Stats

  • Locked Locked
  • Replies 2
  • Subscribers 167
  • Views 11515
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

ERROR(ORCAP-36071): Illegal character "Dot(.)" found in "PCB Footprint" property for component instance.........

MichaelV

So I open an existing .dsn in OrCAD Capture version 16.5 and proceed to make a PCB out of it. The OrCAD on my computer was a recent installation. The project and schematic are from 2 years ago.

Annotation seems to work:

INFO(ORCAP-1378): LAST USED REFERENCES [blah blah blah component references....]

INFO(ORCAP-1379): Done updating part references

Design Rules Check gives only a couple trivial warnings:

Checking Electrical Rules
WARNING(ORCAP-1829): Possible pin type conflict blah blah blah

Checking For Single Node Nets

Checking For Unconnected Bus Nets
WARNING(ORCAP-1595): Two wires/busses of different nets intersect visually, yet nets are not connected blah blah blah

Unfortunately, Create Netlist... produces about 80 of the following errors in the netlist.LOG:

Illegal character "Dot(.)" found in "PCB Footprint" property for component instance............................

Illegal character "Forward Slash(/)" found in "PCB Footprint" property for component instance..............................

Property "PCB Footprint" missing from instance.............................

Pin number missing from Pin "1" of Package..................................

#87 Info: PCB Editor does not support Dots(.), Forward Slash(/) and White space in footprint names. The supported characters include Alphabets, Numerics, Underscore(_) and Hyphen(-).

If I select all components in the schematic and look at Properties... the PCB Footprint column cells typically have content like this: RAD/.200X.100/LS.100/.031 or are blank. So, this is an example of the '.' and '/' that the netlist generator doesn't like.

Library Verification/Correction doesn't seem to do anything.

I can't Back Annotate because I don't seem to have any .SWP that it wants.

If I look at the properties of a component in the schematic OrCAD typically tells me ERROR(ORCAP-1733): Allegro footprint AX/.400X.100/.034 was not found in the search path.

If I go and Place Part, the design cache and DISCRETE.OLB libraries open. If I select a part from the DISCRETE library that doesn't exist in my design and place it and Edit Properties... the PCB Footprint is always blank, no matter what part or from what built-in library. And these are the built-in Cadence libraries and parts, NOT something I created myself. So how come Cadence removed the PCB footprints from all parts and rendered their product useless?

If I fill in the PCB Footprint cells with something acceptable to the netlist, OrCAD will go ahead and create a .brd file, but what Allegro shows is just empty space. If I try to Place parts, it complains it can't find the footprint specified in the Properties.

OK what am I doing wrong here?

  • redwire

    The error messages are very clear.  You need to correct the footprint names and not use "." and "/" in the name.   And of course, all parts will need a footprint name assigned to them.  Make sure that you have a matching footprint symbol in your PCB symbol path (PSMPATH).

  • oldmouldy
    It looks like you have footprint names for the old OrCAD Layout tool, this used a format of footprint library name and dimensions and the convention use is not compatible with the PCB Editor (Allegro) naming conventions. In terms of the Discrete schematic library, this is a generic reference library of discrete parts, is you place a part like a resistor, capacitor or transistor from that library, how could a footprint possibly be assigned? Any of those parts could potentially have a dozen, or more, alternatives for a given value.
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.