EAGLE EASILY APPLICABLE GRAPHICAL LAYOUT EDITOR Manual Version 4.
This software and documentation are copyrighted by CadSoft Computer, Inc., doing business under the tradename 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 CadSoft Computer, Inc. All trademarks referenced in this document are the property of their respective owners.
EAGLE LICENSE AGREEMENT This is a legal agreement between you, the end user, and CadSoft Computer, Inc., which markets software products under the trademark EAGLE. CadSoft Computer, Inc. shall be referred to in this Agreement as CadSoft. If you do not agree to the terms of this Agreement, promptly return the diskette package and accompanying items (including written materials and containers) to the place you obtained them for a full refund.
LIMITED WARRANTY CadSoft warrants the accompanying Software and documentation to be free of defects in materials and workmanship for a period of ninety (90) days from the purchase date. The entire and exclusive liability and remedy for breach of this Limited Warranty shall be, at Cadsoft’s option, either (a) return of the price paid or (b) replacement of defective Software and/or documentation provided the Software and/or documentation is returned to CadSoft with a copy of your receipt.
Table of contents 1 Introduction 1.1 What is in This Manual? 1.2 Technical Terms 2 Installation 2.1 What You Have Received 2.2 New Installations Windows Linux 2.3 Updating an Older Version 2.4 Changing or Extending the License 2.5 Multiple Users and Network Licenses Installing in a Network 3 EAGLE Modules and Editions 3.1 EAGLE Modules The Layout Editor, the Basic Module Schematic Module Autorouter 3.2 Different Editions Professional Edition Standard Edition Light Edition 4 A First Look at EAGLE 4.
4.5 The CAM Processor Dialog Generate Data 4.6 The Text Editor Window 5 Principles for Working with EAGLE 5.1 Command Input Alternatives Command Line History Function Function Keys Script Files Mixed Input 5.2 The EAGLE Command Language Typographical Conventions Entering Coordinates as Text 5.3 Grids and the Current Unit 5.4 Names and Automatic Naming Length Forbidden Characters Automatic Naming 5.5 Import and Export of Data Script Files and Data Import File Export Using the EXPORT Command 5.
Specify the Board Outline Arrange Devices Boards with Components on Both Sides Exchanging Housing Forms Changing the Technology Define Forbidden Areas Routing - Placing Tracks Manually Defining a Copper Plane with POLYGON Checking the Layout and Correcting Errors Creating Manufacturing Data 6.4 Multilayer Boards Signal Layers Power Supply Layer with One Signal Ground Areas and Supply Layers with More than One Signal 6.5 Updating Components (Library Update) 6.
mnVia 0..30 mnSegments 0..9999 mnExtdSteps 0..9999 7.6 Number of Ripup/Retry Attempts 7.7 The Autorouter Menu 7.8 Routing Multi-Layer Boards Supply Layers Polygons as Supply Layers 7.9 Backup and Interruption of Routing 7.10 Information for the User Status Display Log file 7.11 Parameters of a Control File 7.12 Practical Tips General Single-Sided Boards SMD Boards With Supply Layers What can be done if not all signals are routed? 8 Component Design Explained through Examples 8.
Gerber Format Drill Data Data for Milling Machines Data for Component Insertion Machines 9.2 Which Files does the Board Maker Need? Files Generated with the CAM Processor Additional Information for the Board Manufacturer 9.3 Rules that Save Time and Money 9.4 Generating the Data with Ready-Made CAM Jobs Gerber.cam Job for Two-Layer Boards Job rs274x.cam Drill Data 9.5 Set Output Parameters 9.6 Names of the Output Files 9.7 Automating the Output with CAM Processor Jobs Defining a Job Extending gerber.
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.
EAGLE Manual Appendix Lists useful additional information and explains some error messages EAGLE prompts in certain situations. For a quick, hands-on introduction, refer to the EAGLE Tutorial. Please read the tutorial for a better understanding before working with the manual. Anybody who has already been working with a prior version of EAGLE is advised to read the file UPDATE under Linux or UPDATE.TXT under Windows. It contains a description of all the differences from earlier versions.
Introduction 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. 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.
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 installation or for an extension of your license. In all cases, however, there is a new License Certificate and a new license disk.
EAGLE Manual 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 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.
Installation 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!). Usage 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.
EAGLE Manual license.key file (on the license disc) and for the installation code. Enter both of these and click OK. The program has now been re-licensed. You can call up the license data at any time in the EAGLE Control Panel by means of the Help/Product Information menu. 2.5 Multiple Users and Network Licenses Multiple-user licenses may be installed separately on different computers, or may be used in a network within the scope of the license conditions.
Installation Special Instructions Under Windows Path Information It has been found to be helpful to use the server names in UNC notation when giving the path for calling EAGLE, rather than the drive letters. For example: \\netservername\eagle\bin\eagle.exe Different Operating Systems at the Working Computers If network computers having different Windows systems are in use, it is first necessary to perform an installation as described above.
Chapter 3 EAGLE Modules and Editions 3.1 EAGLE Modules A number of EAGLE editions are offered. You can add an Autorouter Module and/or a Schematic diagram Module to the Layout Editor. The term module is used because EAGLE always behaves like one single program. The user interface is identical for all parts of the program.
EAGLE Manual Autorouter You can route the airwires automatically if you own the Autorouter module. You can choose single nets, groups of nets or all nets for the automatic routing pass (AUTO command). The program will handle various network classes having different track widths and minimum clearances. 3.2 Different Editions EAGLE offers various performance/price categories (editions) called Light, Standard, and Professional. The facilities mentioned in this manual always refer to the Professional edition.
EAGLE Modules and Editions • copper pouring • support of different package variants Schematic Module • • • • • up to 99 sheets per schematic online Forward&Back Annotation between schematic and board automatic board generation automatic generation of supply signals (for IC’s) Electrical Rule Check (checks logic in the schematic and the consistency of schematic and layout) Autorouter Module • • • • • • • • • • fully integrated into basic program uses the set of Design Rules you defined for the layout cha
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.
EAGLE Manual The Control Panel: On the right, the description of a TTL library Library Summary The possibility of displaying the contents of the libraries is particularly interesting. It provides a very rapid overview of the available devices. Double-click on the Libraries entry. The library branch opens, and you can see the available libraries. In the Description field you can see a brief description of the contents.
A First Look at EAGLE 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.
EAGLE Manual 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 on 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 First Look at EAGLE Context menu for project management 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. 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, library, CAM job, ULP, script or text file.
EAGLE Manual 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 any other text editor. Open Opens an existing file of the types mentioned above. Save all All changed files are saved. The current settings for the project are saved in the file eagle.epf. Refresh Tree The contents of the tree view are updated. Exit The program is terminated.
A First Look at EAGLE The directories dialog in the Options menu Type the path directly into the corresponding box, or select the desired directory by clicking on the Browse button. 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 wit the SET command.
EAGLE Manual All these backup files can be further processed in EAGLE if they are renamed and given the usual file endings (brd, sch, lbr). Backup dialog 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. 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.
A First Look at EAGLE 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.
EAGLE Manual Product Registration The registration dialog is called automatically when you start EAGLE the first time. If you want to install an upgrade you must start this dialog from the Help menu, and then enter the necessary information according to the License/Product Registration section of the help function. Read the notes in the chapter on Installation for more information.
A First Look at EAGLE 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 you can double-click on a schematic diagram file in the tree view. If you want to create a new schematic diagram, select the menu File/New/Schematic.
EAGLE Manual 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. Below, in the status line, instructions for the user appear if a command is active.
A First Look at EAGLE 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.
EAGLE Manual 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. 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).
A First Look at EAGLE 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. COPY Copy objects. MIRROR Mirror objects. ROTATE Rotate objects (also possible with MOVE). GROUP Define a group which can then be moved, rotated, or copied (with CUT and PASTE) to another drawing.
EAGLE Manual ADD Add library elements to the schematic. A search function helps devices to be found quickly. USE specifies which libraries are available. NAME Give names to components, nets, or buses. VALUE Provide values for components. Integrated circuits normally get the type (e.g. 74LS00N) as their value. SMASH Separate name and value texts from a device, so that they can be placed individually. The size of smashed texts can also be individually changed.
A First Look at EAGLE CIRCLE Draw a circle. Circles with a width of 0 are drawn as filled circles. ARC Draw an arc. RECT Draw a rectangle. POLYGON Draw a polygon. BUS Draw a bus line. The meaning of a bus is more conceptual than physical. It is only a means to make a schematic easier to read. Only nets define an electrical connection. Nets, however, can be dragged out of a bus. NET Draw a net. Nets with the same name are connected (even if located on different sheets).
