Rack: Configuration table for a drilling machine. Needed for generating drill data. Ratsnest: Command for calculating the shortest airwires. Restring: Remaining width of the copper ring around a plated-through 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 WIRE command).

Chapter 2 Installation

2.1 What You Have Received
The EAGLE pack, with the license agreement on the outside, contains the EAGLE CD-ROM, a license disk, the User License Certificate with the personal installation code, a training manual and this reference manual. It may be that not all of these items are included if you have asked for an upgrade to an existing Version 4.1 installation or for an extension of your license. In all cases, however, there is a new License Certificate and a new license disk. If your computer is not equipped with a floppy disk drive, you may copy the file license.key from the license disk to another media or, if available, make it accessible through a network computer. Keep the User License Certificate with your personal installation code in a safe place, inaccessible to unauthorized persons! Never give the license file or installation code to others! Never send your installation code by e-mail to CadSoft or to anyone else. You need the license card as evidence of your entitlement to future upgrades or updates.

2.2 New Installations

The CD contains EAGLE for Windows (95, NT 4.0, and above) and Linux. Any particularly recent or additional information about the installation may be found in the README files in the relevant directories on the CD-ROM or on an included floppy disk.

EAGLE Manual Windows

Place the CD-ROM in the drive. After a short delay the CD-ROM startup window should open. If this does not happen, double-click on the CD-ROM symbol in the My Computer folder on the Windows desktop. When the CD-ROM startup window has opened, the first thing to do is to select the language in which you want to work. The user interface, help texts, and additional documentation will be installed in that language. In the next window, click on the Install program item, and then simply follow the setup routine. You will be asked for the license disk as the installation proceeds. Keep it to hand. The program must be licensed the first time it is called. Enter the path to the license file (usually A:\license.key) and your personal installation code, as noted on the EAGLE User License Certificate, into the EAGLE Product Registration window. The program will then start, and will show the license data in the Control Panel. You can display the license data at any time in the EAGLE Control Panel by means of the Help/Product Information menu.

You can either use the RPM or the TGZ archive to install EAGLE on your system. Depending on the selected archive file the user interface, help texts, and additional documentation will be installed in the respective language. The following assumes that you have mounted the EAGLE CD-ROM as /cdrom, and that you are logged in to your system as root user.
Installing the RPM Archive:
Use rpm to install the package:
rpm -i /cdrom/english/linux/install/eagle-4.xxe-1.i386.rpm
By default this package installs to /opt/eagle, but you can relocate it to a different directory using rpms -prefix option. Note that a shell script will be executed that installs a symbolic link to the executable file in /usr/local/bin, and also copies the manual page to /usr/local/man/man1. You can use rpms -noscripts option to avoid this. Enter the command /opt/eagle/bin/eagle to invoke the product registration (you need to have write access to that directory for doing this!).

Installation

Installing the TGZ Archive:
Create a new directory on your system (e.g. /opt/eagle): mkdir /opt/eagle cd /opt/eagle Use tar to extract the archive:
tar xvzf /cdrom/english/linux/install/eagle4.xxe.tgz
Change into the directory that has just been extracted from the archive: cd /opt/eagle/eagle-4.xxe Run the installation script:./install Enter the command bin/eagle to invoke the product registration (you need to have write access to that directory for doing this!).
To use EAGLE you should create a working directory mkdir /home/username/eagle change into that directory cd /home/username/eagle and start the program eagle
2.3 Updating an Older Version
Follow the same procedure described in the section on New Installations on page 15. Please read the file update.txt in the EAGLE directory, in order to familiarize yourself with the changes in the new version of the program. Additional notes on installing an update may be found in the latest README files. For reasons of safety it is good practice to create a backup of your previous data before proceeding! Files from earlier versions can be used directly with the current one. In case the files were made with a version prior to EAGLE 2.60 you have to convert them with a program named Update26.exe. Detailed information about this can be found on page 243.

