are in specific shapes so a component can be soldered to it.
1.2 Eagle Intro
Eagle is a CAD tool used to design printed circuit boards (PCBs). The program is
split up into three sections which build upon one another to result in files that are sent
to a PCB manufacturer.
First all parts to go on the board are created in libraries which describe the pins
on the part and the footprint of the part for when it is soldered to the board. Then
these parts are used in the Schematic design which describes the electrical connections
on the board. Then the board is laid out by following the parts and connections made
in the schematic to place parts on the physical board then route where the physical
connections will go between parts.
Tips & Tricks
•Everything in Eagle can be done through clicking buttons or by using its
command line. Design can be done much quicker by learning to use the
command line.
•In order to use some Eagle functions such as creating new files or adjusting
certain settings you must switch back to Eagle’s Control Panel window
1.3 Eagle Installation
1. Download at https://www.autodesk.com/products/eagle/free-download
2. Install Eagle using free or educational version
•Free version: 2 Board Layers, 80cm2Board Area
•Educational version: 16 Board Layers, Unlimited Board Area
–https://www.autodesk.com/education/free-software/eagle
2 Libraries
Libraries are used to store information about a part which are used in the schematic
and the board layout. Eagle has built-in libraries for many common parts but very often
you have to make your own.
Libraries are split into three parts. Symbol, Footprint and Device. The Symbol
is what is seen in the schematic and is how you describe the pins on your part which
electrical connections go to. The Footprint is the exposed metal part used for board
layout which you will solder the component to on the physical board. The Device brings
the Symbol and Footprint together so what is created in the schematic can be translated
into the board layout.
2
2.1 Create Library
1. (At Control Panel) File→New→Library
2. Save to a directory where you will keep all Eagle libraries
Tips & Tricks
•Libraries are commonly split up into components types such as resistors or
connectors
•Eagle has a default folder it searches for its libraries, but you can
have it search additional folders for your libraries by (At Control Panel)
File→Options→Directories then appending to the Libraries path a
colon then the path to your directory
2.2 Library Part: Symbol
1. Create new symbol: Library→Symbol
2. Name symbol with part number
3. Draw box using wire (Type into console or select GUI icon from left)
•This aspect is purely visual so any size/shape is okay, but use standard sym-
bols which are commonly represented in schematics helps everybody under-
stands your work.
4. Add necessary amount of pins using pin
•These pins are what wires are connected to in the schematic
5. Name pins corresponding to datasheet using name then click on pin
6. Clean up Symbol: Adjust part outline so all pins fit and pin names can be seen
7. Add Name and Value using text
•>NAME and >VALUE are keywords for text that are automatically filled
out with the name and value when inserted into a schematic.
8. Change Layer of Name and Value using info then clicking on the part and changing
Layer to Name and Value respectivly
9. Return to Library: Library→Table of Contents
Tips & Tricks
•Always keep pins snapped to the 0.1 in grid (Hold option/alt and click
components to snap them).
•Right click while placing or moving to rotate.
•To move a group use group, select what you want to move then Right
Click→Move:Group.
•Objects are clickable and selectable from the grey + symbol when they
have been inserted into schematics/layout.
3
Figure 1: Example of completed symbol
2.3 Library Part: Footprint
This is typically the footprint for the component which is found in the datasheet for
the part. In the datasheet you will find all measurements needed to create the foorprint.
This footprint will go on the PCB and is what the component will be soldered to. Before
version 9.0, Eagle uses ’package’ for ’footprint’.
1. Create new footprint: Library→Footprint
2. Name footprint with package name
•Common for multiple parts to have the same footprint.
3. Place first pad
•Place surface mount using SMD
•Place through hole pad using pad
4. Resize pad using info clicking on pad then changing SMD size to size given in
datasheet
5. Use copy to copy correct amount of pads and place them in approximate positions
6. Use values given in datasheet to calculate position (to pad center) for each pad
then move pads using info and change position values
7. Rename pads using rename. Pad numbers given by datasheet
8. Add part outline using line then changing Layer dropdown to 51 tDocu then
draw basic part outline
•The tDocu is just for reference to ensure no overlapping parts so it will not
appear on the board.
9. Adjust part outline to the dimmensions given on the datasheet. Adjust to exact
values using info
10. Add silkscreen
•Silkscreen gets printed on the board and is used to help place components
4
•Draw lines on the 21 tPlace layer as an outline that does not intersect with
pads
•Add a dot to indicate where Pin 1 is on component to help when soldering
component
11. Add Name and Value using text
•Use >NAME and >VALUE similar to in symbol
•Adjust Layer to Name and Value respectivly
12. Return to Library: Library→Table of Contents
Tips & Tricks
•Change grid size using grid
–Change grid size to whatever is helpful to you.
