EAGLE-Tutorial Version 4.Features of EAGLE

System Requirements

EAGLE is a powerful graphics editor for designing PC-board layouts and schematics. In order to run EAGLE the following hardware is required: IBM-compatible computer (586 and above) with Windows 95/98/ME, Windows NT4/2000/XP or Linux based on kernel 2.x, libc6 and X11 with a minimum color depth of 8 bpp, a harddisk with a minimum of 50 Mbyte free memory, a minimum graphics resolution of 1024 x 768 pixels, and preferably a 3-button mouse.

Professional Version

General maximum drawing area 64 x 64 inches (about 1600 x 1600 mm) resolution 1/10.000 mm (0.1 microns) mm or inch grid up to 255 layers, user definable colors command files (Script files) C-like User Language for data import and export simple library editing composition of user-defined libraries with already existing elements by Drag&Drop easy generation of new package variants from any library by Drag&Drop free rotation of package variants (0.1 degree steps) library browser with powerful search function support of technology feature (e.g. 74L00, 74LS00.) generation of graphics output as well as manufacturing and testing output with the CAM processor or the help the User Language printouts via the OS's printer drivers user-definable, free programmable User Language to generate data for mounting machines, test equipments, milling machines or any other data format partlist generation with database support (bom.ulp)
EAGLE-Tutorial Version 4.1
Drag&Drop in the Control Panel automatic backup function Layout Editor full SMD support support of blind and buried vias rotation of elements in arbitrary angles (0.1-degree steps) texts can be placed in any orientation dynamic calculation of signal lines while routing the layout tracks can be layed out with rounded corners in any radius mitering to smooth wire joints Design Rule Check for board layouts (checks e.g. overlaps, measures of pads or tracks) copper pouring (ground plains) package variants support Schematic Module up to 99 sheets per schematic simple copying of parts Online-Forward&Back Annotation between schematic and board automatic board generation automatic generation of supply signals Electrical Rule Check (error check in the schematic and consistency check between schematic and layout)

Autorouter Module fully integrated into basic program uses the layout's Design Rules change between manual and automatic routing at any time ripup&retry algorithm user-definable strategy by cost factors routing grid down to 0.02 mm (about 0.8 mil) no placement restrictions up to 16 signal layers (with user definable preferred directions) up to 14 supply layers full support of blind and buried vias takes into consideration various signal classes
Standard Edition The following restrictions apply to the Standard Edition in the Layout Editor: The layout area is restricted to a maximum of 160 x 100 mm (about 6.3 x 3.9 inches). Outside this area it is not possible to place packages and draw signals. A maximum number of 4 signal layers are allowed (top, bottom, and 2 inner layer). Light Edition (Freeware) The following restrictions apply to the EAGLE Light Version, which is available as Freeware (for testing and evaluation): The board area is restricted to 100 x 80 mm (about 3.9 x 3.2 inches). Outside this area it is not possible to place packages and draw signals. Only two signal layers can be used (no inner layers). A schematic can consist of only one single sheet. Larger layouts and schematics can be printed with the smaller editions. The CAM processor can generate manufacturing data as well.
EAGLE-Tutorial Version 4.Installation and Program Start

Windows

Insert the media into the CD-ROM drive. Select the desired menu item directly in the CD-ROM start window. If the start window does not automatically appear, double-click on the CD-ROM symbol in My Computer. Follow the instructions on the screen. For the Freeware installation you do not need a User License Certificate. Answer the question for a valid license by clicking Run as freeware. If you decide to uninstall EAGLE, use the unInstallShield program which will be installed along with the EAGLE program. The EAGLE CD-ROM supplies a playable Freeware. You can start it without installing it on your harddisk. But there are some minor restrictions due to the fact, that EAGLE can't write files on the CD-ROM.
Insert the CD and mount the CD-ROM drive. Choose the corresponding directory (/english/linux/install) and read the installation notes in the README file. While installing the program you will be asked if you want to run EAGLE as Freeware or as a licensed version. Choose Run as freeware, if you don't have a valid license. The EAGLE CD-ROM supplies a playable Freeware. You can run it from CD-ROM directly. Therefor you have to mount the CD-ROM drive as executable. But there are some minor restrictions due to the fact, that EAGLE can't write files on the CD-ROM.