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 command: Execute a script file. This enables you to execute any command sequence with a few mouse clicks. RUN command: Start a User Language program (ULP).
WINDOW command: These icons represent different modes of the WINDOW command: Fit drawing into the screen (Alt-F2), zoom in (F3), zoom out (F4), redraw screen (F2), display new area. That part of the drawing displayed on the screen can be shifted by holding down the Ctrl key and moving the mouse at the same time. To move the current drawing window click the middle mouse button and move your mouse! Press the Shift key simultaneously and you are allowed to scroll beyoned the drawing boundaries!
UNDO and REDO: These commands allow you to cancel previous commands and to execute commands which have previously been cancelled. Function keys: F9 and F10 (default). Terminates the execution of EAGLE commands (Edit/Stop command). Starts the execution of the active EAGLE command. This is only necessary if further parameters could be entered by the user.
The Schematic Command Toolbar
Provides information about the object to be selected.
Highlights the object to be selected.

DISPLAY

Select and deselect the layers to be displayed. See the Appendix for the meaning of the layers. For further details please see help function.
The following mouse click defines the new origin for the coordinate display. Relative coordinates (R x-value y-value) and polar values (P radius angle) are shown in addition to absolute coordinates in the coordinate display box. If you first click the MARK icon and then the traffic-light icon, only the absolute coordinate values will be displayed again.
Move any visible object. The right mouse button rotates the object. 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 (net) will be created. To move groups of objects: define the group with the GROUP command, click the MOVE icon, then select the group with the right mouse button and move it to the desired location. The right mouse button rotates the group by 90 degrees.
Copy parts and other objects.

ASSIGN

Assign function keys. The most convenient way of doing this is to use the Options/Assign menu.
Select and define net classes (Edit/Net classes.). A net class specifies the width of a track, the clearance from neighboring signals, and the diameter of vias for the Autorouter and the ROUTE command. These settings are also used in polygons.
Text command for closing an editor window (File/Close).
Text command for loading a file or a library object. You can, for instance, load a board from the Schematic Editor (EDIT name.brd).

EXPORT

Output lists (especially netlists), directories, script files, or images (File/Export.).
Choose or define the drawing layer. When using drawing commands the layer can be chosen in the parameter toolbar.
Specifies the contents of the text menu. See also the example in the appendix. The text menu can be made visible with the aid of Options/User Interface. See help function for details.
Text command for opening a library for editing (Library/Open). This command is not identical to the File/Open menu item of the Schematic Editor, which only lets you select schematics. You can use the OPEN command as an alternative to the File menu of the Control Panel.
Call up the print dialog with the printer icon in the action toolbar or the menu item File/Print. Normally the PRINT command is used to print schematics or check the drawings needed for the pcb production. The actual production data are generated with the CAM Processor. If you want to output your drawing in black and white check the Black option (and Solid, if you dont want layers to be printed in their different fill styles). The caption text is suppressed unless you check Caption (available via the Page button). Set Page limit to 1 if your drawing is to be fitted on one page.
Quit EAGLE. Identical with the menu item File/Exit or Alt-X.

REMOVE

Delete files or schematic sheets. REMOVE.S3 for instance, deletes sheet 3 of the loaded schematic.
Set system parameters and modes. Best done via the Options/Set menu item. Please note that not all of the possibilities are available through this dialog. Presettings can be defined in the script file eagle.scr by using text commands. Further information can be found in the help function.

UPDATE

The UPDATE command checks the parts in a board or schematic against their respective library objects and automatically updates them if they are different. (Library/Update. or Library/Update all). The context menu in the Control Panel's' tree view offers the Options Use all and Use none for a quick selection of libraries.

