Stats

  • Locked Locked
  • Replies 4
  • Subscribers 166
  • Views 15773
  • 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

ORCAD Hierarchical subprojects.

SolderMonkey

Hi,

I'm trying to annotate & netlist a project that references other projects. I'm running OrCAD 16.6.

When creating a H-Block, the Place H-Block form is filled out like this example:

I have multiple H-Blocks in the top level each calling out a separate project. This is what the real project looks like:

It works. Subproject1.opj can be edited, annotated and netlisted as a separate project. I can descend from the top level into any of the hierarchical projects. I can synchronise Hierarchical ports between top level and the referenced opj.

However, there appear to be two issues:

1/ Annotating at the top level does not annotate the referenced projects. I can live with this.

2/ Netlist at the top level fails. This is what I need help with please.

Netlister says:

INFO(ORCAP-32002): Netlisting the design
INFO(ORCAP-32004): Design Name:
W:\HARDWARE\CADENCE\000 12G EXPANSION CONTROLLER 5000206A\5000206A.DSN
Netlist Directory:
W:\Hardware\Cadence\000 12G Expansion Controller 5000206A
Configuration File:
W:\Hardware\Cadence\SPB16_6\tools\capture\allegro.cfg

Spawning... "C:\Program Files\Cadence\SPB_16_6\tools\capture\pstswp.exe" -pst -d "W:\HARDWARE\CADENCE\000 12G EXPANSION CONTROLLER 5000206A\5000206A.DSN" -n "W:\Hardware\Cadence\000 12G Expansion Controller 5000206A" -c "W:\Hardware\Cadence\SPB16_6\tools\capture\allegro.cfg" -v 3 -l 31 -s "" -j "PCB Footprint" -hpath "HPathForCollision"
#1 ERROR(ORCAP-36023): Unable to find package for JBOD1: TOP, P01 TOP LEVEL (157.48, 96.52).
#2 ERROR(ORCAP-36023): Unable to find package for BPCONNECTOR1: TOP, P01 TOP LEVEL (73.66, 5.08).
#3 ERROR(ORCAP-36023): Unable to find package for CTRL_PWR_JBOD1: TOP, P01 TOP LEVEL (350.52, 5.08).
#4 ERROR(ORCAP-36023): Unable to find package for RAID_CONTROLLER1: TOP, P01 TOP LEVEL (157.48, 187.96).
#5 ERROR(ORCAP-36018): Aborting Netlisting... Please correct the above errors and retry.

Exiting... "C:\Program Files\Cadence\SPB_16_6\tools\capture\pstswp.exe" -pst -d "W:\HARDWARE\CADENCE\000 12G EXPANSION CONTROLLER 5000206A\5000206A.DSN" -n "W:\Hardware\Cadence\000 12G Expansion Controller 5000206A" -c "W:\Hardware\Cadence\SPB16_6\tools\capture\allegro.cfg" -v 3 -l 31 -s "" -j "PCB Footprint" -hpath "HPathForCollision"
INFO(ORCAP-32005): *** Done ***

Error ORCAP-36023 isn't listed in the user manuals. What package is the netlister looking for? How do I fix this netlisting error?

Thanks,

  • Which exact version of 16.6 are you running? (Check from Help>About in Capture) This certainly works with the last version of 16.6, 16.6-2015.s086 (Hotfix installation 16.6.s112). You should be able to Annotate the underlying blocks attached from other projects and create a netlist without issues. Your installation seems to be treating the H-blocks as components, check that you have the H-blocks to "Primitive = NO", or "DEFAULT", in the H-Block properties. If you have "DEFAULT" set, check that the Design Properties, available from a right-click on the DSN file entry in the Project Manager window, then Schematic Design tab, then Design Properties, Hierarchy tab and that H-Blocks have Primitive set to "No".

  • I'm running 16.6-S055 (v16-6-112EM) June 8 2015 13:04:08 and unless there's something wrong with my method it definitely doesn't work out of the box!

    I've attached a very simple example project, if you could verify that it's the software and not me, I'd be very grateful. I get the following error when I try to netlist:

    Spawning... "C:\Program Files\Cadence\SPB_16_6\tools\capture\pstswp.exe" -pst -d "C:\TESTSCHEM\TEST.DSN" -n "C:\TESTSCHEM\allegro" -c "C:\Program Files\Cadence\SPB_16_6\tools/capture/allegro.cfg" -v 3 -l 31 -s "" -j "PCB Footprint" -hpath "HPathForCollision"
    #1 ERROR(ORCAP-36023): Unable to find package for S1: SCHEMATIC1, PAGE1 (35.56, 25.40).
    #2 ERROR(ORCAP-36023): Unable to find package for S2: SCHEMATIC1, PAGE1 (66.04, 25.40).
    #3 ERROR(ORCAP-36018): Aborting Netlisting... Please correct the above errors and retry.

    The top level in the design is test.opj.TestSchem.zip

    Thanks,

    Mike Veal.

  • in reply to SolderMonkey

    The H-Block properties are incorrect. Hierarchy in Capture is joined by Schematic folder so "Implementation" needs to be the name of the Schematic folder that you want the block to reference in the design, in your sample, this is the default "Schematic1" for both blocks, The "Implementation Path" needs to be path and filename for the DSN file (OPJ is just a text file referencing the DSN file and project settings) - you can use .\ for a relative path to make things a bit more "portable". The "Implementation Type" needs to be "Schematic View". Then "everything" will hang together.

  • in reply to SolderMonkey

    OldMoldy, you sir are a gent.

    Yes that fixed it.

    Attached is the amended example project, here for perpetuity so that should anyone else have this issue they can dig up a working example.

    6813.TestSchem.zip

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.