Show Mark Mirror Rotate Change Paste Add Replace Value Miter Optimize Ripup Text Arc Polygon Signal
Info Display Move Mirror Group Copy Rotate Change Paste Add Gateswap Value Miter Invoke Text Arc Polygon Net Label Ratsnest ERC Errors Wire Circle Rectangle Via Hole Cut Delete Pinswap Name Smash Split Route
Info Display Move Mirror Group Cut Delete Pinswap Name Smash Split Wire Circle Rectangle Bus Junction ERC

Show Mark

Auto DRC
Command toolbar of the Schematic Editor (left) and the Layout Editor (right)
EAGLE-Tutorial Version 4.Control Panel
After starting EAGLE, the Control Panel will be opened. It allows you to load and save projects as well as to setup certain program parameters. Right mouse click to an entry in the Projects branch of the tree view opens a context menu that allows to start a new project. The tree view allows a quick survey of EAGLE's libraries. Double-click an entry in the Libraries branch. Now the contents of the library is displayed. Selecting an object shows a short descriptive text on the right.
Control Panel: Preview of the library contents The Control Panel offers also an overview of User Language programs, Script files, and CAM jobs. Try selecting various entries. On the right you will get the referring description. The Control Panel supports Drag&Drop in usual manner. A right mouse click on any entry in the tree view opens a context menu that offers options like print, open, copy, etc. The paths for each branch of the tree view are set in Options/Directories.

EAGLE Files

The following table lists the most important file types that can be edited with EAGLE: Type Board Schematic Library Script File User Language Program Any text file Window Layout Editor Schematic Editor Library Editor Text Editor Text Editor Text Editor Name *.brd *.sch *.lbr *.scr *.ulp *.*
The Linux version only recognizes lower case letter file extensions!

Backup Files

EAGLE creates backup data of schematic, board, and library files. They will be saved with modified file extensions:.brd becomes.b#1,.sch becomes.s#1, and.lbr becomes.l#1. There can be a maximum number of 9 backup files. It is also possible to have EAGLE files saved in a certain time-interval. In this case the files get the extension b##, s## or l##. The files can be used again after renaming them with the original file extension. All settings concerning backups can be done in the Options/Backup menu of the Control Panel.

Create EAGLE Projects

Lets create a new project first. After starting the program, first the + character of the Projects path, then the + character of the entries examples and tutorial in the tree view. The contents of the tutorial directory appears. tutorial with the right mouse button. Select the option New Project in the popup menu. Name the new project MyProject, for example and hit the Enter key. This way you are creating a subdirectory of tutorial that is named MyProject. This directory should contain all data files that belong to your project. Of course you may define additional subdirectories. To define the path where your project directories will be stored, click Options/Directories and enter it in the Projects field. A right mouse click on the project entry and you can open new schematics, layouts and libraries. Each project directory contains a file named eagle.epf which stores project-specific settings, window positions etc.
The currently active project is checked (green) in the Control Panel. After starting the program again the previous situation will be restored. The last used project and other user-specific settings are saved in the file ~/.eaglerc (Linux) or eaglerc.usr (Windows). Before starting the following examples we want to copy the files demo1.sch, demo2.sch, and demo2.brd into the directory MyProject. Press the Ctrl key, click the desired file and drag it to the tutorial entry. Release the mouse button now. Repeat this for the other files. The Ctrl key effectuates that the files will be copied, otherwise they would be moved to the target directory. Now open the schematic file demo1.sch with a double click. If you end the program with Alt+X and start it again, you will get the previous settings and editor windows.
EAGLE-Tutorial Version 4.Load File and Select Monitor Zoom
Now let us start doing some exercises. Start EAGLE, and wait until the Control Panel appears. Expand the entry Projects/examples/tutorial/MyProject of the tree view. Now load the demo2.brd file. You can do this either by the entry demo2.brd, or by selecting the file from the menu File/Open/Board. The schematic with the same name will be loaded along with the board. Enlarge the board editor window. First click the icon in the action toolbar to zoom into the drawing. This WINDOW command can also be executed by pressing the function key F3. If you are working with a wheel mouse, you can zoom into or out of the drawing by turning the mouse wheel. The setting for Mouse wheel zoom = 0 in the Options/User Interface menu deactivates this feature. The zoom factor can be set with the option Mouse wheel zoom. Click this icon or press F4 to zoom out of the drawing.
By clicking this icon the drawing will be shown in full size to fit your screen (you can also use Alt+F2 instead). Click this icon and then mark a rectangular area by dragging the mouse cursor while the left mouse button is pressed. Then release the mouse button. The marked area will now be displayed. To move the chosen window simply click the middle mouse button and move the mouse. This also works while an editor command is active, for example, while drawing nets or wires. To scroll beyond the drawing borders additionally press the Shift key. If the cursor is over the vertical or horizontal scroll bar and you are working with a wheel mouse, you can move the screen up and down or to the right or left by turning the mouse wheel. During certain actions it may happen that objects in the drawing disappear or get corrupted. In this case refresh the screen by clicking the Redraw icon (also F2 possible).