EAGLE Manual Commands Not Available in the Command Toolbar Menu items already explained in the Control Panel section are not discussed here. The following commands can be entered into the command line. Some of them are available as menu items. ASSIGN Assign function keys. The most convenient way of doing this is to use the Options/Assign menu. CLASS Select and define net classes (Edit/Net classes...).
A First Look at EAGLE OPEN Text command for opening a library for editing (Library/Open). This command is not identical to the File/Open menu item of the Schematic Editor, which only lets you select schematics. You can use the OPEN command as an alternative to the File menu of the Control Panel. PRINT 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.
EAGLE Manual USE Select libraries that will be referred to by the ADD dialog. Click the USE icon in the Layout Editor's or Schematic Editor's action toolbar or select the menu item Library/Use to start this command. This selection can also be done by clicking on the library markers (green for selected, gray for deselected) in the Libraries branch of the Control Panel's tree view.
A First Look at EAGLE 4.3 The Layout Editor Window The Layout Editor window opens when you open an existing board file or create a new board. If you own the Schematic Editor you will normally draw a schematic first and then generate the board file with the BOARD command, or by clicking the Switch to board icon. The Layout Editor window appears very much like the Schematic Editor window.
EAGLE Manual The Commands on the Layout Command Toolbar INFO Provides information about the object to be selected. SHOW Highlights the object to be selected. DISPLAY Select and deselect the layers to be displayed. Components on the top side of the board can only be selected if the layer 23, tOrigins, is displayed. The same applies to components on the bottom side of the board and layer 24, bOrigins. See Appendix for the meaning of the layers.
A First Look at EAGLE GROUP Define a group which can then be moved, rotated, or copied (with CUT and PASTE) to another drawing. After the icon has been clicked, a rectangular group can be defined by holding down the left mouse button and dragging the cursor to the diagonal corner of the rectangle. If you want to define a group by a polygon, use the left mouse button to determine the corners of the polygon. Then click the right mouse button to close the polygon.
EAGLE Manual SMASH Separates name and value texts from a component, so that they can be placed individually. The size of smashed texts can also be changed individually. PINSWAP Swap two signals connected to equivalent pads of a component, provided the pins have been defined with the same swaplevel. REPLACE Replace a package with another package from any library. This is permitted as long as you are working in a layout that is not connected to a consistent schematic by Forward&Back Annotation.
A First Look at EAGLE CIRCLE Draw a circle. This command creates restricted areas for the Autorouter if used in the layers 41, tRestrict, 42, bRestrict, or 43, vRestrict. ARC Draw an arc. RECT Draw a rectangle. This command creates restricted areas for the Autorouter if used in the layers 41, tRestrict, 42, bRestrict, or 43, vRestrict. POLYGON Draw a polygon. Polygons in the signal layers are treated as signals.
EAGLE Manual DRC Define Design Rules and perform Design Rule Check. ERRORS Show errors found by the DRC and clear error polygons. 4.4 The Library Editor Window The Library Editor window opens when you load a library for creating or editing components. A library normally has three different elements: packages, symbols and devices. • A package is a device’s housing, as will be used in the Layout Editor (on the board). • The symbol contains the way in which the device will be shown in the schematic.
A First Look at EAGLE Library Editor window: No element has yet been loaded Load or Rename Package, Symbol, or Device The following commands are important for navigating within a library: EDIT Load device or package (if you only have the Layout Editor) for editing. From the left: Load device, load package, load symbol. These icons are shown in the action toolbar. REMOVE Delete device/package/symbol from library. Available only through the Library menu or the command line. See help.
EAGLE Manual The Package Editing mode The definition of a device is described briefly below. There is a more extensive guide in the Component Design Explained through Examples section. The icons available in the command toolbar are equivalent to the identical icons of the Schematic or Layout Editor. Design New Package You change into package editing mode through the Edit a package icon in the action toolbar.
A First Look at EAGLE Design a New Package from an Existing One Load the existing package, display all layers, define a group (GROUP command) containing all of the objects, click the CUT icon and then the origin of the drawing area (coordinates 0 0). You can also type the CUT command on the command line and give a reference point, for example: CUT (0 0) ; Open a new package (in the same or another library) for editing, click the PASTE icon and then the origin of the drawing area.
EAGLE Manual You can adjust the pin parameters (name, direction, function, length, visible, swaplevel) while the PIN command is active, or with the CHANGE command. The pin parameters are explained starting on page 142 and in the help pages under the keyword PIN. Pin names are changed using the NAME command.
A First Look at EAGLE • how the gate behaves when added to a schematic (addlevel), • the prefix for the component name, if a prefix is used, • if the value of the component can be changed or if the value should be fixed to the device name, • which pins relate to the pads of the package (CONNECT command) • whether a description for this component should be stored in the library.
EAGLE Manual The addlevel defines, for instance, if a gate is to be added to the schematic only on the users request. Example: the power gate of an integrated circuit which is normally not shown on the schematic. NAME Change gate name. CHANGE Change swaplevel or addlevel. PACKAGE Define and name package variant(s). The PACKAGE command is started by clicking on the New button in the Device Editor window, or by typing on the command line. CONNECT Define which pins (gate) relate to which pads (package).
A First Look at EAGLE DESCRIPTION Compose a description of the device which can also be examined by the search function associated with the ADD dialog. 4.5 The CAM Processor Dialog Manufacturing data is generated by means of the CAM Processor. A number of drivers for the data output are available. The drivers are defined in the file eagle.def , which can be edited with any text editor. Output to matrix printers, however, is not created with the CAM Processor but with a PRINT command.
EAGLE Manual Generate Data Load Job File A job defines the sequence of several output steps. You can, for example, use a job to generate individual files containing the Gerber data for several pcb layers. A job is loaded with the File menu of the CAM Processor or via the Control Panel. A job is not absolutely essential for output. All the settings can be made manually. Load Board Before you can generate an output you must open the File menu and load a board.
A First Look at EAGLE 4.6 The Text Editor Window EAGLE contains a simple text editor. You can use it to edit script files, User Language programs or any other text file. When in the text editor, the right mouse button calls up a context menu. The menus bring you to a variety of functions such as commands for printing, copying and cutting, searching, replacing and so on.
Chapter 5 Principles for Working with EAGLE 5.1 Command Input Alternatives As an alternative to the mouse, the EAGLE Schematic, Layout, and Library Editors allow you enter all commands: • on a command line by typing text commands, • via function keys, • via script files. • via User Language programs. In any case it is necessary to understand the syntax of the EAGLE command language which is described in the following section. The commands are described in detail on the help pages.
EAGLE Manual HOLE 0.15 (5 8.5) ; Place a hole with drill diameter 0.15 at position 5 8.5. VIA 'GND' 0.070 round (2.0 3.0) ; A round shaped via with a diameter of 0.070 belonging to signal GND will be placed at position 2.0 3.0. History Function You can recall the most recently entered commands by pressing CrsrUp (↑) or Crsr-Down (↓) and edit them. The Esc key deletes the contents of the command line.
Principles for Working with EAGLE The dialog for the ASSIGN command To predefine certain assignments you can also use the ASSIGN command in the file eagle.scr (see page 78). Examples: The combination of Ctrl + Shift + G displays a grid of 0.127mm: ASSIGN CS+G 'GRID MM 0.
EAGLE Manual Mixed Input The various methods of giving commands can be mixed together. You can, for instance, click the icon for the CIRCLE command (which corresponds to typing CIRCLE on the command line), and then type the coordinates of the center of the circle and of a point on the circumference in this form (2 2) (2 3) ← on the command line. The values used above would, if the unit is currently set to inch, result in a circle with a radius of one inch centered on the coordinate (2 2).
Principles for Working with EAGLE Bold Type or Upper Case Commands and parameters shown here in UPPER CASE are entered directly. When they are entered, there is no distinction made between upper and lower case. For example: Syntax: GRID LINES Input: GRID LINES grid lines Lower Case Parameters shown here in lower case are to be replaced by names, numbers or keywords. For example: Syntax: GRID grid_size grid_multiple Input: GRID 1 10 This sets the grid to 1 mm (assuming that the current unit is set to mm).
EAGLE Manual Input: SET BEEP ON or SET BEEP OFF The beep, which is triggered by certain actions, is switched on or off. Repetition Points The .. characters mean either that the function can be executed multiple times, or that multiple parameters of the same type are allowed. For example: Syntax: DISPLAY option layer_name.. Input: DISPLAY TOP PINS VIAS The layer number can alternatively be used: DISPLAY 1 17 18 More than one layer is made visible here.
