PCB Design Tech Tips

I changed some of the footprints in OrCAD^® Capture, but when I read the new netlist into the .max file, the footprints didn't change.

You need to use AutoECO/Override Attributes to change the footprints in OrCAD Layout. The regular AutoECO will not change component, net properties or footprints. It is important to backannotate from OrCAD Layout to OrCAD Capture before running AutoECO/Override Attributes.

To backannotate:
1) From the Auto menu in OrCAD Layout, select Backannotate. This creates a swap file with the .swp extension.
2) To keep the OrCAD Layout .max file synchronized with your schematic, OrCAD Layout prompts you to save your file.
3) Launch OrCAD Capture and open your schematic.
4) In the Project Manager, highlight the .dsn file.
5) From the Tools menu, select Backannotate.
6) From the OrCAD Layout tab in the Backannotation File text box, select the correct path and filename to the .swp file you created in step 1, and click OK.
7) Make any necessary changes to the schematic.
8) Create a new netlist in OrCAD Capture. From the Tools menu, select Create Netlist.
9) Select the OrCAD Layout tab, and confirm the correct path and .mnl filename are in the Netlist File text box. Click OK to create the netlist.

To run AutoECO:
1) In the Layout session frame from the Tools menu, point to ECOs and select AutoECO/Override Attrs. The AutoECO utility launches.
2) In the File A dialog box, select the original .max file and click OK.
3) In the File B dialog box, select the new .mnl file and click OK.
4) In the Output Report dialog box, select an appropriate .lis filename and click OK. The .mnl and .max files are merged.
5) In the Merged Output Binary dialog box, enter your .max filename and click OK.
6) Open the new .max file to view changes.

Return to EMA Currents eNewsletter

How do I configure a basic database with OrCAD Capture CIS?

1) Create a database with columns containing Part Number, Value, Schematic Symbol, Part Type and other optional fields like Footprint, Datasheet, Electrical Parameters, etc.
2) From your system Control Panel, create a new data source name using ODBC setup, and point this data source to your database.
3) From the CIS Configuration option in OrCAD Capture CIS, select the data source name and configure a .dbc file.
4) To display schematic symbols in the OrCAD Capture CIS Explorer window, the corresponding library location should be present under Part Library Directories in your capture.ini file.
5) To view footprints in OrCAD Capture CIS Explorer, the viewer type Allegro^® or OrCAD Layout and the footprint library location should be entered in Allegro Footprints or OrCAD Layout Footprints section in the capture.ini file.

Return to EMA Currents eNewsletter

Are there certain symbols I should avoid using in OrCAD PCB Editor?

Usage of the following characters in <name>: PART_NAME, <source package>, <design name>, <schematic name>, or
<hierarchal block name> will cause problems during OrCAD Capture-PCB Editor flow:

~ ` ! * ( ) _ + = | \ } ] { [ : ; “ ‘ < > . ?

As a good practice, avoid using the above characters in the property VALUE.

The following characters are invalid in the property VALUE:

( ) @ :

All extended character sets plus the following are invalid characters for pin
names:

/ ; ! < > : \ “ , *

A pin name must be alphanumeric, but you can have numbers as pin names
for scalar pins. The other characters that are supported in flow for pin names are:

- # $ % + = | ? ^ _ . ( )

Return to EMA Currents eNewsletter

Why must I used a special ground with PSpice A/D?

All nodes on the circuit must have a DC path to ground. For PSpice^® , Node 0 is the only ground. Typically, this is done by using the ground symbol 0/SOURCE from the Source.olb library in your design. Other ground symbols merely name the net with the symbol’s name. With no DC path to ground, PSpice will report one of the following error messages:

Node is floating
Less than two connections at node

With 15.7 the Node 0 ground symbol is included in the Capsym library within
OrCAD Capture library.

Return to EMA Currents eNewsletter