–Use same units as given in datasheet. Values for position and size are
in these units.
–Create vias/pads that are bigger than physical component sizes will
help you phenomenally.
–Recommended: Size = 0.5mm, Alt = 0.25mm.
•Use positions such that (0,0) is at the center of the component
Figure 2: Example of completed footprint and how the physical component goes on a
footprint that was created
2.4 Library Part: Device
This is where the Symbol and Footprint come together to create what will be added
to the schematic.
1. Create new device: Library→Device
2. Name with general part number
•Not footprint specific because a single device can have multiple footprint
5
3. Add symbol using add then select previously created symbol
4. Place symbol so grey + is in center of component
5. Click new button in footprint window and select local footprint
6. Connect pins by clicking connect button in footprint area
7. Use datasheet to see what pin names correspond to what pad numbers then connect
by selecting pin and pad then click connect. Repeat for each one
8. Click prefix button to add current prefix to match component type
Tips & Tricks
•A wildcard character *can be used in Device name to allow you have names
for different versions of the part without creating a new device. Example:
You have parts A45C and A46C that have the same pins and footprint,
but have some minor internal difference. You can name device A4*C then
specify two technologies: 5 and 6.
•You can add multiple footprints and set the variant name to specify the
footprint. This variant name is appended to the end of the Device name
•Done with library part and ready to be added to schematic
•Many more parts can be added to this library. Parts that share footprints only
need footprint to be created once so check if that footprint exists first so you don’t
have to remake it.
3 Schematic
Schematics are used to set up how the board is organized by adding all the parts
used on the board and making the electrical connections between these parts.
1. (At Control Panel) File→New→Schematic
2. Save to a directory where you are storing this project
Tips & Tricks
•Always keep parts and wires snapped to 0.1 in grid
3.1 Schematic: Adding Parts
1. Prepare Eagle with necessary libraries
•Libraries can be added by automatically searching a folder as shown in section
2.1
•Libraries can also be temporarily added by Library→Use then select library
you created
2. Add components using add then select the library containing the component then
select the component
6
•Add a frame to keep schematic organized
•Add all components needed for schematic
•Resistors and Capacitors are found in rcl library. R-US and C-US are the
parts commonly used and the SMD footprint 0603 is commonly used (parts
named R-US R0603 and C-USC0603 respectively)
3. Change value of parts using value
•This value has no effect on the board, only used as reference
Tips & Tricks
•When adding components you can search for components but Eagle uses
exact matching so you must add wild cards. Example: you want to search
for part number containing 0603, search using *0603*
3.2 Schematic: Wiring
1. Organize components
•Components need to be placed in a way so it is easy to read
2. Use the net tool draw connections between components
•NOT the wire tool. The wire tool is only used for visuals, does not make
any actual connections
3. Connect power and ground using parts from the supply library. All supply parts
that are the same on a schematic are connected together
•Good practice to have ground supply parts pointing down and power supply
parts pointing up
Tips & Tricks
•Connections can be made without running nets between components. This
is done by using name on a multiple nets and naming them the same thing.
All nets with the same name are treated as being connected.
–Pins cannot be named, add a short net connecting to the pin then
name that net
–Name these nets something useful so it is easier to follow
–To see that nets are named the same and connected, you can use label
on a net and place the label at the end of the net
•Connections can be checked with show
3.3 Schematic: Error Checking
•Use the Electrical Rule Check (ERC) to check for electrical errors and warnings
•The ERC is often useful to show connections you missed
•Many warnings can be ignored from the ERC because they often have to do with
net names, etc.
7
4 Board Layout
The board file is how you layout the final physical board. All steps up to this point
have been to assist you in the creation of this.