Principles for Working with EAGLE Entering Coordinates as Text The program sees every mouse click as a pair of coordinates. If it is desired to enter commands in text form on the command line, then instead of clicking with the mouse it is possible to enter the coordinates through the keyboard in the following form: (x y) where x and y are numbers representing units as selected by the GRID command. The textual input method is necessary in particular for script files.
EAGLE Manual You draw a rectangular forbidden area in layer 41 tRestrict: LAYER TRESTRICT; RECT (0.5 0.5) (2.5 4) ; 5.3 Grids and the Current Unit EAGLE performs its internal calculations using a basic grid size of 1/10 000 mm (0.1 micron). Any multiple of that can be set as the working grid. Microns, mils, inches and mm can be used for the unit. The current unit as set with the GRID command applies to all values. You should always use the pre-set 0.1 inch grid for schematic diagrams.
Principles for Working with EAGLE Style specifies the way it is displayed: Lines or Dots. The two options On and Off under Display switch the grid display on or off. Finest sets the finest grid that is possible. Clicking on default will select the editor's standard grid. The last button returns to whatever grid was previously set. 5.4 Names and Automatic Naming Length Names in EAGLE can have any desired length. There is no limit. Forbidden Characters No names may contain spaces or umlauts.
EAGLE Manual ADD NAND 'A' ¬ • • • • fetches four NAND gates with the names A, B, C and D. If the generated name reaches Z, then names with the default prefix will again be generated (e.g. G$1). 5.5 Import and Export of Data EAGLE provides a number of tools for data exchange. • Script files for importing • The export command for exporting • EAGLE User Language programs for import and export. The User Language is very flexible, but does call for a suitable program to be created.
Principles for Working with EAGLE Comments can be included following a #-character. The execution of a script file can be stopped by clicking the Stop icon. File Export Using the EXPORT Command The EXPORT command has the following modes: DIRECTORY Outputs a list of the contents (devices, symbols, and packages) of the currently loaded library. NETLIST Outputs a netlist for the currently loaded schematic or board in an EAGLE-specific format. It can be used to check the connections in a drawing.
EAGLE Manual IMAGE The option Image allows you to generate files in various graphic formats. The following formats are available: bmp Windows Bitmap file png Portable Network Graphics file pbm Portable Bitmap file pgm Portable Grayscale Bitmap file ppm Portable Pixelmap file xbm X Bitmap file xpm X Pixmap file Settings for graphic file output Click the Browse button, select the output path, and type in the graphic file name with its extension.
Principles for Working with EAGLE 5.6 The EAGLE User Language EAGLE contains an interpreter for a C-like User Language. It can be used to access any EAGLE file. Since version 4 it has also been able to access external data. It is possible, with very few restrictions, to export data from EAGLE, import a wide range of data into EAGLE, or to manipulate data within EAGLE. ULPs can, for example, manipulate a layout file or a library directly.
EAGLE Manual 5.7 Forward&Back Annotation A schematic file and the associated board file are logically linked by automatic Forward&Back Annotation. This ensures that the schematic and the board are always consistent As soon as a layout is created with the BOARD command (or by means of the Switch to board icon), the two files are consistent. Every action performed on the schematic diagram is simultaneously executed in the layout.
Principles for Working with EAGLE 5.8 Configuring EAGLE Individually There are a number of settings that permit the program to be adjusted for individual needs. We distinguish between program, user and project-specific settings. Basic program settings that will apply to every user and every new project are made in the eagle.scr file. Under Windows, personal preferences are stored in the file eaglerc.usr, or, under Linux, in ~/.eaglerc.
EAGLE Manual Settings in Options/Set/Misc The above window is reached through the Options/Set menu in an editor window, or by entering SET on the command line. 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. The eagle.scr File The script file eagle.
Principles for Working with EAGLE The DEV, SYM and PAC labels indicate those segments within the file which are only to be executed if the device, symbol or package editor mode is activated. Commands which are defined before the first label (normally BRD:) are valid for all Editor windows. If, because of the specifications in a project file, EAGLE opens one or more editor windows when it starts, it is necessary to close these and to reopen them so that the settings in eagle.scr are adopted.
EAGLE Manual SYM: Display all; Grid Default On; Change Width 0.010; #Menu Arc Change Copy Cut Delete Display Export \ # Grid Group Move Name Paste Pin Quit Script \ # Show Split Text Value Window ';' Wire Write Edit; PAC: Grid Default On; Change Width 0.005; Change Size 0.050; Change Smd 0.039 0.
Principles for Working with EAGLE EAGLE Project File If a new project is created (by clicking the right mouse button on an entry in the Projects branch of the tree view and then selecting New/Project in the context menu in the Control Panel), a directory is first created which has the name of the project. An eagle.epf configuration file is automatically created in every project directory.
Chapter 6 From Schematic to Finished Board This chapter illustrates the usual route from drawing the schematic diagram to the manually routed layout. Particular features of the schematic diagram or Layout Editor will be explained at various points. Use of the Autorouter and the output of manufacturing data will be described in subsequent chapters. We recommend to create a project (folder) first. Details about this can be found on page 28. 6.
EAGLE Manual Open the Schematic Diagram You first start from the Control Panel. From here you open a new or existing schematic diagram, for instance by means of the File/Open or the File/New menus, or with a double click on a schematic diagram file in the directory tree. The schematic diagram editor appears. Create more schematic sheets if needed. For that purpose, open the combo box in the action toolbar with a mouse click, and select the New item. A new sheet will be generated (see page 37).
From Schematic to Finished Board return to the schematic diagram editor. The frame is now hanging from the mouse, and it can be put down. The bottom left hand corner of the frame is usually at the coordinate origin (0 0). Library names, device names and terms from the device description can be used as search keys. Wildcards such as * or ? are allowed. A number of search keys, separated by spaces, can be used.
EAGLE Manual If you have placed a device with ADD, and then want to return to the ADD dialog in order to choose a new device, press the Esc key or click the ADD icon again. Give the devices names and values (NAME, VALUE). If the text for the name or the value is located awkwardly, separate them from the device with SMASH, and then move them to whatever position you prefer with MOVE. Clicking with DELETE on either of the texts makes it invisible.
From Schematic to Finished Board Devices with Several Gates Some devices consist not of one but of several gates. These can normally be placed onto the schematic diagram one after another with the ADD command. To place a certain gate you can use the gate name directly. Example: The device 74*00 from the 74xx-eu library consists of for NAND gates named A to D and one power gate named P. If you want to place the gate C first, use the gate name with the ADD command: ADD 'IC1' 'C' 74LS00@74xx-eu.
EAGLE Manual The JUNCTION command is used to mark connections on nets that cross one another. Junctions are placed by default. This option, (Auto set junction), can also be deactivated through the Options/Set/Misc menu. Nets must be drawn with the NET command, not with the WIRE command. Do not copy net lines with the COPY command. If you do this, the new net lines won’t get new net names. This could result in unwanted connections.
From Schematic to Finished Board The index of a partial bus name may run from 0 to 511. The help system provides you with more information about the BUS command. Specifying Net Classes The CLASS command specifies a net class. The net class specifies the minimum track width, the minimum clearance from other signals and the hole diameter for vias in the layout for a specific class of signals. The default setting is net class 0, which means that none of these things are specified.
EAGLE Manual Swaplevel: Pins layer is visible Input pins 1 and 2 have swaplevel 1, so they can be exchanged with one another. The output pin, 3, which has swaplevel 0, cannot be exchanged. You can find the swaplevel of a gate by means of the INFO command. Power Supply Pins defined as having the direction Pwr are automatically wired up. This is true, even if the associated power gate has not explicitly been fetched into the schematic. The name of the Pwr pin determines the name of the voltage line.
From Schematic to Finished Board If a supply pin (with pin direction Sup) is placed on a net (with ADD, MOVE) then this net segment will receive the name of the supply pin. If the last supply pin on a net is deleted, it is given a new, automatically generated name. Check and Correct Schematic A schematic diagram must be checked with the aid of the Electrical Rule Check (ERC), when the design of the schematic diagram has been completed, if not before.
EAGLE Manual Open Pins when MOVEing If an element is moved then its open pins will be connected to any nets or other pins which may be present at its new location. Use UNDO if this has happened unintentionally. 6.2 Considerations Prior to Creating a Board Checking the Component Libraries The EAGLE component libraries are developed by practicing engineers, and correspond closely to present-day standards.
From Schematic to Finished Board You will find more details on this in the section on the Preparing of Manufacturing Data (Chapter 9). Specifying the Design Rules All the parameters relevant to the board and its manufacture are specified in the Design Rules. Use the menu Edit/Design Rules.. to open the Design Rules window. The layout can be checked at any time with the aid of the Design Rule Check (DRC). The DRC command makes a wide range of parameters available.
