3.5 Preparing for orcad layout  (Page 7/9)

Next, I like to sort the spreadsheet so that it makes a little more sense. Highlight all of the rows and columns of your spreadsheet except the first row. Then select Data-->Sort… to bring up the Sort dialog.

I like to sort by Value and then by Part Reference . Once this is done, your parts should all be grouped by common value. For example, all of your 0.1uF capacitors should be next to each other. This will make it much easier to assign footprints and other properties to similar parts.

Fill in the remaining footprints based on the chart below. The reference designators in your schematics may vary slightly from those in the table, but this will make no difference to the design. Two things are important when you are assigning the footprints. First, make sure that you enclose the value in quotation marks or the importback into OrCAD won’t work. Second, make sure that the footprint name matches exactly the name that you gave your footprint in your library. If the name does not match, then you will get errors when you export your design to Layout.

Save the file in Excel. You will get several warnings about the incompatibility of the format. You can just ignore these. There is one small last step that we need to do before we can import back into OrCAD. Excel will replace one set of double quotes with three, so we need to open the file in a text editor. Use Notepad or another texteditor to open the file and do a search and replace to change """ with " . Save the file when you are done.

Now you can import the properties file back into OrCAD. In Capture, highlight the design file in the file view of the project explorer. Select Tools-->Import Properties… Browse to your properties file and click OK . You should not get any errors during the import. If you do, then there is likely a wrong footprint name or some missing quotation marks in the file. You will need to correct this before proceeding.

Embedding the bom in schematics

You may have noticed in Excel that some parts had some extra information. OrCAD is a great place to store information about where parts are bought, who makes them, how much they cost, etc. If all the information is there, then OrCAD can use the information to automatically generate the BOM (Bill of Materials). The BOM will helpyou be organized when ordering parts, and it is essential for the person assembling your board. There are several extra fields that you probably saw with this kind of information.

• Description – A description of the part. Usually I cut and paste this from the description of the part from the supplier’s web page (e.g. Digi-Key).
• ManPartNum – The manufacturer’s part number.
• Manufacturer – The manufacturer of the part.
• Notes – Any miscellaneous information about the part that you want to record. Maybe it has a long lead-time and you want to note that.
• PerUnitCost – How much each part costs.
• SupPartNum – The supplier’s part number (e.g. Digi-Key, Arrow, Newark, etc.).
• Supplier – The supplier of the part.