The WINDOW command is more versatile than in other programs: Click this icon if you want to select a new center with the same zoom factor, mark the center with a click and finally click on the traffic light icon in the action toolbar. If you want to select a new center and a new zoom factor simultaneously, click on the same icon. Three mouse clicks will give you the desired result: the first click will define the new center and both last clicks will define the zoom factor. If the third point is further away from the first, the program will zoom into the drawing and vice versa. Try it to find out how it works. Further possibilities can be found on the help pages of the WINDOW command. These can be called up by simply typing in the command line: HELP WINDOW
EAGLE-Tutorial Version 4.Selecting Layers for Display
EAGLE-Drawings contain objects in different drawing layers. In order to obtain a useful result several layers are combined for the output. For example, the combination of Top, Pad, and Via layers is used to generate a film for etching the component side of the printed-circuit board. Consequently the combination of Bottom, Pad, and Via layers is used to generate the film for the solder side of the board. The Pad layer contains the through-holes for the component connections and the via layer contains the via-holes which are needed when a signal track changes to another layer. Load the board demo2.brd using the menu File/Open/Board and click in the command toolbar on the icon for the DISPLAY command (look at the toolbar layout on the previous pages). The marked layers are currently displayed. By clicking on the layer number the display of each layer can be switched on or off. The All and None buttons switch on or off all layers. By selecting/deselecting layer 21 tPlace (silk screen upper side), the layers 23 tOrigins, 25 tNames, 27 tValues, and 51 tDocu are selected/deselected, too. The same applies to layer 22 bPlace (silk screen bottom side). Very important: Components on layer 1 Top can only be moved or selected in the drawing if layer 23 tOrigins is on. The same applies to components on layer 16 Bottom and the layer 24 bOrigins. To select a certain layer in the DISPLAY menu click on the layer name. Now you can use the Change button to modify the layer's properties like name, color, or fill style. Please consult the help page of the LAYER command for the meaning of the different EAGLE layers.
EAGLE-Tutorial Version 4.Setting up Grid and Unit
Schematics should always be drawn on a grid of 0.1 inches (2,54 mm) since the libraries are defined this way. The grid for boards is determined by the components used and by the complexity of the board. Grid and unit are setup with the GRID command by clicking on the GRID icon in the parameter toolbar. All values are given in the currently selected unit. Please consult the help pages of the GRID command for detailed information. For all settings in the Design Rules window ( Edit/Design Rules.) one can use values in mil or in millimeters (1 mil = 1/1000 inch). The default unit is mil. If you prefer to work with millimeters simply add the unit to the value, for example: 0.2mm Inch - Mil - Millimeter Table for the Most Usual Values: inch mil mm 0,0,2032 0,0,2540 0,0,3048 0,0,4064 0,0,6096 0,0,8128 0,1,0160 0,1,2700 0,2,5400 The GRID dialog allows setting an alternative grid which can be activated by pressing the Alt key in the Editor window.

EAGLE-Tutorial Version 4.Wires, Circles, Arcs, Rectangles, and Text
Wires, circles, arcs, rectangles, and text are created with the WIRE, CIRCLE, ARC, RECTANGLE and TEXT commands. On one hand these objects serve as pure drawing elements for symbols, packages, frames etc., and on the other hand they can perform special functions, such as the definition of restricted areas. First a new schematic file is to be created. Close all of the editor windows and select File/New/Schematic from the Control Panel. A new file with the name untitled.sch is now created. Normally you should never save a file with the name untitled, but should use File/Save as to choose a different name. However, in this tutorial no file is to be saved at all. Now enlarge the editor window.

