3.5 Preparing for orcad layout  (Page 8/9)

Export the properties of your design again and fill in the information for each part. To help you, I have put an Excel version of the BOM in the following location on Owlnet.

/home/jpfrantz/elec424/tutorial/assy/BOM.xls

When you have finished editing the properties, save the file and import them into Capture just like you did for the footprints.

Now you are ready to have OrCAD generate a BOM for you. To do this, highlight the design file in the file view of the project explorer. Select Tools--> Bill of Materials… to bring up the Bill of Materials dialog.

You will want to change a few of the default settings. Cut and paste the following text into the Header and Combined Property String fields of the dialog box.

Item\tQuantity\tReference\tPart\tDescription\tSupplier\tSupPartNum\tManufacturer\tManPartNum\tUnitCost\tNotes

{Item}\t{Quantity}\t{Reference}\t{Value}\t{Description}\t{Supplier}\t{SupPartNum}\t{Manufacturer}\t{ManPartNum}\t{PerUnitCost}\t{Notes}

Then click OK to generate the file. This should put a file called Elec424Tutorial.bom in your sch directory. This will be a tab-delimited file just like when you exported the design properties. You can use Excel or another program to make it look a little more readable. Do thisand put the finished version into the assy directory. This is one of the files that you will give to the assembler when you are ready to have your boards assembled.

Creating a board template file

You are almost ready to export your schematic design to Layout. Before doing this, we must create a board template file. This file defines some default properties for the board that will be used throughout layout. To create a template, start Layout and select File-->New . When you see the dialog, press Cancel . You should now see a blank workspace. You can use the same shortcut keys that you used in Capture to zoom and center the design (‘ I ’, ‘ O ’, and ‘ C ’).

The first thing we need to do is draw a board outline to define the perimeter of the board. For this PCB, we will make the board 3 inches by 2 inches. The board outline is an obstacle like the ones you placed in the footprint editor. To create the board outline, select the Obstacle Tool , right-click and choose New… and then right-click again and select Properties… Name the obstacle BOARD_OUTLINE , its type should be Board Outline , its Width should be 50 (mils) and it should be placed on the Global Layer . Place the first corner of the board at 0,0 and then draw from there. While drawing, you can use the information in the status bar to tell you where in the workspace you are. When finished, your board outline should look likethis.

Next, you will edit the layer stackup. Layout has spreadsheets just like the Library Manager does. Click the View Spreadsheet icon and select Layers . This spreadsheet defines all the layers that your board uses and their respective functions in the design. You will see a spreadsheet that looks something like this.

You are making a 4-layer board, so we will turn off some of the pre-defined layers because we will not use them. Double-click the INNER1 layer to bring up the Edit Layer dialog.