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.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.

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 ARC Command

To activate the ARC command, which is used for drawing arcs, ARC An arc is defined with three mouse clicks: the first click defines the start point, the second the diameter and the third the end point. Place the cursor at the desired starting point and. Now move the cursor some grid units to the right but remain on the same Y-coordinate. A circle appears which shows the diameter of the arc. and the circle will become an arc. Now you can change the direction of the arc with the right mouse button. Click several times with the right button and you will see what is meant. You can also enlarge or minimize the arc by moving the mouse. After reaching the desired form, to fix the arc. The parameters flat and round determine the shape of the arc's ends. Practice by drawing some arcs. Use the help function to find out more about the ARC command. All this can be done with the WIRE command as well!

The RECT Command

To activate the RECT command, used for creating filled rectangles, RECT To define a rectangle two mouse clicks are required: The first one will determine one corner and the second determines the position of the opposite corner. Move the cursor to the point where a corner of the rectangle should be and. Move the cursor slightly to the right and up. When the rectangle has reached the desired size, to fix it. The rectangle is filled with the color of the layer in use. Use the help function to find out more about the RECT command.

The TEXT Command

To activate the TEXT command, used for placing text, TEXT Now type the desired text and OK. Then place the text with. A copy of the same text is now attached to the cursor. To stop placing text simply click the next command icon. For placing a different text, type the text and terminate it with the Enter key. The text will show up in the command line. Texts containing spaces or a semicolon have to be enclosed in single quotes, like this one: 'This is a text' To change the text font: CHANGE FONT EAGLE supports a vector, a proportional, and a fixed font. To change the size of a text: CHANGE SIZE Value in the menu or type in any desired value in the command line (confirm with the Enter key) and lower left corner of the text. At a rotated text the point of origin can move to its upper right corner. A text in a schematic is always displayed in a way that it can be read from the front or from the right. The Layout Editor allows to display texts in any orientation. Use the Spin flag which is located in the parameter toolbar while the TEXT, MOVE, or ROTATE command is active to get texts readable from all directions. To change a text CHANGE TEXT and at the point of origin of the text, then edit the text and on OK. Using CHANGE RATIO you can change the line width in a text in relation to the height of the vector font. See help page for more information about TEXT and CHANGE.

Special Text Variables

If you place the text >SHEET this string will be substituted with the current sheet number, e.g. 1/1 (sheet one of totally 1). EAGLE offers a number of similar text variables, e.g. for date/time which reflect the latest change in the file (>LAST_DATE_TIME) or the drawing output (>PLOT_DATE_TIME). Library parts are defined with text variables for the name >NAME and the value >VALUE of a component. Furthermore one can use >PART and >GATE for symbols.
EAGLE-Tutorial Version 4.Using Libraries
EAGLE comes with a lot of library files that contain through-hole and surface mount devices. The tree view in EAGLE's Control Panel offers detailed information about the contents of the libraries. In this section you will learn how to insert schematic symbols into a drawing and how to use them. Open a new schematic to start with a blank drawing area File/New/Schematic.

The ADD Command

To select symbols from a library, ADD in the command toolbar, and a window pops up. On the left side a list of available libraries should appear. Each library entry can be opened by clicking the + character. Now it's contents will be shown. Select an entry and you will see the corresponding preview on the right. Now you can enter on or more search patterns in the Search field. You may use the name of a device or any word of the device description. Wild cards like * and ? are allowed. If there are no entries visible after using ADD for the first time, no libraries have been loaded. In this case, please read the following chapter dealing with the USE command. We want to place, for example, the device 74LS00. Enter in the Search field: 74*00* or 74LS00* * is the wild card of the technology and/or the package variant. The search result shows the device in various technologies and package variants. Select the desired device and OK. Now you can place it in the schematic. Place the cursor slightly to the left of the display center and. Move the cursor to the right, and place a second gate with the next mouse click. Place four gates around the center of the drawing area in this way. Now place a fifth gate somewhere nearby. Please note that EAGLE has named the first four gates IC1A.IC1D, whereas the fifth gate has been named IC2A, since this gate requires a second IC. If you now show the layer 93, Pins, either as described before or by typing DISPLAY PINS in the command line, further pin parameters are displayed in green. Zoom in on the drawing, so that a gate is shown on a large scale. You will see that the pins are marked as Input (In) or Output (Out), and that a number