The image above shows three buttons in the Palette column. Click on one of them. For example, the button for Colored Background. The Color window opens now. On the left an 8 x 8 matrix is visible that contains already 16 pre-defined colors. There are alternating eight 'normal' colors with their corresponding eight highlight colors. A color of the palette at position x can be given the corresponding highlight color at position x+8. In order to define new values select an unused box of the matrix and adjust the new color with the help of the color selection area and the saturation bar on the right. Click Set Color to apply your color. Now select a new color box in the matrix and repeat the procedure for the next color. You may also enter values for Red, Green, Blue or Hue, Sat, Val directly.
Color Window: Defining Colors The image above shows four further pairs of colors (normal and corresponding highlight color vertically arranged). In order to change the color palette for an editor window select the appropriate Background in the menu Options/User Interface. Alternatively the color definition and change of palette can be made in a script file or in the command line. SET PALETTE <index> <rgb> defines a color, where the color value has to be given hexadecimal. Example: SET PALETTE 0 0xFFFF00 sets the background color (entry 0) to yellow (corresponds to the decimal RGB value 0 which is hexadecimal FF FF 00). Hexadecimal values are marked by a leading 0x. To activate the black color palette type in the command line: SET PALETTE BLACK The new palette will become visible after refreshing the drawing area with the WINDOW command.
The color assignment for layers is done with the DISPLAY command or with SET COLOR_LAYER. More details about the syntax can be found in the help function.
Miscellaneous SET Options
The Misc tab of the Settings window contains the most common options, which are switched on or off by check boxes. Some options allow entering values.
Settings at Options/Set/Misc Options overview: Beep: Switches on/off the confirmation beep. Default: on. Check connects: Activates the package check while placing parts in the schematic. Default: on. Undo: Switches on/off the undo/redo buffer. Default: on. Optimizing: Enables the automatic removal of bends in straight lines. Default: on. Ratsnest processes polygons: The contents of polygons will be calculated with the RATSNEST command. Default: on. Snap bended wires: If active, wire bends always lie on a grid intersection point. Due to this fact it can happen that traces don't adhere 45 angles. Default: off. Display pad names: Pad names are displayed in the Layout or Package Editor. Default: off.
Auto end net and bus: If placing a net on a pin or a bus the net drops from the mouse cursor. Default: on. Auto set junction: Ending a net on another net a junction will be set automatically. Default: on. Min. visible text size: Only texts with the given minimum size are displayed. Default: 3 pixels. Min. visible grid size: Grid lines/dots which are closer than the given minimum distance are no longer displayed on the screen. Default: 5 pixels. Select factor: Within this radius (given in % of the height of the current drawing window) EAGLE offers objects for selection. Default: 2%. Snap length: Ending a wire with the ROUTE command within this radius around a pad or smd will snap it on the middle of the pad/smd automatically. This is also true for airwires which are dynamically calculated while ROUTE is active. Default: 20 mil. Display mode: Pads/vias are shown with a drill hole (real) or without it (No drills). Default: real. Changes can also be made by typing in the complete SET command. Entering SET POLYGON_RATSNEST OFF or, in short SET POLY OFF for instance switches off polygon calculation for the RATSNEST command. The help system provides you with more instructions about the SET command.

Thermals: Determines whether pads in the polygon are connected via thermal symbols, or are completely connected to the copper plane. This also applies to vias, assuming that the option has been activated in the Design Rules. The width of the thermal connectors is calculated as the half of the pad's drill diameter. The width has to be in the limits of a minimum of the wire width and a maximum of twice the wire width of the polygon. Don't choose the polygon's width too fine, otherwise the thermal connectors won't resist the current load. Orphans: Determines if a polygon may contain areas (islands) which are not electrically connected to the polygon's signal. If Orphans is set Off such un-connected areas won't be drawn. When drawing a polygon, please take care to ensure that the outline is not drawn more than once (overlapping) anywhere, and that the polygon outline does not cross over itself. It is not possible for EAGLE to compute the contents of the area in this case. An error message Signalname contains an invalid polygon! is issued, and the RATSNEST command is aborted. If this message appears, the outline of the polygon must be corrected. Otherwise, manufacturing data cannot be created by the CAM Processor. The CAM Processor automatically computes the polygons in the layout before generating its output.
DRC Checking the Layout and Correcting Errors
The Design Rule Check (DRC) is carried out at the end of the board design, if not before. If you have not yet specified any Design Rules for the layout, this is your last opportunity. See the section on Specifying the Design Rules from page 98. If the DRC finds errors, an error window opens automatically. This lists all the errors. The window can be opened at any time by means of the ERRORS command. If an error in the list is selected, a line points to the corresponding location. The error is marked. Correct the error in the layout. The DRC error window remains in the foreground. Clicking on the Del button will delete the selected error entry. Del all deletes all the error marks from the layout. The dialog is ended with Close.
DRC error list in the Layout Editor Signal layers which are not visible (DISPLAY command) will not be checked by the Design Rule Check!
Error messages and their meaning
Angle: Tracks are not laid in an angle of 0, 45, 90 or 135. This check can be switched on or off in the Design Rules (Misc tab). Default: off. Blind Via Ratio: The limit of the ratio of depth to drill diameter is exceeded. In this case you have to adjust the via's drill diameter (see Design Rules, Sizes tab). Clearance: Clearance violation between copper elements. The settings of the Design Rules' Clearance tab and the value for Clearance of a given net class will be checked. In addition the Isolate value will be taken into consideration for polygons with the same rank and polygons which are defined as part of a package. To deactivate the clearance check between elements that belong to the same signal, use the value 0 for Same signals in the Clearance tab. Dimension: Distance violation between smds, pads, and connected copper objects and a dimension line (drawn in Layer 20, Dimension), like the board's outlines. Defined through the value for Copper/Dimension in the