EAGLE Manual The Apply button stores the values that are currently set in the layout file. This means that the values that have so far been chosen are not lost if you do not immediately start the error check and if you want to leave the DRC dialog via the Cancel button. Changes to various Design Rules are immediately displayed in the Layout Editor after clicking on Apply. The Design Rules can be saved in a special Design Rules file (*.dru) by the use of the Save as.. button.
From Schematic to Finished Board Minimum Clearances Clearance refers to the minimum distances between tracks, pads, SMDs and vias of different signals, and between SMDs, pads and vias of the same signal. Setting the values for Same signal checks to 0, disables the respective check. Distance allows settings to be made for the minimum distances between objects in layer 20, Dimension, in which the board outline is usually drawn, and between holes.
EAGLE Manual Design Rules: Restring setting The diagram illustrates the template for setting the width of the residual ring. The standard value for the restring around holes is 25% of the hole diameter. Since the width of the ring on small holes specified this way would soon fall below a technically feasible value, a minimum value (10 mil in this case) is specified here. It is also possible to specify a maximum value. Example: The ring around a hole with 40 mil diameter is 10 mil (25%).
From Schematic to Finished Board Shapes A rounding factor can be specified here for SMD pads. The value can be between 0% (no rounding) and 100% (maximum rounding). Roundness: 0 - 10 - 25 - 50 - 100 [%]. Right: 100%, square A square SMD has been placed instead of an oblong one on the far right of the diagram. After assigning the property Roundness = 100%, the SMD becomes round. This is where the form of the pads is specified. It is possible to give different settings for the top and bottom layers.
EAGLE Manual The Isolate values for Thermal and Annulus determine the width of the thermal bridge or ring. The Restring option determines whether the insulation bridge of the thermal symbol should be drawn immediately at the edge of the hole or at a distance from the hole given by the restring value (Restring tab, Inner setting). If the Restring option for Annulus is deactivated, a filled circle is generated instead of the annulus ring. This is the default setting.
From Schematic to Finished Board Design Rules: Settings for Solder Stop and Cream Frame The default value for solder stop is 4 mil, i.e. minimum value is maximum value is 4 mil. The percent value has no effect in this case. The value for the cream frame is set to 0, which means that it has the same dimensions as the smd. If the values are given in percent, in the case of smds and pads of the form XLongOct or YLongOct the smaller dimension is the significant one.
EAGLE Manual Check angle ensures that all tracks are laid at whole multiples of 45 degrees. This test is normally switched off, but can be activated if required. Check font (de-)selects the font check. The DRC checks if texts are written in vector font. Text which is nonvector font is marked as an error. This check is necessary due to the fact that the CAM Processor can't work with others than vector font for the generation of manufacturing data.
From Schematic to Finished Board 6.3 Create Board After you have created the schematic, click the Switch to board icon. An empty board is generated, next to which the components are placed, joined together with airwires. Supply pins are connected by those signals which correspond to their name, unless another net is explicitly joined to them. The board is linked to the schematic by the Forward&Back Annotation.
EAGLE Manual Board command: Create the layout from the schematic The devices are automatically placed at the left of the board. The board outline is drawn as a simple line in layer 20, Dimension. The outline of an eurocard is displayed in the Professional and Standard editions, a half-eurocard in the Light edition. If you wish, you may alter the size or shape of the empty board with the MOVE and SPLIT commands. You can also delete the outline and add a frame out of a library (such as 19inch.lbr) with ADD.
From Schematic to Finished Board If, for example, you type MOVE R14 onto the command line, the device named R14 will be attached to the mouse cursor, and can be placed. Precise positioning results from input such as: MOVE R14 (0.25 2.50) R14’s locating point is now located at these coordinates. A group of devices can be transposed by combining the GROUP and MOVE commands.
EAGLE Manual Boards with Components on Both Sides If the board is also going to have components on the underside, the MIRROR command is used. It causes devices on the underside to be inverted. SMD pads, the silk screen and the layers for the solder stop and solder cream masks are automatically given the correct treatment here. It is not necessary for the Package Editor to define devices in the library as being on the bottom side.
From Schematic to Finished Board If you want to change a package which you gave a new value with the help of the VALUE command before, the value text of the new package will drop to the original value although the device has been defined with VALUE Off in the library. See also page 56. REPLACE command If you have a layout without an associated schematic diagram, you exchange the package with the aid of the REPLACE command.
EAGLE Manual Routing - Placing Tracks Manually The ROUTE command allows the airwires to be converted into tracks. A click on the center mouse button while a track is being laid allows a change of layer. A via is placed automatically. Clicking with the right mouse button changes the way in which the track is attached to the mouse and how it is laid (SET command, Wire_Bend parameter).
From Schematic to Finished Board Defining a Copper Plane with POLYGON EAGLE can fill regions of a board with copper. Simply draw the borders of the area with the POLYGON command. You give the polygon a signal name, using NAME followed by a click on the border of the polygon. Then all the elements that carry this signal are connected to the polygon. Both pads and, optionally, vias (as specified in the Design Rules) are joined to the copper plane through thermal symbols.
EAGLE Manual Isolate: Defines the value that the polygon must maintain with respect to all other elements not part of its signal. If higher values are defined for special elements in the Design Rules or net classes, the higher values apply. 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.
From Schematic to Finished Board 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.
EAGLE Manual Design Rules (Distance tab). Setting the value Copper/Dimension to 0 deactivates this check. In this case polygons do not keep a minimum distance to objects in layer 20, Dimension, and holes! The DRC will not check if holes are placed on tracks! Drill Distance: Distance violation between holes. Defined by the value Drill/Hole in the Design Rules (Distance tab). Drill Size: Drill diameter violation in pads, vias, and holes. This value is defined in the Design Rules (Minimum Drill, Sizes tab).
From Schematic to Finished Board Width: Minimum width violation of a copper object. Defined by Minimum Width in the Design Rules (Sizes tab) or, if defined, by the track parameter Width of a referring net class. Also texts in signal layers will be checked. Wire Style: The wire style of a wire which is connected to a signal is not Continuous. Net, device and pin lists can be output by means of EXPORT or by various User Language programs.
EAGLE Manual 6.4 Multilayer Boards You can develop multilayer boards with EAGLE. To do this, you use one or more inner layers (Route2 to Route15) as well as the layers Top and Bottom for the top and undersides. You display these layers when routing. Signal Layers You use the ROUTE command as before to place tracks in those inner layers which are provided for signals. Eagle will itself ensure that the tracks are connected by way of plated-through holes to the appropriate signals in the outer layers.
From Schematic to Finished Board LAYER 2 $GND This specifies that layer number 2 (previously known as Route2) is henceforth known as $GND, and that it will be treated as a power supply layer The preferred direction for the Autorouter is to be set to N/A for power supply layers. This will cause the Autorouter not to use this layer. Pads are connected to power supply layers with what are known as thermal symbols, or are isolated with annulus symbols.
EAGLE Manual (with the exception of polygons with rank = 0, drawn as a part of a package in the Package Editor). Rank = 6 signifies the lowest priority. Polygons with the same rank are compared by the DRC. Please read the notes regarding polygons in the section on Defining a Copper Plane on page 105. Please note that this does not apply to supply layers defined by $name... Supply layers made with polygons are not plotted inversely.
From Schematic to Finished Board modifications to the library in two steps (e.g. first the pin names and then the pin positions), or the library element can be given a new name, so that it is not exchanged. If Forward&Back Annotation is active, the components are replaced in the schematic diagram and in the layout at the same time. You will find further information on the program's help pages.
EAGLE Manual The currently selected printer is shown at the top of the window. The selected printer can be altered by means of the Printer... button. Style permits a number of output options to be selected: Mirror inverts the drawing from left to right, Rotate turns it 90 degrees, and Upside down turns it through 180 degrees. If both are activated, a rotation of 270 degrees is the result. If the Black option is chosen, a black-and-white printout is made.
From Schematic to Finished Board Calibrate allows correction factors for the x and y directions to be entered. This allows linear errors in the dimensional accuracy of the print to be corrected. The Caption option switches the appearance of the title, printing date, filename and the scale of the print on or off. If, when a layout is printed, the drill holes in the pads and vias are not to be visible, select the No Drills option for the Display mode by way of the menu item Options/Set/Misc.
Chapter 7 The Autorouter 7.1 Basic Features • • • • • • • • • • • • Any routing grid (min. 0.02 mm) Any placement grid (min. 0.
EAGLE Manual Autorouters whatsoever. However, in practice, the required amount of time is not always available, and therefore certain boards will not be completed even by a 100 % Autorouter. The EAGLE Autorouter is based on the ripup/retry algorithm. As soon as it cannot route a track, it removes prerouted tracks (ripup) and tries it again (retry). The number of tracks it may remove is called ripup depth which is decisive for the speed and the routing result.