The WIRE Command

The WIRE command is used to draw lines. Click the WIRE command in the command toolbar. All parameters for this command can be set up in the parameter toolbar. Next select layer 94, Symbols, from the layer-selection combo box. In this layer a rectangular line is to be drawn.
Parameters of the WIRE command Define the starting point by a click on the left hand mouse button. Move the cursor slightly up to the right and press the right hand mouse button a few times. This way one changes the bend mode (wire bend). Among some diagonal and orthogonal modes you will find some to draw 90-arcs and free definable arcs. However, in the Schematic Editor the arc modes can be selected only in the parameter toolbar, not with the right mouse button. Keeping the Shift key pressed while clicking the right mouse button will change the selection order. Pressing the Ctrl key toggles between corresponding wire bends. When the connection is displayed in a square angle, press the left hand button to fix its position. Now move the cursor to the starting point and to drop the line. Now you should be able to see a rectangular outline. As
observed before, an angle between wire segments can be created by clicking the right hand mouse button. This is more effective than using the symbols in the parameter toolbar. Attention: Do not use the WIRE command to draw net or bus lines in schematics - use NET or BUS instead! In the Layout Editor: If the lines (WIRE command) are placed on the board layers Top, Bottom, or Route2.15 EAGLE treats them as electrically conducting tracks. Wires are also used to create board outlines. Lets start using this command.

Changing Line Width

As long as the WIRE command is active, you can select the line width from the combo box in the parameter toolbar or type in a specific value, separate for each segment. To change the line width of an existing object, CHANGE icon in the command toolbar and a popup menu will open up. WIDTH entry and a further popup menu will show up where the present value is marked. Select the desired value by a left mouse click, then click the object to be changed. To change the line width to a value that is not shown in the menu of the CHANGE command, click the entry. and type in the value in the Change Width window. Alternatively use the command line to type in the value, for example: CHANGE WIDTH 0.017 Then click on the wire segment you want to change or start drawing a new wire. To change the wire style CHANGE and Style. Select the style and the wire you want to change.
Change Object to another Layer
To move an object, for example a wire segment, to another layer CHANGE LAYER Select the target layer, for example 94 Symbols, by. Then OK, and then on the selected object(s). Note that some objects, such as bus or net lines, cannot be moved to another layer as they have a special meaning.

Undo/Redo Function

One of the most useful features of EAGLE is the unlimited Undo function. Click the left icon as many times as you want to undo previous actions. Use the right icon to redo the actions which have been cancelled by undo.

The CIRCLE Command

To activate CIRCLE, which is used to draw a circle, CIRCLE EAGLE requires two mouse clicks to define a circle. The first click sets the center of the circle and the second click defines the radius. Place the cursor at any grid point and . Drag the cursor several grid points to the right. When the circle has the diameter you want, to fix it and terminate the command. The line width of the circle can be changed as described before for wires. A circle with line width 0 will be filled. Example for drawing a circle using coordinate values: A circle with the origin at position x = 10 and y = 25 and a radius of 15mm should be drawn. First set the grid to millimeter: GRID MM Draw the circle now: CIRCLE (10 25) (10 40) or CIRCLE (10 25) (10 10) The second pair of coordinates describes any location on the
circumference. So various values are possible to describe one certain circle. To find out more about the CIRCLE command press F1 as long as the command is activated or type HELP CIRCLE. To cancel a command, click the stop sign icon or activate another command. Pressing the Esc key generally unlocks an object from the cursor.

The schematic consists of the following elements: Part
C1 C2 C3 C4 C5 D1 IC1 IC2 JP1 JP2 Q1 R1 F1
30p 30p 10n 47u/25V 47u 1N4148 PIC16F84AP 78L05Z PROG APPL 2,2k

Device

C-EUC1206 C-EUC1206 C-EU025-025X050 CPOL-EUTAP5-45 CPOL-EUTAP5-45 1N4148 PIC16F84AP 78L05Z PINHD-1X4 PINHD-1X17 XTAL/S R-EU_R1206 DINA4_L

