3.6 Starting layout in orcad  (Page 9/9)

Documenting the design

Good documentation of your design will help both in manufacturing and debug. First, we can add some useful text to the board. For example, the MAX603 part has a maximum input voltage of 11.5V, so maybe we want to put some text on the board to indicate that. You can use the Text Tool to create new text. Right-click anywhere in the design and select New… to get the Text Edit dialog.

Most text you create will be Free . For good readability, I suggest a Line Width of 8 and a Text Height of 75. A 6 mil Line Width is about as small as you can go to keep the text readable.

There are a few other things we can place on the silkscreen to document our board. One very useful thing is to label the pins on the programming header for the PLD. This will make it easier to hook up the programmer.

It is also useful to label the IO header pins with the pin numbers of the PLD that connect to it. You can also remove the pin numbers of the connector itself to avoid confusion.

It is also customary to add a logo and some information about the board, as well as the initials of the person who designed it. First, let’s add a logo for Rice University. Using the Component Tool , right-click and select New… Give this new component a reference designator of OWL1 . The Footprint should be RICELOGO from your library. The logo will actually be in the metal layer, so place it somewhere where it will not interfere with any traces or pads. When placed, open the Edit Component dialog from the components spreadsheet and check the Fixed , Non-Electric and Locked boxes, uncheck the Route Enabled box. When you next save your design you will be asked to back annotate since you just added a new component.

Next, we will add the some information about the board. You will use the Text Tool , but place this information on the TOP layer instead of silkscreen ( SSTOP ).

We also need to add a few things to the Drill Drawing layer. It is customary to provide board dimensions and engineering contact information on this layer. Make the Drill Drawing layer visible if it is not already. First move the drill chart to the right of the board by selecting ToolàDrill ChartàMove Drill Chart from the menu. Next, add dimension lines using ToolàDimensionàNew. Your board should measure exactly 3000 mils by 2000 mils. Now use the Text Tool to add some text with your name, phone number and email beneath the drill chart. When you are done everything should look like this.

For the final documentation steps, you will need to turn on some of the other layers. Make sure that all of the following layers are visible: TOP , BOT , GND , PWR , SMT , SMB , SST , DRD . You are going to add some text to each layer (outside the boundary of the board) to indicate what layer this is. This is necessary because you will make a separate Gerber file for each layer and you will need to be able to tell which layer you are viewing. Using the Text Tool put the following text on each layer above the board and aligned with the left edge:

Finally, we need to add some cut lines to mark the board outline on the TOP and silkscreen ( SST ) layers. The board shop will use these cut lines to route out the board from a larger panel. Click View Spreadsheet and then Obstacles to open the obstacles spreadsheet. Find your board outline. It will be the only one with the obstacle type of Board outline . Press CTRL-C twice to create two copies of the board outline. Double-click one to open the Edit Obstacle dialog. Change the Obstacle Type to Detail , Width to 10 and the Obstacle Layer to TOP . Do the same with the other one, but place it on the SSTOP layer.

Your design is now complete and you are ready to generate Gerber files for fabrication. Before proceeding, you will want to run the DRC again to check for errors. Once all errors are resolved, you can proceed to the next step. The Rice logo will generate some errors that can be ignored.

Creating gerber files

So, you’ve finished your design and you are ready to send off the Gerber files for fabrication. Creating the Gerber files is quite easy. First, select Options-->Post Process Settings… You already set these when you made your board template, but just check to make sure that the following Plot output File Names are Batch Enabled : *.TOP , *.BOT , *.GND , *.PWR , *.SMT , *.SMB , *.SST , and *.DRD . Also verify that each output file’s Device is EXTENDED GERBER . If everything looks OK, then select Auto-->Run Post Processor from the menu. You will get a series of dialog boxes, just click OK, and then you will see a lis file in Notepad with a report of the processing. At the very bottom of the file, it should say No warnings or errors . That’s it. Your Gerber files have been made. If you look in your board directory, you will see the files with the extensions listed above, plus a few others.

Viewing the gerber files

Before submitting your Gerber files for fabrication, it is best to look at them in a Gerber viewer. You will often catch mistakes there that you don’t see in layout. OrCAD has a built in Gerber viewer and editor called GerbTool. This is actually a very powerful program that you can use to edit the Gerber files, but you will just use it to look at them for now. In the main Layout window select Tools-->GerbTool-->Open… In your board directory there should be a file called Elec424Tutorial.gtd . Find this file and open it. You should see your design in GerbTool.

As noted before, GerbTool can do many different things with your design. However, the only thing that concerns you here is inspecting your Gerber files. The buttons on the right side of the screen control which layers are visible. Use them to inspect each layer individually. Once you are satisfied that each layer looks in order, close GerbTool. You do not need to save any changes when prompted.