1. When done with schematic switch to board by File→Use
•If no board file is found one will be generated
•It is generated with parts from the schematic randomly placed and lines
showing the connections to be made between parts called airwires
4.1 Board Layout: Layers
•What is actually printed:
–Top Silkscreen (printed on top of board for reference, typically white)
–Top Soldermask (applied over copper to protect from solder, typically green)
–Top Copper (makes electrical connections and components are soldered to)
–Substrate (FR4: used to support and separate copper layers)
–Bottom Copper
–Bottom Soldermask
–Bottom Silkscreen
•Use layer to adjust what layers are currently viewed
Tips & Tricks
•Right click on Layer settings to create a group of currently viewable layers
or quickly switch between created groups
Figure 3: Sideview of layers that are created when PCB is manufactured
4.2 Board Layout: Arranging
•Use move and right click to rotate
•How you arrange your parts has a large impact on the routing difficulty in the
next step
•First consider the requirements of your board
–Consider the maximize size you want your board to be
–Consider Location of specific parts
∗Specific locations of connectors and other components that need to be
accessible
∗Decoupling capacitors very close to its IC
8
∗Maximum distances parts can be that must communicate
–Consider mounting holes
–Consider clearance with other boards or objects around it
•Then consider what is easiest placement for when you route the board
–Leave space between parts so no parts collide and so you have enough space
for routing
–Group parts together based on function, referring back to schematic. Reduces
required routing distances
–Minimize intersecting airwires. It is much more difficult to route when air-
wires cross
–Recommended keeping as many components as you can on the top layer so
you can use the bottom layer for routing or ground plane
•Use delete to erase existing dimension then use wire with the layer set to 20
Dimmension then draw a new dimension which all your parts are within
4.3 Board Layout: Routing
•Routing is making all the connections shown by the airwires without overlapping
anything
•Two layer board so you can place components and route on the top or the bottom
–Vias are used to connect between the top and bottom layers
•Don’t worry about ground connections yet, a ground plane will be added later
•Use route (not wire)
–Use layer dropdown to select signal layer you are routing on
–Optional selection for walkaround obstacles to assist you with routing to avoid
overlapping based on DRC rules
–Bend style is the angle of wires when routing (good practice to use 45°
angles)
–Width is how wide the copper trace is (recommended 0.3mm)
∗Trace width must be considered for some applications such as power lines
∗Signal wire width should be sizable compare to their footprint.
–Via settings are for size and shape of via (recommended circle with drill of
0.35mm)
•Start from end of an air wire and route to the other end of that airwire
•Left click when routing to place segment and continue routing
•Ensure no overlap when routing
–For pads and traces on the same layer there must be zero overlap
–Traces on separate layers can overlap
–Vias and through hole components (colored in green) are on both layers so
traces cannot overlap with these on either layer
9
•Vias can be added by changing layers while routing (using middle click), or change
layer (in top left drop-down list) or by adding manually with the via tool
–Vias added manually do not have the net automatically set so must use name
to change name of via to same as net you want to connect it to
•Different PCB manufacturers have specifications for the minimum distance they
can produce between traces
–You must ensure your traces are at least that far apart
•Traces and vias cannot be removed with delete, you must use ripup
Tips & Tricks
•Right click while routing to switch bend styles
•Use ratsnest to recalculate airwires to shortest length
Figure 4: Example of allowable routing connections
4.4 Board Layout: Polygons
Polygons are how large sections of copper (like ground planes) are done. Using a
ground plane allows you to connect many ground pins without routing as well as other
benefits.
1. Use polygon to draw the shape around you want to fill
•For ground plane you typically want to fill the whole board so draw the
polygon along the dimension lines
2. Use name to connect this polygon to the net with the same name
3. Use ratsnest to fill in the polygons
10
Figure 5: Example of Good vs Bad Routing Plans
Tips & Tricks
•Change the polygon’s rank when you have intersecting polygons to give one
higher priority
•Add polygon inside of another and change Polygon pour to cutout if there
is a section of the board you don’t want a polygon
•Check or uncheck thermals based on application (typically good idea to use
when polygon overlaps pads so the component is easier to solder on)
4.5 Board Layout: Silkscreen
•Silkscreen is printed on the top and bottom of the board and has no effect on the
function of the board. Rather it is used to identify parts on the board and to help
with component soldering.
•Most of the silkscreen comes from individual parts on Names layer identifying part
names
•Often these names for parts are misaligned. Use smash on the component to
allow you to move these labels
•Add other markings to silkscreen on layers tPlace or bPlace for the top and bottom
silkscreen respectively
4.6 Board Layout: Error Checking
•Use ratsnest then check the notification at the bottom left for how many airwires
are left to see if there is stuff left to route. Everything is routed if ”Nothing to do”
•Use the Design Rule Check (DRC) to check for clearance, overlap, etc
11
Figure 6: Example of fully completed board
•Settings of DRC can be changed to fit the requirements of where your board is
being printed
•When ”Ratsnest: Nothing to do” and ”DRC: No errors” you are done
4.7 Board Layout: Exporting
You must export the board into Gerber files which are sent to the manufacturer to
print. This is a set up multiple files, one for each layer
1. Use File→CAM Processor then File→Open→Job and select gerb274.cam
•There is also a 4 layer version of this CAM
2. This exports a file for each layer with the exception of of bottom silkscreen. This
can be added if desired by clicking add and selecting Dimension, bPlace, and
bNames
3. Repeat CAM Processor with excellon.cam job to generate drill file
12