Example 4: Blind Vias in the Inner Layer Stack

8-Layer Board

Example 5: Layers 1, 2, 3, 4, 5, 6, 7, and 16 are used. Board structure: Three cores, prepregs outside. Connections: 1-3, 6-16 (blind vias), 2-3, 4-5, 6-7 (buried vias), 1-16 (through vias). Setup expression: [3:1+(2*3)+(4*5)+(6*7)+16:6] Explanation: (2*3)+(4*5)+(6*7) Three cores, each with buried vias, are pressed together and isolated with prepregs. 1+(2*3)+(4*5)+(6*7)+16 Outer copper layers 1 and 16 which are isolated through prepregs are pressed onto this layer stack. (1+(2*3)+(4*5)+(6*7)+16) Parenthesis allow through vias from 1-16. [3:(1+(2*3)+(4*5)+(6*7)+16):6] Blind vias from 1-3 and 16-6.
Example 5: Layer Setup for an 8-Layer Board
Hints For Working With Blind, Buried, and Micro Vias

VIA command

Depending on the Layer setup vias can have different lengths. The parameter toolbar of the VIA command shows all available lengths in the Layer box. When routing manually (ROUTE command) EAGLE takes the shortest possible via length in order to change layers. It is also possible that vias at the same position are elongated. The via length can be changed with the CHANGE VIA command. Select the value from the according menu and click the via with the left mouse button. Alternatively use the command line: CHANGE VIA 2-7 and a click on the via changes the length from layer 2 to 7. If the given via length is not defined in the Layer setup it will be elongated to the next possible length or, if this is not possible, an error message will be generated. VIA 'GND' 1-4 (1.05 2) places a via that belongs to the signal GND and reaches from layer 1 to 4 at position (1.05 2).

ROUTE Command

If you want to change the layer while laying-out the board, EAGLE always takes the shortest possible via (CHANGE LAYER). It is also possible that a via at the same position is elongated automatically.
If micro vias are enabled in the Design Rules, EAGLE sets a micro via when routing from an SMD and immediately changing to the next inner layer.

Autorouter

The Autorouter supports blind and buried vias. If you decide to use the Autorouter for a multilayer board that uses blind and buried vias it is not allowed to work with automatically generated supply layers (see page 122). In this case inner layers can be defined with the help of polygons. Already existing supply layers can be transformed into layers with supply polygons by renaming the layer (no $ sign at the beginning of the name), removing possibly existing isolation wires, drawing a polygon covering the whole layout, and naming the polygon with the favored signal name.

cfBase.xx: 0.20

Base costs for one step on the corresponding layer. Recommendation: outside layers (Top, Bottom) always 0, inside layers greater than 0.
The Autorouter cfVia: 0.99
Controls the use of vias. A low value produces many vias but also allows the preferred direction to be followed. A high value tries to avoid vias and thus violates the preferred direction. Recommendation: low value for the routing pass, high value for the optimization.