The Autorouter Busses, as understood by the Autorouter, are connections which can be laid as straight lines in the x or y direction with only a few deviations. Busses are only routed if there is a layer with an appropriate preferred direction. Routing Pass The actual routing pass is then started, using parameters which make a 100 % routing as likely as possible. A large number of vias are deliberately allowed to avoid paths becoming blocked.
EAGLE Manual 7.4 What Has to be Defined Before Autorouting Design Rules The Design Rules need to be specified in accordance with the complexity of the board and of the manufacturing facilities available. You will find a description of the procedure and of the meanings of the individual parameters in the section on Specifying the Design Rules on page 89.
The Autorouter Routing Grid The Autorouter grid has to be set in the AUTO command setup menu (Routing Grid). This is not the same as the currently used grid in the Layout Editor window that you have selected with the GRID command. Bear in mind that for the routing grid the time demand increases exponentially with the resolution. Therefore select as large a grid as possible. The main question for most boards is how many tracks are to be placed between the pins of an IC.
EAGLE Manual When choosing the grid, please also ensure that each pad covers at least one grid point. Otherwise it can happen that the Autorouter is unable to route a signal, even though there is enough space to route it. In this case the Autorouter issues the message Unreachable SMD at x y as it starts. The parameters x and y specify the position of the SMD pad. The default value for the routing grid is 50 mil. This value is sufficient for simple through-hole layouts.
The Autorouter Inner layers are converted to supply layers if they are renamed to $name, where name is a valid signal name. These layers are not routed. Supply layers with more than one signal can be implemented with polygons. These layers are treated as normal signal layers. In the case of boards that are so complex that it is not certain whether they can be wired on two sides, it is helpful to define them as multilayer boards, and to set very high costs for the inner layers.
EAGLE Manual An area drawn in layer 20 can also be used as a restricted region for all signals. It should, however, be noted that this area should be deleted before sending the board for manufacture, since layer 20 is usually output during the generation of manufacturing data. Cost Factors and Other Control Parameters The default values for the cost factors are chosen on the basis of our experience in such a way as to give the best results. The control parameters such as mnRipupLevel, mnRipupSteps etc.
The Autorouter 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.
EAGLE Manual cfBonusStep, cfMalusStep: 1..3 Strengthens the differentiation between preferred (bonus) and bad (malus) areas in the layout. With high values, the router differentiates strongly between good and bad areas. When low values are used, the influence of this factor is reduced. See also cfPadImpact, cfSmdImpact. cfPadImpact, cfSmdImpact: 0..10 Pads and SMDs produce good and bad sections or areas around them in which the Autorouter likes (or does not like) to place tracks.
The Autorouter mnVia 0..30 Controls the maximum number of vias that can be used in creating a connecting track. mnSegments 0..9999 Determines the maximum number of wire pieces in one connecting track. mnExtdSteps 0..9999 Specifies the number of steps that are allowed at 45 degrees to the preferred direction without incurring the value of cfExtdStep. See also cfExtdStep. 7.
EAGLE Manual If one of these values is exceeded, the router interrupts the ripup process and reestablishes the status which was valid at the first track which could not be routed. This track is considered as unroutable, and the router continues with the next track. 7.7 The Autorouter Menu When running the Autorouter with the AUTO command, the setup menu appears first. All the necessary settings are made there.
The Autorouter Autorouter setup: Settings for the Route pass The parameters in the Layer costs, Costs and Maximum groups can be different for each pass. The Active check box specifies whether this step should be executed or not. Additional optimization passes can be inserted with the Add button. Clicking on the Select button allows certain signals to be selected for autorouting. Select these with a mouse click, or enter their names on the command line.
EAGLE Manual Autorouter setup: Restarting an interrupted job Do not at first make any changes to the parameters if you want to restart an interrupted routing job. Use the Continue existing job check box to decide whether you want to continue with an existing job, or whether you want to choose new settings for the remaining signals. End job ends the autorouting job and loads the previous routing result. 7.8 Routing Multi-Layer Boards There are two different ways of implementing supply layers.
The Autorouter Polygons as Supply Layers It is possible with polygons to create supply layers that contain more than one supply voltage, and a few individual wires as well. Please note the instructions on page 110, Ground Planes and Supply Layers with Several Signals. These are not the kind of supply layer identified by a $ in the name, but are in fact ordinary layers. • Define the polygons before running the Autorouter. • Give the appropriate signal names to the polygons.
EAGLE Manual 7.10 Information for the User Status Display During the routing, the Autorouter displays information on the actual routing result in the status bar. The displayed values have the following meaning: Route: Vias: Conn.: Ripup: Signals: result % (hitherto maximum, best data Number of vias Connections total/found/not routable No. of ripups/cur. RipupLevel/cur. RipupTotal Signals found/signals handled/signals prepared Connections means 2-point connections.
The Autorouter Router memory : Passname: 1121760 Busses Route Time per pass: 00.00.21 00.08.44 Number of Ripups: 0 32 max. Level: 0 1 max. Total: 0 31 16 0 6.7 % Routed: Vias: Resolution: Final: 238 338 100.0 % Optimize1 Optimize2 Optimize3 Optimize4 00.06.32 0 0 0 00.06.15 0 0 0 00.06.01 0 0 0 00.05.55 0 0 0 238 178 100.0 % 238 140 100.0 % 238 134 100.0 % 238 128 100.0 % 100.0% finished 7.
EAGLE Manual 7.12 Practical Tips This section presents you with some tips that have, over a period of time, been found useful when working with the Autorouter. Look on these examples as signposts suggesting ways in which a board can be routed. None of these suggestions guarantee success. General The layer costs (cfLayer) should increase from the outer to the inner layers or be the same for all layers. It is unfavorable to use lower values in the inner layers than in the outer layers.
The Autorouter Now switch off the bus router and all the optimization passes in the Autorouter setup. Only the routing remains active. Alter the following cost factors: cfVia = 0 Vias are wanted mnVia = 1 Max. 1 via per connection cfBase.1/16 = 30..99 Short tracks in Top/Bottom mnSegments = 2..8 short tracks Start the Autorouter, using the Select button, and choose the signals to be routed. After the routing pass it is possible, if appropriate, to optimize the result manually.
Chapter 8 Component Design Explained through Examples When developing circuits with EAGLE, components are fetched from libraries and placed into the schematic or, if the Schematic Editor is not being used, into the layout. All the component information is then saved in the schematic or board file. The libraries are no longer needed for continued work with the data. So when you want to pass your schematic to a third party to have a layout made from it, you do not also have to supply the libraries.
EAGLE Manual Would you like to change the name of an element in your library? Then use the RENAME command. You can type it in the command line. For example: RENAME DIL16 DIL-16; The package receives the new name DIL-16. 8.1 Definition of a Simple Resistor First open a new library in the EAGLE Control Panel using the File/New/Library menu. Alternatively you can type the command OPEN on the command line of the Schematic or Layout Editor windows. Then enter a library name in the file dialog.
Component Design Explained through Examples You should not draw any objects in layer 17, Pads, or 18, Vias! They will not be recognized, nor by the DRC, neither by polygons drawn in the layout, and can lead to short circuits! For a SMD resistor, select SMD, and set the pad dimensions in the parameter toolbar. You can either select one of the offered values, or directly type the length and breadth into the entry field.
EAGLE Manual Layer 51, tDocu, is not used to print onto the board itself, but is a supplement to the graphical presentation which might be used for printed documentation. Care must be taken in layer 21, tPlace, not to cover any areas that are to be soldered. A more realistic appearance can be given, however, in the tDocu layer, which is not subject to this limitation.
Component Design Explained through Examples Restricted area for components In layer 39, tKeepout, you should create a restricted area over the whole component (RECT command). This allows the DRC to check whether components on your board are too close or even overlapping. Description Finally, you click on the Description box. Text can then be entered in the lower part of the window which then opens. Rich Text format can be used.
EAGLE Manual Set the Grid Now check that 0.1 inch is set as the grid size. The pins in the symbol must be placed on this grid, since this is what EAGLE expects. Place the Pins Select the PIN command. You can now set the properties of these pins in the parameter toolbar, before placing them with the left mouse button. All these properties can be changed at a later stage with the CHANGE command. Groups can again be defined (GROUP) whose properties can then be altered with CHANGE and the right mouse button.