Package

C1206 C1206 C025-025X050 TAP5-45 TAP5-45 DO35-10 DIL18 TO92 1X04 1X17 QS R1206

Library

rcl rcl rcl rcl rcl diode microchip linear pinhead pinhead special rcl frames
Use the ADD command to place the listed devices. Please keep in mind: You really should not change the default grid of 100 mil (= 2.54 mm) in the Schematic Editor. Only this way you can be sure that nets will be connected to the elements' pins. You can toggle the grid on and off by clicking the GRID icon or more easily by using F6, to help you locating the parts. Once you have placed the parts you can relocate them with the MOVE command. Activate the MOVE command by clicking the appropriate icon in the command toolbar, then move the cursor to the part you want to move and . EAGLE will highlight the part, to let you know that it is attached to the cursor and ready to be relocated. Relocate the part, and to place it in its new location. The MOVE command is still active and ready to move the next part. Press the right mouse button if you want to rotate a part. For duplicating parts you may use the COPY command (for example, C1 and C2). Thus you don't have to fetch each part with the ADD command. When you have located the parts, start connecting them using the NET command.
Attention: Use the NET command, not WIRE!
The NET Command A net is only connected to a pin if it is placed on the connection point of the pin. Display the layer 93, Pins, with the DISPLAY command to locate these connection points. They are marked with a green circle. EAGLE automatically names electrical connections (nets). In our example demo1.sch the net lines at C5 pin +, U1 pin 3(VI), and JP2 pin16 have the same name. The pins are connected to the same net, although the net lines are not draw continuously. While the NET command is active, the status bar below shows properties of the selected net. As mentioned before, nets with the same name define an electrical connection. The NAME Command EAGLE automatically allocates names such as B$. for buses, P$. for pins and N$. for nets. NAME and then the net connected to IC1 pin OSC1 (16). A popup menu shows the predefined name of the net. Type in OSC1 and OK. The net immediately now has this name. The names of components and busses can be changed in the same way. The LABEL Command The LABEL command allows you to place bus or net names on a schematic in any location. LABEL, locate the cursor on the net MCLR/PGM and . The name of the net is attached to the cursor and you can place it in any location. You can also rotate the label with the right mouse button. Locate the label approximately as shown in the figure and to fix its position (near JP1 pin 3). If net or bus names are changed, the relevant labels are also changed. Label text is not changed with the CHANGE TEXT command but with the NAME command and a click on the net line or the bus line. CHANGE FONT or CHANGE SIZE changes the font or the text size. The DELETE Command You can delete objects with this command. If it is applied to nets, wires or busses, a single segment is deleted at a time. To use this command,

The GROUP Command One of the most useful commands of EAGLE is the GROUP command. It allows you to select several objects, change their attributes and move, rotate or mirror them all at once. To use the GROUP command GROUP Then, by clicking and releasing the left mouse button, draw a polygon around a group of objects and close the polygon by pressing the right mouse button (dont use the POLYGON command). The selected objects are now highlighted. Please make sure that you only select objects which are in a visible layer. Packages on the Top layer can only be selected if layer 23 tOrigins is visible, and packages at the Bottom layer can only be selected if layer 24 bOrigins is visible. Use the DISPLAY command to show or hide layers. Next select the MOVE command and use the right mouse button to attach the group to the cursor. This way you can move all the objects simultaneously, rotate them with the right mouse button and fix them with the left mouse button. After a group has been defined with the GROUP command, the attributes of the contained objects can be changed with the CHANGE command. Select a group that contains some wires, CHANGE in the command toolbar, Width, and 0.032. Then click the right mouse button somewhere in the editor window. You can reverse the action with the UNDO command. A rectangular group can be defined by selecting the GROUP icon, clicking one corner of the area of interest, keeping the mouse button pressed and dragging the mouse button until the rectangle contains the desired objects. The SPLIT Command With the SPLIT command you add a bend in a wire. SPLIT in the command toolbar on a wire segment near its target point Drag the wire on the screen a bit. You will see that the longer segment remains as a direct line to the selected point, while the shorter segment splits into two. The angle of the two new segments is controlled with the right mouse button. fixes the wire segments. The CHANGE Command Use the CHANGE command, to change the width of wires or to move a wire to another layer. To change the width of the wire:

