I'm having to migrate an OrCAD schematic that was originally layed out in OrCAD PCB to work with Allegro. I get the error
ERROR(ORCAP-36055): Illegal character in \ic (logic )\. when I try and netlist but I need help in tracking down the illegal characters. I've searched the footprint names and I've searched a netlist generated for PADS2K so what can I try next.
Check the part name and location in the design cache. OrCAD (and Allegro) don't like ().
In reply to steve:
How do I find which part has the problem?
PS design has 1156 parts in it.
In reply to Mr Opamps:
When you netlist check the session log. This should narrow down the part that has the issue.
Sadly the session log doesn't give any more info than my subject line. That would be too easy :(
Open the PSTXPRT.DAT netlist file and search for the string, spaces and braces will be the issue when the netlister process built the "device" field, the RefDes will be listed for the part(s), you will likely need to change the file location stored in the Design Cache for the affected part(s), this may be down to the original library location, OLB file, or that the parts have been edited locally in the design, DSN listed as the source. In the Project Manager window, open the Design Resources "+" icons so the the Design Cache items are visible, Replace the symbols in the Design Cache so that they are sourced from an acceptable library path, restricting the path to names with a-z, 0-9 and underscore characters is preferable.
In reply to oldmouldy:
I don't have a PSTXPRT.DAT file. How do i make one?
OK, sounds like you don't get that far with creating the netlist logic.
Open the design
From the menu, Window and take the OPJ entry for your design.
The Project Window has File and Hierarchy tabs, select the File tab.
Open the "+" if required for the DSN entry, this will list the Schmatic Folder(s) and Design Cache.
Open the "+" for the Design Cache.
In the Design Cache you will see the Symbol name and File location, the File Location will contain the \ic (logic)\ as part of the Path.
You will need to select the entry and use right-click>Replace Cache to replace the existing part with one from an acceptable library path - basically a path that does not contain illegal characters.
Aha, so just because it's a legal Windows path doesn't mean that Capture will accepts it.
I'm getting proper error messages now, but this is turning into a nightmare because Allegro throws out duplicate pin names and missing pin numbers :(