Component Design Explained through Examples The SHOW command can be used to check whether a net is connected to a pin in the schematic diagram. The pin line and the net are displayed more brightly if they are connected. If a pin with length 0 is used, or if it was drawn as a line with the WIRE command, it cannot be displayed brightly. Visible The next four icons in the parameter toolbar specify whether the pins are to be labeled with pin names, pad names, both or neither.
EAGLE Manual The Pwr and Sup directions are used for the automatic connection of supply voltages (see page 171). Swaplevel The swaplevel is a number between 0 and 255. The number 0 means that the pin cannot be exchanged for another pin in the same gate. Any number bigger than 0 means that pins can be exchanged for other pins which have the same swaplevel and are defined within the same symbol. The pins can be swapped in the schematic or in the board with the PINSWAP command.
Component Design Explained through Examples Pin Names The NAME command allows you to name pins after they have been placed. The automatic name allocation, as described on page 69 also operates. Schematic Symbol The schematic symbol is drawn in the symbols layer using WIRE and the other drawing commands. Place the texts >NAME and >VALUE in layers 95, Names, and 96, Values (TEXT command). Place them where the name and value of the component are to appear in the schematic.
EAGLE Manual You can change the name of the gate or gates with the NAME command. The name is unimportant for a device with only one gate, since it does not appear in the schematic. Keep the automatically generated name! In the case of devices with several gates, the name of the particular gate is added to the name of the device. Example: The gates are called A, B, C and D, and the name of the component in the schematic is IC1, so the names which appear are IC1A, IC1B, IC1C and IC1D.
Component Design Explained through Examples The resistor gate in this example is automatically identified as G$1, for which reason the pins G$1.1 and G$1.2 of this gate appear in the Pin column. The two connections of the housing are listed in the Pad column. Mark a pin and the associated pad, and click on Connect. If you want to undo a connection that you have made, mark it in the Connection column and click Disconnect. Clicking on a column’s header bar changes the sorting sequence.
EAGLE Manual The Device Editor: Fully defined resistor Save This completes definition of the resistor, and it can be fetched into the schematic diagram. If you have not already saved the library, please do it at this stage! Use The newly created library has to be made available for the schematic or layout with the help of the USE command. This command has to be used in the Schematic or Layout Editor. It is also possible to mark a library as in Use in the Control Panel's tree view. See help for details.
Component Design Explained through Examples 8.2 Defining a Complex Device In this section we use the example of a TTL chip (541032) to define a library element that is to be used in two different packages (pin-leaded and SMD). It is a quad OR gate. The schematic diagram symbol is to be defined in such a way that the individual OR gates can be placed one after another. The power supply pins are not initially visible in the schematic diagram, but can be fetched into the diagram if needed.
EAGLE Manual Data sheet for the 541032 All the data for this component has been extracted from a data book published by Texas Instruments, whom we thank for permission to reproduce it.
Component Design Explained through Examples Creating a New Library Click on the File/New/Library menu in the EAGLE Control Panel. The Library Editor window appears, containing a new library, untitled.lbr. It is, of course, also possible to expand an existing library. In that case you would use File/Open/Library to select the library you want, or you would click on the Libraries entry in the Control Panel’s tree view, selecting the desired library with a click of the right mouse button.
EAGLE Manual Set the Grid 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.
Component Design Explained through Examples The following procedure is recommended for components that have a large number of sequentially numbered pads: Select the PAD command, type in the name of the first pad, e.g. '1', and place the pads in sequence. The single quote marks must be typed on the command line. See also the section on Names and Automatic Naming on page 69. Draw the Silk Screen Symbol A simple silk screen symbol that is to be visible on the board is drawn in layer 21, tPlace.
EAGLE Manual The descriptive text for our DIL-14 might look like this: DIL-14
14-Pin Dual Inline Plastic Package, Standard Width 300 mil It is also possible to add, for instance, the reference data book, the e-mail address of the source or other information here. The search facility in the Layout Editor’s ADD dialog also looks in this text for keywords. Package Editor with DIL-14 Save At this stage if not before the library should be saved under its own name (e.g. my_lib.lbr).
Component Design Explained through Examples SMD package, FK version. Click again on the Edit a package icon, and enter the name of the package in the New box in the edit menu. The package is to be called LCC-20. Click on OK and confirm the question Create new package ‘LCC-20’? by answering Yes. Set the Grid Adjust the grid to 0.635 mm (0.025 inch), and let the grid lines be visible.
EAGLE Manual Click therefore in the SMD icon, and type 0.8 2 ← on the command line. Create two vertical rows as well. The SMDs can be rotated in 90 degree increments with the right mouse button. Placing the SMDs The Roundness parameter (CHANGE command) specifies whether curves should be given to the corners of the solder pads. The default value is 0%, which means that there is no rounding. See also the section on page 95.
Component Design Explained through Examples onto the command line, then click on the SMD. Drag it with MOVE so that it is located at the correct position. The INFO command is helpful for checking the position and properties of the solder pads. When a SMD is placed (in the Top layer), symbols for solder stop and solder cream are automatically created in layer 29, tStop, and layer 31, tCream, respectively.
EAGLE Manual Package Name and Package Value The labeling now follows. Use the TEXT command and write >NAME in layer 25, tNames, for the name placeholder, and >VALUE in layer 27, tValues, as the placeholder for the value, and place this at a suitable location. The texts can be separated and relocated at a later stage using SMASH and MOVE. Area Forbidden to Components In layer 39, tKeepout, you should create a forbidden area over the whole component (RECT command).
Component Design Explained through Examples The fully defined LCC-20 By the way: Supposed you found a package (or of course a symbol) that is exactly the one you need, simply copy it into your current library. This can be done by the commands GROUP, CUT, and PASTE. See also page 53.
EAGLE Manual 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.
Component Design Explained through Examples 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 and ARC commands 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.
EAGLE Manual Defining a Power Supply Symbol Two pins are needed for the supply voltage. These are kept in a separate symbol, since they will not initially be visible in the schematic diagram. Click on the Edit a symbol icon. Enter a name for the symbol on the new line, such as VCC-GND, and click OK. Confirm the question Create new symbol ‘VCC-GND’? with Yes. Check the Grid First check that the grid is set to the default value of 0.1 inch.
Component Design Explained through Examples The supply symbol Associating the Packages and Symbols to Form a Device Set We now come to the final step, the definition of the device set. A device set is an association of symbols and package variants to form real components A device set consists of several devices, which use the same symbols for the schematic but different technologies or package variants.
EAGLE Manual Click on the Edit a device icon. Enter the name for the device on the new line. In our example this is a 541032A. This device is to be used in two different technologies, as the 54AS1032A and as the 54ALS1032A. A * is used as a placeholder at a suitable location in the device name to represent the different technologies. Enter, therefore, the name 54*1032A, and confirm the question Create new device ‘54*1032A’? with Yes. The device editor window opens.
Component Design Explained through Examples The swaplevel determines whether a device’s gates can be swapped within the schematic diagram. The value that is currently set is − like the addlevel − displayed above left in layer 93, Pins, for each gate. The default value is 0, meaning that the gates may not be exchanged. The swaplevel can have a value from 0 to 255. Gates with the same swaplevel can be exchanged with one another. Our device consists of four identical gates that may be swapped.
EAGLE Manual The pin assignment for the packages Select the J version from the package list and click on the CONNECT button. The connect window opens. CONNECT dialog The list of pins is on the left, and the pads are in the center. Click on a pin-entry, and select the associated pad. Both entries are now marked. You join them with the connect button. This pair now appears on the right, in the Connection column. Join each pin to its pad in accordance with the data sheet.
Component Design Explained through Examples There is now a green tick to the right of both package variants, and this indicates that connection is complete. This is only true when every pin is connected to a pad.
EAGLE Manual Specifying the Prefix The prefix of the device name is defined simply by clicking on the Prefix button. IC is to be entered in this example. Value The setting of value determines whether the VALUE command can be used to alter the value of the device in the schematic diagram and in the layout. The default setting is off, so that alteration is not permitted. Since that appears to be appropriate here too, value is left off. The value of the device corresponds to the device name in this case.
Component Design Explained through Examples Device-Editor: 54*1032A.dev 8.3 Supply Voltages Component Power Supply Pins The components’ supply pins are to be given the direction Pwr in the symbol definition. The pin name determines the name of the supply signal. Pins whose direction is Pwr and which have the same name are automatically wired together (even when no net line is shown explicitly).
EAGLE Manual NAND symbol 7400 (European representation) The two input pins are called I0 and I1 and are defined as having direction In, swaplevel 1, visible Pin and function None. The output pin is called O and is defined with direction Out, swaplevel 0, visible Pin, and function Dot. Now define the supply gate with the name PWRN, and the following properties: Power gate The two pins are called GND and VCC. They are defined with direction Pwr, swaplevel 0, function None, and visible Pad.