CHANGE WIDTH in the popup menu the value for the new width Then move the cursor to the wire segment to be changed and. To change the width to a value not present in the menu, e.g. to 0.23 inches, the entry. A window pops up where you can type in the value. You could also use the command line: CHANGE WIDTH.23 and click the wire segment. To move a wire segment to another layer : CHANGE LAYER desired layer wire segment In case a via is needed to complete the signal path, EAGLE will automatically insert it. If a via becomes redundant, EAGLE will automatically remove it. The ROUTE Command Use the ROUTE command to change an airwire into a wire. You can fix the position of a wire segment with , then change direction and fix the next segment until the airwire is completed. See also the section Routing Manually some pages before. The RIPUP Command If you would like to turn for example the routed signal tracks GND and VCC into airwires (this process is called ripup), click the RIPUP icon in the command toolbar and type: GND VCC Pressing F9 twice reverses the action. If you would like to ripup all signals except GND and VCC, type: ! GND VCC after the RIPUP command has been activated.
The SHOW Command Use the SHOW command to highlight airwires, wires or components. Click on the Zoom-to-fit icon and then the SHOW icon. Then type: IC1 to locate IC1. The status bar shows information about the object. Refresh Screen Use the F2 key to refresh the screen contents or click the Redraw icon. Undo/Redo Function All actions mentioned can be reversed with the UNDO icon in the action toolbar (F9) and repeated with the REDO icon (F10). Inner Layers Inner layers (Route2.15) can be used for routing in the same way as the Top and Bottom layers. This is not possible in the freeware (light edition). Supply Layers Only possible in standard and professional edition! Inner layers (Route 2.15) can be used as a signal or ground plane simply by renaming the layer $signalname, when all signals with that name will then be connected to this layer. To demonstrate this feature load the board file demo2.brd and type: SHOW GND The GND signal will be highlighted. Then type: RIPUP GND The signal GND will now be displayed as airwires only. Now we will define layer 2 as the ground layer by naming it $GND (the name of the signal must be preceded with the $): LAYER 2 $GND You can also select Layer 2 Route2 in the DISPLAY menu, click the Change button, activate the option Supply Layer and type in the name GND. Click the RATSNEST icon to make the airwires of the signal GND
disappear. To have a look at the result switch of all layers except for the $GND layer. This can be achieved by clicking on the DISPLAY icon, or simply by typing the following command on the command line: DISPLAY NONE $GND Remember you can use lower case characters and abbreviate key words. So you can type dis none $gnd Now type SHOW GND and the thermal symbols which connect the GND signal to the supply layer are highlighted. The annulus (round) symbols isolate the throughholes not belonging to the GND signal. In our example the elements C1 and C2 don't have a connection to the inner layer yet. You have to ROUTE a short track out of the smd and place a VIA on the tracks end. Now the connection to the inner layer is made. Supply layers defined with $name are plotted inversely, i.e., objects with the color of the supply layer define copper-free areas. The thermal symbols connect the ground plane with the through-hole using four conducting paths. Copper Pouring with the POLYGON Command The POLYGON command enables you to define areas which belong to a signal, connecting all of the related pads to this signal with thermal symbols. Such a signal retains a user-defined distance to any other signal path. You can design layers that contain multiple polygons such as different ground areas, and you can design polygons on multiple layers. To demonstrate this feature of EAGLE, lets fill the Top layer of a board with the GND signal. Reload the board demo2.brd once again, enlarge the window, and ripup the GND signal: RIPUP GND Use the DISPLAY command to switch on the layer 1 Top, 17 Pads, 18 Vias, and 20 Dimension. Use the button None, in the menu, to switch off the display of all other layers first. Click the POLYGON icon in the command toolbar and type: GND to provide the name GND for the polygon to be defined. Only then will it belong to the GND signal.

Resistor Package

Select the package editing mode via the icon in the action toolbar, and enter the package name R-10 in the New field. Answer the question Create new package R-10? with Yes. Later when creating a new symbol and a new device you will again have to answer the corresponding questions with Yes. Use the GRID command to set an appropriate grid size for the pad placement. 0.05 inch (i.e. 50 mil) is usual for standard components with lead wires. For a resistor with lead-wires, select PAD, and set the pad shape and the drill diameter in the parameter toolbar. Default value for pad diameter is 0. It should not be changed. The final diameter in the layout results from the values given in the Design Rules. Then place two pads at the desired distance. The origin of the drawing will later be the identifying point with which a component is selected. For this reason it should be somewhere near the center of the device. 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. Select Top as the layer, even if the component will later be placed on the underside of the board. SMD components are located on the other side of a board using the MIRROR command. This moves the elements in all the t.-layers into the corresponding b.-layers. Place the two SMD pads (which in EAGLE are just called SMDs) at the
desired distance. To use round SMDs (BGAs) define a square one first, then CHANGE the value for Roundness = 100%. You can now enter the names, such as 1 and 2, for the pads or SMDs using the NAME command. A different procedure is however recommended for components with many sequentially numbered pads: Select the PAD command, type in the name of the first pad, e.g. '1' (the inverted commas must also be entered), then place the pads in sequence. Now use the WIRE command to draw the silkscreen symbol in layer 21 tPlace. This layer contains what will be printed on the board. It is up to you how much detail you give to the symbol. Set a finer grid size if it helps. Take the information provided in library.txt (in eagle/doc) as a guideline for the design of components.You may also use the ARC, CIRCLE, RECT and POLYGON command to draw silkscreen symbols. Please take care in layer 21 tPlace not to cover any areas that have to be soldered. In layer 51 tDocu a more realistic appearance can be given which is not subject to this limitation. 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 print documentation. In the example of the resistor, the symbol can be drawn in layer 21 tPlace, but the wires, which go over the pads, are drawn in layer 51 tDocu. With the TEXT command you place the texts >NAME in layer 25 tNames and >VALUE in layer 27 tValues in those places where in the board the actual name and the actual value are to appear. SMASH and MOVE can be used later to change the position of this text relative to the package symbol on the board. The CHANGE command can be used at a later stage to alter object properties such as the stroke thickness of texts (ratio), text height, or the layer in which the object is located. If you want to change the properties of several objects at one go, define a group with the GROUP command, click the CHANGE command, select the parameter and the value, and click into the group with the right mouse button. Example: Use GROUP to define a group that contains both pads, then select CHANGE and SHAPE/SQUARE. Click on the drawing surface with the right mouse button. The shape of both pads changes.

