Re: Access and CIS ORCAD configuration
I don't think your part numbers are being reduced. I think you probably also have an ID field in the database and this is being shown in CIS Explorer and confusing you.
Your Access database should have a "ID" field and it is best if this is set to "Autonumber" for the type. This will help to keep unique ID's for each record. Set this "ID" field as the Primary Key in the table. The CIS configuration wizard will display this field as "Counter" and will not have any problems with it.
Keep your existing "Part Number" field in the database (ie. W_N0000) in the various tables. In the CIS Configuration Wizard, for each table in your database, set the "Property Type" for this "Part Number" field to "Part_Number" and check the "Transfer to Design" box.
Now, to see the Orcad layout footprints in CIS explorer ("PCB Footprint" field), exit Capture CIS then:
1) Open "Capture.ini" in your CIS program folder (ie. C:\Cadence\PSD_14.2\tools\capture)
2) Look for the section labeled as "[Footprint Viewer Type]" and set the "Type" line below it to:
"Type=Layout"
3) Look for the section labeled as "[Layout Footprints]" and create "DirX" entries below it pointing to your footprint library paths. For example:
Dir0=C:\Cadence\PSD_14.2\tools\Layout_Plus\Library
Dir1=C:\Data\Cadence\Libraries\SFM\Main\Footprints
Note: Capture CIS will automatically look for PCB Footprints in all libraries located in the above directories.
Finally, to be able to see the schematic symbols in CIS Explorer, make sure you have added each symbol library to the Capture CIS search path:
1) Open a schematic page in Capture CIS
2) Hit the "P" button to place a component
3) Click "Add Library" and then add each library with symbols (referenced in your database).
4) Restart Capture CIS in order for CIS Explorer to start using the new libs