Component Design Explained through Examples The addlevel of Next means that as these gates are placed into the schematic, they will be used in that sequence, i.e., the sequence in which they were fetched into the device. Then place the PWRN symbol once, using addlevel Request and swaplevel 0. Name this gate P. Addlevel Request specifies two things: • The supply gate will only be fetched into the schematic if requested, i.e. with the INVOKE command. The ADD command will only be able to place NAND gates.
EAGLE Manual Supply symbol for GND As has been explained above, the device receives the name of the pin that is used in the symbol. The corresponding device is defined with addlevel Next. If you set value to off you can be sure that the labeling is not accidentally changed. On the other hand, you have more flexibility with value set to on. You can alter the label if, for instance, you have a second ground potential. You must, however, then create explicit nets for the second ground.
Component Design Explained through Examples 8.5 Labeling of Schematic Symbols The two text variables >NAME and >VALUE are available for labeling packages and schematic symbols. Their use has already been illustrated. There are two further methods that can be used in the schematic: >PART and >GATE. The following diagram illustrates their use, in contrast to >NAME. The symbol definition on the left, the appearance in the schematic diagram on the right.
EAGLE Manual 8.6 Pins with the Same Names If you want to define components having several pins of the same name, then proceed as follows. Let us suppose that three pins are all to be called GND. During the symbol definition the pins are given the names GND@1, GND@2 and GND@3. Only the characters in front of the “@” are visible in the schematic, and the pins are treated there as if they were all called GND. However these pins are not necessarily internally connected. 8.
Component Design Explained through Examples Relay: Coil and First Contact must be Placed A relay with three contacts is to be designed, of which typically only the first contact will be used. Define the coil and one contact as their own symbols. In the device, give the coil and the first contact the addlevel Must. All the other contacts are given the addlevel Can.
EAGLE Manual Package of a circuit board connector Now define a symbol representing one contact area. Set visible to Pad, so that the names 1 to 10, defined in the package, appear in the schematic. Connector symbol for the schematic diagram Then fetch the symbol ten times into a newly created device, setting the addlevel in each case to Always, and use the CONNECT command to create the connections between the SMDs and the pins.
Component Design Explained through Examples Connector with Fixing Hole and Forbidden Area A connector is to be defined having fixing holes. On the solder side (bottom), the Autorouter must avoid bringing tracks closer to the holes than a certain distance. Fixing holes with restricted areas The drill holes are placed, with the desired diameter, on the package using the HOLE command. The drilling diameter can be retrospectively changed with CHANGE DRILL.
EAGLE Manual Text variables in the documentation field The text variables >DRAWING_NAME, >LAST_DATE_TIME and >SHEET are contained, as well as some fixed text. The drawing’s file name, date and time of the last change appear at these points together with the sheet number in the schematic (e.g., 2/3 = sheet 2 of 3). In addition, the variable >PLOT_DATE_TIME is available. It contains the date and time of the last printout.
Chapter 9 Preparing the Manufacturing Data There are pcb firms who need only the EAGLE board file in order to manufacture films or prototypes. You will find links to such firms on our Internet pages. If however your board maker is not set up to process EAGLE board files directly, you will have to supply him with a set of files. You generate these with the aid of the CAM Processor.
EAGLE Manual RS-274D, or subsets of it, is the commonest format, which can be generated with the CAM Processor. Therefore choose the devices GERBER and GERBERAUTO. In this case a file with the associated aperture table must be supplied, in addition to the files with the plot data. All the further explanations in this section are based on this format. Drill Data The generation of drill data is very similar to the generation of photoplot data.
Preparing the Manufacturing Data The ULP executes the following steps: • Drawing a polygon with the name _OUTLINES_ in the selected layer over the whole board area • Setting the properties of the polygon: Rank = 6 Width = diameter of milling tool • Computing the polygon; the filling defines what has to be milled out • Generating output data • Deleting the polygon in the layout Further information can be found in the help function, Outline data.
EAGLE Manual File Active layers Comments/recommended options demo.cmp Top Via Pad Component side. Options: pos. coord., optimize, fill pads. demo.ly2 Via Pad Multilayer inner layer. Options: pos. coord., optimize, fill pads. demo.ly3 $GND Multilayer supply layer. Is automatically output inverse. Options: pos. coord., optimize. demo.sol Bottom Vias Pads Solder side. Options: pos. coord., optimize, fill pads. demo.plc tPlace Dimension tName Component side silkscreen. Options: pos. coord.
Preparing the Manufacturing Data 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.
EAGLE Manual 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.
Preparing the Manufacturing Data • Check the parameters and change them to fit your needs (e.g. choose a different device driver like SM1000 or SM3000). A tolerance of 6 2.5% makes sense to avoid problems due to internal unit conversions. Only the layers 44, Drills, and 45, Holes, may be selected. No other layers! You can display the selected layers by clicking Layer/Show selected. • Save the file via File/Save job if you made any changes. • Execute the job (Process Job). • Send the files name.drl and name.
EAGLE Manual 9.5 Set Output Parameters This section describes the setting of the parameters for the output of a drawing or a file, which will then be started with the button Process job or Process section. The parameters for a section, as described below, are set in the same way. Load the schematic or board file from the CAM Processor’s File/Open menu, and set the following parameters: • Select the driver for the desired output device in the Device combo-box. • Enter the output data in the File field.
Preparing the Manufacturing Data Fill Pads: Pads will be filled. This option is on for generating manufacturing data. Devices of the generic type (see eagle.def), for example PostScript, allow to deactivate this option. The drill holes for pads will be visible on the output. • Select sheet (for schematics only): Use the Sheet combo box as far as the schematic consists of more than one page. 9.
EAGLE Manual CAM Processor: Solder side section of the gerber.cam job. The diagram shows the ending .whl in the Wheel line for the aperture table. This means that the file democmp.whl is looked for. The output (File) receives the name democmp.sol. The flag options Optimize and Pos. coords. are active. A tolerance of 6 1% is permitted for the aperture selection. This is necessary in order to compensate for small rounding errors (of around 0.
Preparing the Manufacturing Data 9.7 Automating the Output with CAM Processor Jobs Defining a Job A job consists of one or more sections. A section is a group of settings, as described above in the Set Output Parameters chapter, which defines the output of one file. In this way you can use a job to generate all the files that are necessary for a project. You define a job as follows: • Start the CAM Processor. No job is loaded at first, unless there is a file called eagle.cam in the cam directory.
EAGLE Manual Extending gerber.cam Job for Multilayer Boards The gerber.cam job can be used as the basis of the job for multilayer boards. It must simply be extended for the additional layers. Example: You want to output the files for a board with SMD components on the top and bottom sides, a supply layer $GND in Layer2, and another inner layer with a polygon VCC in Layer 15 (which is renamed to VCC).
Preparing the Manufacturing Data Check once more whether all the necessary layers for the creation of the aperture table are active in the first section. The output file generated in the first section cannot be used. For this reason, the file name.$$$ should be deleted. Layers that refer to the bottom side of your layout will be generated mirrored in all predefined job files. If your board house recommends non-mirrored files, please deactivate this flag option for each section.
EAGLE Manual Info File The apertures which have not been found are then listed in the file name.gpi, where name here stands for the name chosen for the output file. You can then change your board in such a way that the existing apertures can be used. After generating plot or drill files you should always check the related info files.
Preparing the Manufacturing Data The following apertures are available: Name Dimension Draw diameter Round diameter Square length Octagon diameter Rectangle length-X x width-Y Oval diameter-X x diameter-Y Annulus outside diameter x inside diam. Thermal outside diameter x inside diam.
EAGLE Manual 9.9 Device Driver in File eagle.def Creating Your Own Device Driver Output device drivers are defined in the eagle.def text file. Here you will find all the information that is needed for the creation of your own device driver. The best way is to copy the block for an output device of the same general category, and then alter the parameters where necessary. Please use a text editor that does not introduce any control codes into the file.
Preparing the Manufacturing Data Units in the Aperture Configuration File When automatically generated with the GERBERAUTO driver, the aperture table (wheel file) contains values in inches. If your pcb manufacturer insists on mm units, you can achieve this by altering the GERBER or GERBERAUTO drivers. In order to do this, use a text editor (one that does not introduce any control codes) to edit the eagle.def file.
EAGLE Manual 9.11 Documentation Many documentation items can be generated with the aid of User Language programs. You can find a description of a ULP in the User Language programs branch of the tree view in the Control Panel, or at the start of a ULP file itself. In that case, examine the ULP with a text editor. Note also the wide range of programs that are made available on our web server. Parts List The parts list can be created by a number of User Language programs.