Adding and Changing Text

You can add lines, text and other objects to predefined frames and text fields in the library. Or you can design and save your own frames. Variable texts, e.g. the project title or the revision number, can be inserted directly in the Schematic Editor where you are now. Frames are saved as symbols in the library, therefore it makes sense to write the text in layer 94, Symbols. Now bring the frame text field into the editor window so that it is completely visible. Next click the icon for the TEXT command and enter the following text
CadSoft After clicking the OK button, the text is attached to the cursor and can be placed with the left mouse button. Move the text in the upper empty line of the text field and place it with a. A further copy of the text, which will disappear as soon as another command is activated or the stop sign icon is clicked, is still attached to the cursor. If you did not define the size of the text while the TEXT command was active, you can use the CHANGE command to set it to another value: CHANGE From the menu select: SIZE and a further window opens in which the presently selected text height is shown. 0.15 and move the cursor to the lower left corner of the text CadSoft. Click the left mouse button and the text height will be changed to 0.15 inches. Just in case you would like to set a size not present in the CHANGE SIZE menu, like. 0.17, simply type: CHANGE SIZE 0.17 and then click the lower left corner of the text. Attention: Use dots for decimals! The current grid setting determines the unit! Practice manipulating texts by adding an address or a document number in the text field. TITLE: contains the file name in use (text variable >DRAWING_NAME). DATE: contains the date of the most recent save command (text variable >LAST_DATE_TIME). Both fields are automatically filled with the actual data when the drawing is saved, since the frames stored in the frames library have been defined with the appropriate text variables.

Entering a Schematic

Now lets start drawing a schematic. We will be drawing the schematic shown in the following figure, which you can use for reference. If you dont want to enter the whole schematic you can use the file demo1.sch stored in the eagle/examples/tutorial directory. Start by pressing ALT+F2 or clicking the Zoom-to-fit icon to fill the window with the drawing frame.

DELETE in the command toolbar, take the cursor to the object that is to be deleted, and. Keep the Shift key pressed while deleting an object in order to delete the whole net or bus. More about this in the help function. UNDO and REDO work here as well. GROUP, DELETE and a right mouse click delete whole groups.

Schematic demo1.sch

The JUNCTION Command Dropping a net on another net line generates a connection between these two nets. The connection will be represented by a junction, that will be set automatically. Automatic setting of junctions can be switched off with the option Auto set junctions ( Options/Set/Misc). In this case the JUNCTION command is used to draw a connecting node at the intersection of nets which are to be connected to each other. JUNCTION and a node is attached to the cursor. Locate the node at the junction of two net lines and to fix it into place. The SHOW Command This is a good time to demonstrate the function of the SHOW command. This command is used to show names and other details of elements and objects. Complete signals and nets can be highlighted, as well as components. To show for example the net V+, SHOW in the command toolbar then move the cursor to the connection point of U1 pin VI (3) and. Please notice that EAGLE highlights the net wires and each pin connected by this net, as well as the pin name of each part to which it is connected. In addition, the signal is listed in the status bar as: Net: V+, Class: 1 Power While the SHOW command is active the net remains highlighted although you are panning the window by pressing the middle mouse button and moving the mouse or using the WINDOW command. Deactivate the SHOW command by clicking the stop sign icon and use WINDOW REFRESH (F2). Now the objects are no longer highlighted. To show an object with a specific name, SHOW and type the name (for example D0 ) in the command line. You can subsequently type other names without the need to reactivate the SHOW command. This way you can mark one net after the other. Do you wish to highlight several nets at the same time, enter in the command line: SHOW RA4 SHOW RA3 SHOW RA2
The MOVE Command No electrical connection will be generated if you move a net line over a pin (using the MOVE command). On the other hand: if you move a pin over another pin or over a net line, an electrical connection will be generated, and a net line will be attached to the pin when the component is moved further. Remember the UNDO command if you want to detach the net line. Check the connections with the SHOW command, as mentioned before. Additional one can export a net or pin list with the EXPORT command. History Function With the keys up-arrow and down-arrow you can recall the last keyboard instruction into the command line and execute it with the Enter key. The Esc key will delete the command line. Use Alt+F2 to show the whole schematic on the screen, then type: SHOW R1 SHOW C1 SHOW IC1 Quit the SHOW command by clicking the stop sign icon. Redraw the screen, e.g. with F2 and press the up-arrow and down-arrow keys several times. As you can see, you can scroll through the list of the recently used commands. As soon as the desired command appears in the command line press the Enter key.

