3.5 Preparing for orcad layout  (Page 5/9)

You are not quite done with the footprint even though all the pins are placed. There are just a few things left to do. First, we need to define a place outline. A place outline is a mechanical boundary that Layout uses to keep parts from hitting each other once assembled. In this case, the part outline is easy to draw. The physicalswitch does not extend beyond the square defined by the pads, so we will just draw a box around them. To do this we use the Obstacle Tool .

Give the obstacle a meaningful name. Select Place Outline as the Obstacle Type . The width in this case is arbitrary. The layer is very important. This part is a thru-hole part, so in this case we want to make sure that surface mount parts on the bottom side of the board will not interfere with this part.By choosing Global Layer , the place outline will extend through every layer of the board. If this were a surface mount part, we could put the place outline on the top layer only. Click OK when you are done making changes. Now you need to draw the outline. Left-click to place each corner. When you have drawn at least 3 corners, you can press ‘ F ’ to have OrCAD finish the outline for you. It should look like this.

There is just one last thing you need to do to make your footprint complete. It is often nice to have an outline of the part on the silkscreen layer. This is not necessary, but it is a nice touch and makes things a bit easier during assembly of your board. We can easily make this outline by copying the place outline in the obstaclesspreadsheet. Open the obstacle spreadsheet and copy the place outline by highlighting it and pressing CTRL-C just like you did for copying a pin. Double-click the new obstacle to bring up the Edit Obstacle dialog. Give the obstacle a meaningful new name, change the type to Detail , and change the layer to SSTOP .

Congratulations! You have created your first footprint.

I have provided a library of the remaining footprints for use in this design. Use the Add… button to add the library to the list of available libraries. Use the Save As button to copy each footprint into your own library. You can find this library on Owlnet at:

/home/jpfrantz/elec424/tutorial/lib/tutorial.llb

Copy all of the parts from this library into your library.

Assigning footprints to parts

You will now switch back briefly to working in Capture. Open your tutorial schematics if they are not already open. You have defined a set of footprints to be used in your design, but now you must assign those footprints to each of the parts in your design. Each part in your schematics has a property called PCB Footprint and this must match one of the footprints in your footprint library. There are several ways to assign footprints to schematic symbols. One way is to open the Property Editor by double-clicking the part in schematics. This will show you all the properties for that part. Double click the pushbutton switch on the first page of your schematics. This is the part whose footprint you just drew.