cfNonPref: 0.10

Controls following of the preferred direction. A low value allows tracks to be routed against the preferred direction, while a high value forces them into the preferred direction. If cfNonPref is set to 99, track sections can only be placed in the preferred direction. Only select this value if you are certain that this behavior is really wanted.

cfChangeDir: 0.25

Controls how often the direction is changed. A low value means many bends are allowed within a track. A high value produces virtually straight tracks.

cfOrthStep, cfDiagStep

Implements the rule that the hypotenuse of a right-angled triangle is shorter than the sum of the other two sides. The default values are 2 and 3. That means that the costs for the route using the two other sides are 2+2, as against 3 for the hypotenuse. This parameter should only be altered with great care!

cfExtdStep: 0.30

Controls the avoidance of track sections which run at an angle of 45 degrees to the preferred direction, and which would divide the board into two sections. A low value means that such sections are allowed while a high value tries to avoid them. In combination with the parameter mnExtdStep you can control the length of these tracks. If mnExtdStep = 0, each grid step at 45 degrees to the preferred direction causes costs that are defined in parameter cfExtdStep. Choosing for example mnExtdStep = 5 allows a track to run five steps at 45 degrees without any additional costs. Each further step causes costs defined in cfExtdStep. In this way, 90 degree bends can be given 45 degree corners. Settings like cfExtdStep = 99 and mnExtdStep = 0 should avoid tracks with 45 degree

Drawing the Pin-Leaded Package
The component is manufactured in a pin-leaded package. This is a DIL-14 housing with a pin spacing of 2.54 mm (0.1 inch) and a width of 7.62 mm (0.3 inch). If there is a suitable package in another library, it can be copied into the current library. A new definition would not be necessary.
DIL-14 data sheet Click on the Edit a package icon in the action toolbar, and enter the name of the package in the New box of the Edit menu, which is DIL-14 in our present example. Click on OK, and confirm the question Create new package DIL-14? by answering Yes. The Package Editor window now opens.
First set the appropriate grid (50 mil in this case) using the GRID command, and let the grid lines be visible. The grid can easily be shown and hidden with the F6 function key.

Place Pads

Use the PAD command, and place the solder pads in accordance with the specifications on the data sheet. The pads should be arranged in such a way that the coordinate origin is located somewhere near the center of the package. Each pad can have individual properties such as Shape, Diameter, and Drill hole diameter. Available shapes are: Square, Round, Octagon, Long, and Offset (Long with offset drill). Select the desired pad shape and specify the hole diameter. The pad diameter usually is defined with the standard value auto (respectively 0), since the size is finally determined in the layout by means of the Design Rules, Restring tab. The pad appears in the library with the default value of 55 mil. You may, however, assign an individual value. If, for instance, you specify 70 mil, the consequence is that the diameter of the pad on the board cannot be less than 70 mil (independent of the calculated value of the Design Rules). You select this value when the PAD command is active (i.e. the pad is attached to the mouse cursor) using the parameter toolbar. It is also possible to specify the drill hole diameter and the pad shape.
The parameter toolbar when the PAD command is active The properties of pads that have already been placed can be altered at a later stage by means of the CHANGE command. Click on the CHANGE icon and select the property and the appropriate value. Then click on the pads whose properties are to be altered. CHANGE can also be applied to groups (using the GROUP command). After the property has been selected, click inside the group with the right mouse button. As soon as a pad has been placed, EAGLE automatically generates solder stop symbols in layers 29 and 30, t/bStop. The dimensions of the solder stop symbols is specified in the Design Rules, Mask tab, Stop parameter. Pads can be marked with special flags (First, Stop, Thermals). They can be altered with CHANGE subsequently. Giving one pad of a package the First flag (CHANGE FIRST ON) allows to define a special shape for it in the Design Rules, Shapes tab, option First, in order to mark it as the number '1' pad of the package.