Completing the Schematic

Use the ADD command to add the remaining components and the symbols for +5V, V+, and GND from supply1.lbr (search pattern: supply). Supply symbols represent the power signals in your schematic and cause the ERC (Electrical Rule Check)to use special checks for them. Remember that you can use the MOVE command to move objects around and that you can rotate elements attached to the mouse with a right mouse click. Using the NET command, connect the pins of the components according to the schematic and connect the supply symbols to the related pins. Use the right mouse button to alternate between the orthogonal and diagonal modes while using the NET command. Use to fix a segment. If you place a net exactly on a connection point, the net is terminated at this location. Otherwise the net keeps following the mouse.
The SMASH Command You will notice that when you rotate diodes and resistors from the horizontal to the vertical position, their reference designators and value texts rotate with the part. EAGLE provides a SMASH command that allows you to MOVE and ROTATE the name and value texts independently of the symbol. While moving a smashed text EAGLE draws a line from the text to the parts origin to show where the text belongs to. To activate the command SMASH Locate the cursor on the diode symbol and. This separates the text from the symbol. Now click the MOVE icon, move the cursor to the name D1 for the diode, and. The text selection point is marked as a cross and resides, depending on the rotation, on the lower left or the upper right corner. The name is now attached to the cursor. It can be moved to a better location and rotated with the right mouse button. When you have rotated and relocated D1, to fix its location. If you want to change the size of name and value texts which have been separated from the part with the SMASH command, use the CHANGE SIZE command (click the CHANGE icon and select Size from the menu). SMASH may be used with groups. Keep the Shift key pressed while clicking an object or inside the group in order to unsmash all texts. They will appear at their original positions. The VALUE Command EAGLE allows you to define or to change the value elements like resistors or capacitors. In the case of ICs the value informs you about the element type (e.g. 74LS00N). VALUE the resistor, type the new value, 2.2k, OK, and the new value is now displayed. You can use the NAME command to change the names of resistors, capacitors, ICs, nets and buses accordingly. You can change the net names but you dont have to, unless you want to get a descriptive netlist.

