Stats

Locked Locked
Replies 2
Subscribers 165
Views 3902
Members are here 0

Netlisting error - part references across multiple instances of hierarchical blocks

FormerMember over 8 years ago

I'm having problems going from OrCAD Capture to Allegro, I think due to multiple instances of hierarchical blocks... initially I got thousands of errors of the type:

ERROR(ORCAP-36035): Multiple pin 1's which have different nets connected for C1: PowerConditioner, PAGE1 (2.70, 1.80).

Even though the design netlists just fine when I try to simulate the circuit. I think this is because, when sending the netlist to pspice, it prefixes all references with the reference of the hierarchical block it appears in. So it's fine that I have a capacitor referenced as C1 inside basically every block. I tried renaming one of my C1 capacitors and that particular one disappeared from the error log.

After some searching I tried Annotating my design with the "unconditional" option set. This re-referenced all my components so that they have unique names (up to C1000 etc) on the schematic pages. However, I still have multiple instances of a fair number of hierarchical blocks (many of them appear 32 times, nested inside other multiply-appearing hierarchical blocks). So, even though each of those hierarchical blocks has a unique path of reference designations, I still get 899 of these errors. But at least it's not thousands anymore.

There must be an option/checkbox somewhere that I can select so that Capture passes a sensibly-constructed reference designation for each part to Allegro, based on the reference designation of the blocks it appears in, just like it does for pspice... but I can't find it... could somebody help? Thanks!

oldmouldy over 8 years ago

PSpice is inherently hierarchical and physical layout of a PCB is not, not least because placing hierarchical part references wouldn't be too trivial. Since you have a lot of hierarchy, you will need to take a copy of the DSN file, use File>Open>Design, open the copy of the DSN file and set the project type to "Schematic". Once you have that, Tools>Annotate, set the "Action" to "Unconditional", the "Mode" to "Update Occurrences (Preferred)" and "Include non-primitive parts" to completely re-reference the design. Note that the PCB flow does not support any schematic parts that have underlying schematic definitions, schematic parts will need to be "Primitive = YES" for a PCB. Run a Design Rule Check for any remaining issues before netlisting.
Cancel
Vote Up 0 Vote Down

Cancel
FormerMember over 8 years ago

Thanks for the quick response, by the way - you didn't hear back because it worked!
Cancel
Vote Up 0 Vote Down

Cancel

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.