The Connect window In this example the resistor gate has been named G$1 automatically. This is the reason why you see the pin name G$1.1 and G$1.2 in the column Pins. The column Pad shows the pads placed in the package. Click on a pin and a pad entry and click the Connect button. If you want to disconnect a pin from a pad, select the pair in the Connection column and click Disconnect. OK ends the CONNECT command and closes the window.
The Device Editor You can enter information concerning the device after clicking the DESCRIPTION command. The entered text will be displayed in the
Control Panel, when you select the device in the tree view. It will also be checked by the search function of the ADD command. Now the definition of the resistor is complete. You can use it in a schematic now. Keep in mind to load the new library with the USE command. Otherwise it is not available for ADD.
EAGLE-Tutorial Version 4.Output of Drawings and Manufacturing Data
EAGLE can output drawings, for example for documentation purposes, using the PRINT command. This command can be found in the File menus of the Schematic or Layout Editor. You can use the printers defined under Windows with this command. The Linux version generates Postscript files that can be sent to lpr or to a file. A printout of the drawing in the active editor window with the actual layer settings (DISPLAY command) will be generated. Film and manufacturing data are generated with the CAM Processor. Start it with the icon in the action toolbar of the Layout Editor window. The CAM Processor uses its own drivers, which can be defined or modified by the user (see file eagle.def in directory eagle/bin). Data for a bill of material, for mounting, milling or testing machines etc. can be generated with the help of EAGLE User Language Programs. Information about ULP's can be found in the file headers or with the help of the descriptions in the Control Panel.
Output a Schematic with the PRINT Command
The schematic demo1.sch is to be printed in black/white and full format on one page. Load the file demo1.sch and choose the layers which should appear on the print-out with the DISPLAY command. All layers visible on the screen will be printed. Click the PRINT icon in the action toolbar. Check the boxes Black, Solid and Rotate (as the drawing is in landscape format). The boxes Mirror and Upside down are not marked. For both Scale factor and Page limit type in 1. This specifies that the drawing is to be output at a scale factor of 1, provided it fits onto one page. If not, EAGLE changes the scale factor, so that the drawing does fit onto one page. With Page limit 0 the drawing will always be printed with the set scale factor. The printer can be selected by using the button Printer. The button Page leads you to the page setup parameters. If the box Caption is checked, the drawing will be printed with a footer, containing the file name, date, time, and scale factor.

Three Modules One Program

Schematic Module

The integrated Schematic module gives you more than just a circuit diagram. When the circuit is drawn, a large part of the layout work is already done!
Please feel free to compare EAGLE with all those high-priced packages!
Download our freeware test version now from www.cadsoftusa.com

Layout Editor

This is the most basic EAGLE module, needed for all versions. You can omit the Schematic Editor and the Autorouter if you want, or you can order them later. With the Layout Editor you can design complete circuit boards manually. It comes complete with all the libraries, with a library editor and the CAM processor, as well as all the available output drivers.

EAGLE 4.1

Schematic Layout Autorouter

Autorouter

The integrated Autorouter takes a lot of routine work away from you. It handles boards of up to 16 layers. Smallest routing grid: 0.02 mm. You can apply the automatic routing to individual signals, to groups of signals, or to all signals that are still unrouted. Design rules and strategy parameters can be set by the user.