EAGLE-Tutorial Version 4.Automatic Forward&Back Annotation
You should always design your boards using Forward&Back Annotation controls; only then can you be sure that boards and schematics will be consistent with each other. This control mechanism is activated when you load a schematic and a board which have the same name and which are consistent with each other. EAGLE always loads both files if they exist in the same directory. Consistent in this context implies that the netlist, components, and values are identical. If you load a schematic and a board which has the same name and which can be found in the same directory (or vice versa), EAGLE launches a consistency check. You have the chance to start an ERC if any differences are found. The results are displayed in a text editor window. They enable you to fix the inconsistencies manually. Using this method it is possible to draw a consistent schematic for an existing layout. The Forward&Back Annotation will be cancelled if either only the schematic window or only the board window is activated. Any changes made can then lead to discrepancies in the files for the board and the schematic. Therefore always make follow this rule: When working on a board, never close the schematic window (you can minimize it to an icon, however) and vice versa. EAGLE generates warnings before operations are carried out which would terminate the Forward&Back Annotation. Under the control of the Forward&Back Annotation any change in the schematic results in an equivalent change of the board, and vice versa. Some changes can be made either in the board or in the schematic (e.g. naming components, nets, etc.). Others are possible only in the schematic (e.g. adding components). EAGLE prevents such operations in the board and prompts you to use the Schematic Editor. To monitor the Forward&Back Annotation load the demo2.sch file. The board demo2.brd will be loaded automatically into the Layout Editor. Now size both of the windows so that you can see them both on the screen. Change some names and values with the NAME and VALUE commands. You will notice that the names and values change in both windows. Experiment also with the DELETE command and remember the UNDO and REDO commands.
EAGLE-Tutorial Version 4.Designing a PC Board
In this section you will create a small PCB design and modify an existing design using the Layout Editor. First, you will create a board without a schematic. This section is useful mainly for those users who have no Schematic Module. If you have the Schematic Module you would normally not have to deal with the steps described in the following section. You should, however, read through this section as it deals with some generally useful points.

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.

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 DESCRIPTION command allows an info text about the package. This text and the package's name will be taken in consideration by the search function of the ADD command.

Resistor Symbol

Select the symbol editing mode, and enter the symbol name R in the New field. This name only has a meaning internal to the program, and does not appear in the schematic. 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. 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. See help function for further details. The NAME command allows you to name pins after they have been placed. The schematic symbol is drawn in layer 94 Symbols using WIRE and the other drawing commands. Place the texts >NAME and >VALUE in the layer 95 Names and 96 Values (TEXT command). Place them where the name and value of the component are to appear in the schematic. For fine adjustment choose a finer grid. This can be done while the TEXT command is active. Afterwards change the grid to default value 0.1 inch again.

Resistor Device

Create the new device R-10 with this icon. When you later use the ADD command to fetch the component into the schematic, you will select it by using this name. It is only a coincidence that in this case the name of the package and the name of the device are the same. To define devices that are available in several technologies and package variants you have to use wild cards in the device name to determine the position of these names. * represents the position of the technology name, ? the package name. Defining for example a device like a 7400 in two technologies (L, LS) the correct device name is 74*00. The name of the package variant will be
added at the end of the name automatically. If you wish to see the package variant's name, for example, at the beginning of the device name you have to use the ? like this: ?74*00. Click the New button on the right lower area of the Device Editor window to assign a package. For our example, please choose the package R-10. To allow further package variants click New again. The PREFIX command is used to specify a prefix for a name. The name itself will initially be automatically allocated in the schematic. For a resistor this would, naturally enough, be R. The resistors will then be identified as R1, R2, R3 etc. The names can be altered at any time with the NAME command. You can specify with the VALUE command whether the devices value can be altered in the schematic or in the board. Value must be On for resistors. For other devices it may be wise to set value Off. The previously defined resistor symbol is fetched into the device with the ADD command. If a device consists of several schematic symbols which can be placed independently of one another in the circuit (in EAGLE these are known as gates) then each gate is to be individually brought into the schematic with the ADD command. Set an addlevel of Next and a swaplevel of 0 in the parameter toolbar, and then place the gate near the origin. The swaplevel of a gate behaves very much like the swaplevel of a pin. The value of 0 means that the gate cannot be exchanged for another gate in the device. A value greater than 0 means that the gate can be swapped within the schematic for another gate in the same device and having the same swaplevel. The command required for this is GATESWAP. 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. If a device consists of several gates the element's name in the schematic will be expanded by the gate name. 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. With the CONNECT command you specify which pins are taken to which package pads. Click the Connect button now.