Then click on Description in the description box. You can insert a detailed description of this package form here. The Rich Text format can be used. This format is described in the programs help system under Rich Text.
The entry of the LCC-20 in Rich Text format could look like this: <b>LCC-20</b> <p> FK ceramic chip carrier package from Texas Instruments. The ADD dialog in the Layout Editor can search for this description or for keywords within it.
Please do not forget to save the library from time to time!
The fully defined LCC-20 Supposed you found a package that is exactly the one you need, simply copy it into your current library. More information about this on page 205.
Component Design Explained through Examples Defining the Logic Symbol for the Schematic Diagram
Our device contains four OR gates, each having two inputs and one output. We first create an OR symbol.
Logical appearance of the 541032. Click on the Edit a symbol icon. Enter a name for the symbol on the New line, such as 2-input_positive_or, and click OK. Confirm the question Create new symbol 2-input_positive_or? by answering Yes. You now have the Symbol Editor window in front of you.

Check the Grid

Check that the grid is set to the default value of 0.1 inch. Please try to use only this grid, at least when placing the pins. It is essential that pins and net lines are located on the same grid. Otherwise there will not be any electrical connection between the net and the pin!
Select the PIN command, and place 3 pins. The pin properties can be changed by means of the parameter toolbar as long as the pin is attached to the mouse cursor and has not been placed. If a pin has already been placed, its properties can be altered at a later stage with the CHANGE command. A number of pins can be handled at the same time with the GROUP and CHANGE commands followed by a click with the right mouse button. The parameters Orientation, Function, Length, Visible, Direction and Swaplevel have been thoroughly described when the example of the resistor symbol was examined (see p. 162). The coordinate origin should be somewhere near the center of the symbol, and, if possible, not directly under a pin connection point. This makes it easy to select in the schematic diagram.

Pin Name

You assign pin names with the NAME command. In our symbol the two input pins are named A and B, and the output pin is named Y.

Draw the Symbol

Use the WIRE command to draw the symbol in layer 94, Symbols. The standard line thickness for the Symbol Editor is 10 mil. You may also choose any other line thickness.
Placeholders for NAME and VALUE

Example: GRID MM ; MARK (0 0); PAD '2' LONG R120 (P 50 120) ;
8.12 Library and Part Management
Copying of Library Elements

Within a Library

If you want to use a symbol or a package which already exists in a related manner for a device definition you can copy it within the library with the commands GROUP CUT, and PASTE. Afterwards it can be , modified as requested. The following sections explain every single step with the help of an example package taken from linear.lbr.

Open Library

Use the menu File/Open/Library in the Control Panel to open the library linear.lbr or select the entry Open from its context menu of the tree view's expanded Libraries branch.

Edit Existing Element

Open the Edit window with Library/Package and select the package DIL08. After clicking OK it is shown in the Package Editor window. Use DISPLAY to show all layers. Draw a frame around all objects to be copied with GROUP. Now click the CUT icon followed by a left mouse click into the group. Alternatively you may enter a reference point in the command line for CUT, as for example: CUT (0 0) ;

Define New Element

Click the Edit-a-package icon in the action toolbar. Enter the name DIL08-TEST in the New field of the Edit window and confirm with OK. Click the PASTE icon followed by a click at the drawing's reference point. The package will be placed. Or use again the command line: PASTE (0 0) ;
Now it can be modified as requested. The given coordinates for CUT and PASTE can be used to move a group by a certain value in the coordinates system. This may be valuable for elements that have been drawn in the wrong grid. This procedure can be applied to symbols too! Devices can't be copied within a library!
From One Library into Another

Devices

If there is a proper device or Device set that you want to use in your current library you can copy it in two different ways. In the Control Panel: Move (with Drag&Drop) the requested Device set from the Control Panel's tree view into the opened Library Editor window. The complete Device set with symbol(s) and package(s) will be copied and newly defined. As an alternative you could use the entry Copy to Library in the context menu of the device entry. With the COPY command: Type, for example, COPY 75130@751xx.lbr or with the whole path COPY 75130@d:\eagle-4.1\lbr\751xx.lbr in the command line, the Device 75130 from library 751xx.lbr is copied into the currently opened library. If the path contains spaces use single quotes for it, for example: COPY '75130@d:\P A T H\751xx.lbr' If the Device should be stored in the current library under a new name simply enter it, like here: COPY 75130@751xx.lbr 75130NEW

which the user has renamed to $GND in accordance with EAGLEs naming convention for supply layers. The filenames are suggestions. You are, of course, free to use unequivocal names of your own definition. The options given in the list are recommendations, which in some cases can be changed.