Windows Linux Mac

Technical Data
EAGLE Professional: max. drawing area 1.6 m x 1.6 m (64 in x 64 in) 1/10000 mm resolution 255 drawing layers 16 signal layers up to 99 sheets per schematic extensive libraries supplied undo and redo function for any number of commands components on both sides (conventional and SMD) rotation of components in any angle support of blind, buried, and micro vias copper pouring (e. g. for filling ground areas) on-line Forward&Back annotation on-line calculation of airwires when laying-out wires wires can be drawn as arcs Design Rules define pad/via attributes net classes for autorouter and DRC round or rounded SMD pads different pad shapes for top, bottom, or inner layers output drivers for all standard photoplotters and drill formats execution of command files integated C-like User Language permits manipulation of EAGLE data for any other software and hardware (e. g. simulators, component insertion machines, ATE). EAGLE Standard: As Professional, but routing is only possible on an area of 160 mm x 100 mm (6.3 x 4 inches), and in up to four signal layers. Larger boards and drawings outside this range can be loaded. EAGLE Light: As Standard, but the maximums are a routing area of 100 mm x 80 mm (4 x 3.2 inches), two signal layers and one schematic sheet (of any size).
CALL US NOW: 800-858-8355

CadSoft Computer, Inc.

801 Federal Hwy., Delray Beach, FL 33483 Support (561) 274-8355, Fax (561) 274-8218 E-Mail : info@cadsoftusa.com
Web: http://www.cadsoftusa.com
Windows is a registered trademark of Microsoft Corporation. Linux is a registered trademark of Linus Torwalds. Mac is a registered trademark of Apple Computer, Inc.
Why have so many top companies chosen EAGLE as their PC-board design tool?
Quality without Compromise Easy to Learn and Use
With EAGLE you can create pcb films and documentation which satisfy the highest demands on quality. There is no need to compromise either quality or size. EAGLE is very easy to use, in spite of all its facilities. Do not underestimate the effect this can have on costs! Schematic, layout and component editors have identical user interfaces. A unique UNDO/REDO function, with which any previous state of the design can be reconstructed with a few keystrokes, is just one example of EAGLE's friendliness. EAGLE was developed by CadSoft itself. This means you can talk to somebody about what you would like to see, and about suggestions for improvement. With EAGLE, CadSoft won first place in a well-known magazine's survey of software users, which shows that this is more than mere words. The quality of the program and the support from the manufacturer were both judged. And at CadSoft there is no hotline fee! Check out EAGLE with our Light Edition which is freeware for test purposes and non-commercial projects. You can download it from our Internet site. EAGLE Light allows you to design boards up to 4 x 3.2 inches (one schematic sheet). All other features are the same as in the Professional and Standard Edition. All of the component libraries are contained in EAGLE Light, as well. Closed solutions are out! Cooperation with other programs and the output of data to other processing engines is becoming ever more important. EAGLE is an open system, with a universal ASCII input interface. And the User Language is able to arrange the output flexibly. The C-like language permits the output of data in any format. But don't worry, you don't have to be a programmer to benefit from this.

Design with EAGLE: It's that simple!
You draw a schematic using the symbols which you fetch from the supplied libraries. You then click the Switch-to-Board icon, and the component's packages appear next to an empty board, with the connections shown as rubber bands. You can then locate the components on the board. Thanks to on-line Forward&Back annotation, the schematic and the board always remain consistent.
Now the desired connections (shown as rubber bands) are converted into non-crossing tracks. In EAGLE this can be done by hand, or the autorouter can do it automatically. Critical connections are usually made by hand, while the remainder are left to the autorouter.
Effective Customer Support

Try Before Buy

To rule out the possibility of errors caused by the manual work, EAGLE carries out a design rule check (DRC). This will check whether, for example, there are shortcircuits on the board, or whether different potentials are too close to one another.
Talk to the Rest of the World
Just a few of our customers
3M, AEG, Airbus, AMD, AMP, Amphenol-Tuchel, AT&T, Audi, BASF, Bayer, Black&Decker, BMW, Caltech, Daimler Chrysler, DFW International Airport, Du Pont, Eastman Kodak, Goodyear, Grundig, Hewlett-Packard, Hitachi, Honeywell, Hughes, IBM, Intel, ITT, Lockheed, Lufthansa, Mercedes, Motorola, Minox, NASA, National Semiconductor, NCR, NEC, Nokia, Philips.
You can design your own circuit symbols and packages as easily as you can schematics and layouts. You can alter or extend existing libraries to suit your needs or comfortably compose your own libraries. You decide what the symbols will look like, where the labeling should appear and what size it should have, what shape and size of solder land you want to use, what the rotation of a package should be. Even complicated components are defined within a few minutes.