Preparing the Manufacturing Data Drill Plan A drill plan can be printed which enables you to check the drill holes and their diameters. It shows an individual symbol for each diameter. EAGLE uses 19 different symbols: 18 of them are assigned a certain diameter; one (Ø) appears if no symbol has been defined for the diameter of this hole. The diameter symbols appear in layer 44, Drills, at the positions where pads or vias are placed, and in layer 45, Holes, at the positions where holes are placed.
EAGLE Manual Assignment of the drill symbols 198
Appendix A.
EAGLE Manual 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 51 52 tGlue bGlue tTest bTest tKeepout bKeepout tRestrict bRestrict vRestrict Drills Holes Milling Measures Document Reference tDocu bDocu Glue mask, top side Glue mask, bottom side Test and adjustment information, top side Test and adjustment inf., bottom side Restricted areas for components, top side Restricted areas for components, bottom s.
Appendix B. EAGLE Files EAGLE uses the following file types: Name Type of file *.brd *.sch *.lbr Layout Schematic Library *.ulp *.scr *.txt *.dru User Language Program Script file Text file (also other suffixes) Design Rules *.ctl *.pro *.job *.b$$ *.cam *.erc Control parameter for the Autorouter Autorouter protocol file Autorouter job Backup file of brd after finishing the Autorouter CAM Processor job Error file from electrical rule check *.b#x *.s#x *.l#x *.b## *.s## *.
EAGLE Manual C. EAGLE Options at a Glance In order to output manufacturing data, for instance, with the CAM Processor, EAGLE can be started directly from a terminal window under Linux or from a console window under Windows. Since Windows programs give up their connection to the console they have been started from, you can use the file eaglecon.exe (located in the demo/bin subdirectory on the CD-ROM) if you want to run the CAM Processor from a batch file.
Appendix -e+ -e- ditto Aperture Emulation off Flag options (e.g. -e) can be used without repeating the ‘-’ character: -eatm Aperture emulation on, annulus and thermal emulation on, mirror output -ea-t+ Aperture emulation on, NO annulus emulation, thermal emulation on Defining tolerance values: If there is no sign, the value applies to either direction, + signifies a positive tolerance, - a negative tolerance. -D0.10 -D+0.1 -D-0.
EAGLE Manual -W Aperture Wheel File: This option defines the path to the wheel file which should be used -X Calls command line version of the CAM Processor -a Annulus Symbol Emulation: Default: off -c Positive Coordinates: If this option is set the CAM Processor creates data without negative coordinates. The drawing is moved to the zero-coordinates. This option can be turned off with the option -c-.
Appendix -q Quick Plot: Generates a draft or fast output, which only prints the frames of the objects. Default: off -r Rotate Output: Rotates the output by 90 degrees. Default: off -s Scale Factor: Those devices which cannot change their scale-factor (in the menu of the CAM Processor), have a scale factor of 1. Default: 1 -t Emulate Thermals: Works only in combination with -e+. Default: off -u Rotate Output by 180 degrees: In combination with -r+ one can rotate by 270 degrees.
EAGLE Manual D. Configuration of the Text Menu With the help of a script file (e.g. menu.scr) you can configure your own text menu. # Command Menu Setup # # This is an example that shows how to set up a complex # command menu, including submenus and command aliases. MENU ‘Grid {\ Metric {\ Fine : Grid mm 0.1; |\ Coarse : Grid mm 1;\ } | \ Imperial {\ Fine : Grid inch 0.001; |\ Coarse : Grid inch 0.
Appendix E. Text Variables Text variable Meaning >NAME >VALUE >PART >GATE >SHEET Component name (eventually + gate name) 1) Component value/type 1) Component name 2) Gate name 2) Sheet number of a circuit diagram 3) >DRAWING_NAME Drawing name >LAST_DATE_TIME Time of the last modification >PLOT_DATE_TIME Time of the plot creation 1) Only for package and symbol 2) Only for symbol 3) Only for symbol or circuit diagram F. Error Messages When Loading a File Library objects with the same names.
EAGLE Manual Pad Replaced with a Hole In older versions of EAGLE it was possible to define pads in which the hole diameter was larger than the pad diameter. This is no longer permitted. If you attempt to load a library file that was created with an earlier version and that contains such a pad, the following message appears: The pad or via is automatically converted into a hole, provided it is not connected by CONNECT to a pin in one of the library's devices.
Appendix Can't update files prior to version 2.60 If this message appears when loading an EAGLE file that was made with a version earlier than 2.60 it is necessary first to convert the file. The program update26.exe, which is located in the eagle/bin directory, is used for this purpose. Copy the file that is to be converted into the directory containing both update26.exe and the file layers.new. Then open a DOS window under Windows, and change into this directory. Type the command: update26 dateiname.
EAGLE Manual In a Library Package/Symbol is in use If a package or symbol is used in a device, no pads or pins may be deleted or added. Therfore the following messages appear after the PAD or PIN command have been selected: It is allowed to CHANGE pins or pads. To change the number of pins/pads you have to delete the corresponding device(s) first (REMOVE command).
Index A Action toolbar 35,37 Add Components 40 ADD 40,47,55 Addlevel 174 Airwire 12 Alt-X 30 Always 174 Annulus aperture 191,192 Annulus symbol 12,95 Aperture Configuration 182,192,195 Draw 192 Emulation 192 Fixed wheel file 191 Flash 192 Forms 193 Shapes 193 Tolerance 192,195 Units 195 ARC 41,49 ASSIGN 42,62,75 AUTO 49 Automatic naming 69 Autorouter 117 Backup 131 Control file 133 Cost Factors 124 Design Rules 120 Features 117 Grid 120,121 Interrupting 131 Layer 122 Load parameters 128 Log file 132 Memory
Drill plan 197 Flag options 186,189 Gerber output 191 Job 189 Messages 183 Output file name 187 Photoplot output 191 Start from a Batch 202 Can 174 Caption 115 CHANGE 39,47,56,75,141 Change font 40 Change package 102 Checking Layout 106 Schematic 89 CIRCLE 41,49 CLASS 42,87 Clearance 93 Clk 142 CLOSE 42 Command language 64 Command line 36,61 Command parameters 37 Command toolbar 36 Commands ADD 40 ARC 41 CHANGE 39 CIRCLE 41 COPY 39 CUT 39 DELETE 39 DESCRIPTION 57 DISPLAY 38 DRC 50 ERRORS 50 EXPORT 71 GATESW
Cursor appearance CUT D Default Default directories Default settings Delete From library Sheet DELETE Design Rule Check Design rules Desktop publishing Device driver Device set Diameter of lands Dimensions of pads Directories Directory Default DISPLAY Distance Documentation Documentation print Dot DotClk Drag&Drop Drawing Frames Name DRC Errors Drill Configuration Data Diameter Hole diameters Info file Plan Rack file Tolerance DRILLCFG.
Function keys G >GATE Gate GATESWAP Generate data GERB274X.CAM Gerber Fixed aperture wheel Information file GERBER GERBER.
Must N >NAME NAME NC Neighboring objects Selecting Net Connection point NET Net Classes Net script Netlist Network License Next None O Object properties Pre-setting OC OPEN Optimization OPTIMIZE Options CAM processor Options menu Orientation Out Output See Also Export as CAM job Device Drawings Drivers Files Parameters P Package Assigning Choosing variants Copy 174 145,173 40,47,56 143 44 13 144 41,85 87 71 71 18 174 142 38 75 143 43 119 48 186 30 142 143 186 189 186 43 194 186 58 13 146 165 53,15
PPM graphic PREFIX PRINT Printout time Product information Product registration Project Creating File (EPF) Management Prototype manufacture Pwr Q QUIT Quotation marks R Rack file Rank Ratio Ratsnest RATSNEST RECT REDO REMOVE Rename Device Package Symbol RENAME REPLACE Request Resistor Device Package Symbol Restring width RIPUP ROTATE ROUTE Routing Automatically Manually 72 56 43,113 178 33,34 34 79 79 28 180 88,143 43 69 13,185,186 105 140 13 49,101 41,49 38 43,51,137 138 138 138 51 48,103 174 145 1
Spacing SPLIT Status display Stopframe Sup Superimposed pins Supply Autorouting layer Defining symbol Hidden gates Invisible Pin Layer Pin Symbol Swaplevel Symbol Copy Editing mode Labeling T Technology Changing Termination Of command Text In copper layer Menu Size, thickness Variables TEXT Text Editor Text menu Thermals In polygons In supply layers Title bar Tool tips Track Decompose Width Tree view Update 105 40,48 132 96 88,143 89 130 162 84 169 123 169 13,171 144 13 54,159 53 173 164 103 38 183 75 9