demo.cmp

Active layers

Top Via Pad Via Pad $GND

Comments/recommended options
Component side. Options: pos. coord., optimize, fill pads. Multilayer inner layer. Options: pos. coord., optimize, fill pads. Multilayer supply layer. Is automatically output inverse. Options: pos. coord., optimize. Solder side. Options: pos. coord., optimize, fill pads. Component side silkscreen. Options: pos. coord., optimize. Solder side silkscreen. Only needed if there are components on the underside Options: pos. coord., optimize. Component side solder mask. Options: pos. coord., optimize. Solder side solder mask. Options: pos. coord., optimize. Component side cream frame. Options: pos. coord., optimize. Solder side cream frame. Only required if there are SMD components on the bottom side Options: pos. coord., optimize. Drilling data for NC drilling machines. Options: (rotate), pos. coord., optimize. Drill data for multilayer boards for distinction of via lengths of blind and buried vias. Optiones: (rotate), pos. coord., optimize.

demo.ly2 demo.ly3

demo.sol
Bottom Vias Pads tPlace Dimension tName bPlace Dimension bName tStop bStop tCream bCream

demo.plc

demo.pls
demo.stc demo.sts demo.crc demo.crs

demo.drd demo.drd.xxxx

Drills Holes Drills Holes
Preparing the Manufacturing Data Additional Information for the Board Manufacturer
You must also supply the service company with the configuration files for apertures (name.whl) and drills (name.drl). You can also include the board file name.brd. This can help to avoid problems with what can become time-consuming questions. In general, alignment marks (which are for example defined in layer 49, Reference) or an information field (in, for example, layer 48, Documentation) can be included. A text file, such as demo.txt, should contain instructions for the board manufacturer.
9.3 Rules that Save Time and Money

Each layer should without fail be uniquely identified (e.g. CS for Component Side). For cost reasons you should, if at all possible, avoid track that narrows to below 8 mil. Only angles should be drawn at the corners to delimit the board. Closed borders can lead to manufacturing difficulties. You should always leave at least 2 mm (about 80 mil) around the edge of the board free of copper. In the case of supply layers on multilayer boards, which are plotted inverse, you do this by drawing a wire around the edge of the board. As already mentioned, text in copper layers ought to be written in vector font. So you can really be sure that the text on your board looks the same as it does in the Layout Editor window. For the sake of completeness we want to point out here again that all questions concerning layer setup, layer thickness, and drill diameter for multilayer boards with blind, buried, or micro vias have to be pre-examined.
9.4 Generating the Data with Ready-Made CAM Jobs
The CAM Processor provides a job mechanism with the aid of which the creation of the output data for a board can be automated. The Control Panel's tree view (CAM Jobs branch) lists all jobs and shows a brief description.
EAGLE Manual Gerber.cam Job for Two-Layer Boards
The gerber.cam job uses the GERBERAUTO and GERBER drivers. These generate files in the RS-274D format. It is set up for two-layer boards which are to receive a solder stop mask on the component and on the soldering side, and is to receive a silkscreen print. Load the job by double-clicking on the gerber.cam entry in the tree view of the Control Panel. In the first step an aperture table name.whl is automatically generated. Two messages appear, which you confirm with OK.
Gerber job messages The first message is generated by the entry in the Prompt field, and reminds you to delete the temporary files created when generating the aperture table when the job is done. The second message advises you that more than one signal layer is active at the same time. Normally only one signal layer is active while output is generated. However, when generating the wheel, all the layers need to be active at the same time in order to form a common aperture table for all Gerber output. Data for the following layers is subsequently output:
name.cmp name.sol name.plc name.stc name.sts component side solder side Silkscreen Solder stop mask, component side Solder stop mask, solder side
If other layers are also to be generated, e.g. silkscreen for the bottom side, or a solder cream mask, the Gerber job can be extended as required. Extending the job is discussed later in this section.