Stats

  • Locked Locked
  • Replies 3
  • Subscribers 166
  • Views 16136
  • 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

Duplicate Name properties in hierarchical design, Capture 16.2

kspringer

 I recently updated to 16.2 capture.  I am trying to netlist a design that was done in 16.0

When I netlist, I get the  Error   [ALG0078] Identical Name property value  on two instances in the design.

This previously netlisted OK with 16.  I tried to change the name in the property editor, but changes of the name property don't seem to be allowed.  I assume these are generated by the tool. The Name property seems to be a truncated version of the instance name.

Is there a way to make the two instances unique?  Error log is attached.

 

Spawning... "C:\OrCAD\OrCAD_16.2\tools\capture\pstswp.exe" -pst -d "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\10g_iom_4pt.dsn" -n "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\allegro" -c "C:\OrCAD\OrCAD_16.2\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"
#1 Error   [ALG0078] Identical Name property value "10G_port_no_mux" found on Hierarchical block instances  10G_port_no_mux_p12: H02 - 10G Port, P01_XFP_PHY (5.40, 1.50) and  10G_port_no_mux_p3: H01 - Top Level, P30 - 10G Ports Asymmetric (3.20, 1.20). The value should be unique for correct netlisting.
#2 Error   [ALG0078] Identical Name property value "10G_port_no_mux" found on Hierarchical block instances  10G_port_no_mux_p12: H02 - 10G Port, P01_XFP_PHY (5.40, 1.50) and  10G_port_no_mux_p3: H01 - Top Level, P30 - 10G Ports Asymmetric (3.20, 1.20). The value should be unique for correct netlisting.
#3 Aborting Netlisting... Please correct the above errors and retry.

Exiting... "C:\OrCAD\OrCAD_16.2\tools\capture\pstswp.exe" -pst -d "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\10g_iom_4pt.dsn" -n "Z:\Hw_TITUS\IO_10GE_4pt_module\schematics\rev_08\allegro" -c "C:\OrCAD\OrCAD_16.2\tools\capture\allegro.cfg" -v 3 -j "PCB Footprint"

  • hpattie

    I searched sourcelink for ALG0078 and found the following:

    Error [ALG0078] Identical Name property value <property value>found on Hierarchical block instances <block instance> and <block instance>. The value should be unique for correct netlisting.

    This error appears in case the "Name" property value is identical for one or more instances of a hierarchical block referring to same schematic view. For example, if you have placed two instances of Halfadder block say H1 and H2 in your top level design, the Name property value should be unique for each of the instances say Name = HalfaddedI nst1 for H1 instance and Name = HalfaddedInst2 for H2 instance.

    In your case you have a block named 10G_port_no_mux on page 3 of your schematic, and an identically named block on page 12.

    Hierarchical block names must be unique. You will have to rename one of the blocks.

    I just tried an experiment on a hierarchical schematic and successfully renamed a block with the following proceedure;

    1. Left click to select the block.

    2. Right click and select edit properties.

    3. in column A, select the name field.

    4. Delete the existing name, and type a new name.

    5. Close the editor

    6. Save the page

    7. Save the schematic.

    Regards,

    Harold Pattie

    harold.pattie@ericsson.com

     

  • Khurana

     This error was fixed in the latest hotfix for OrCAD v16.2.  So, install the hotfix (download from downloads.cadence.com) then delete a hierarchical block and copy the existing one and the tool should auto-assign NAME property (it's system assigned).  Save, then netlist again.  Should work.

  • kspringer

     I loaded the hotfix.  I didn't want to delete the instance, since that would lose all the reference designators.

    I was able to rename the block on H02 and successfully netlist.  The trick was to rename at the top level, not the instances.

     Thanks for the suggestions.

    ..kent

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.