Stats

  • Locked Locked
  • Replies 6
  • Subscribers 167
  • Views 5766
  • 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

Allegro 15.2 - Importing Logic - 'name too long' error

archive

Have taken on a job from a new customer who passed on all design files including ConceptHDL schematic including lib archive etc. and Allegro PCB file.

I can open, view and edit the schematic with no problems - all symbols present. I can package the design (Export physical).

The problems arise when I try to import the logic into Allegro. I just get a pile of errors reported.

 I always thought that long names were truncated automatically - or was that something else altogether? Please can anyone assist?

 Here is a snippet from the netrev.lst log file

Using Design Entry HDL & PCB Editor 15.2 running on Vista Business.

Thanks

Rob

#1   ERROR(302) Device library error detected.

Problems with the name of device 'STANDARD_FERRITE_SMT-1500R[100MHZ],0.40,0.5,MULTIA': 'name too long'.

Device 'STANDARD_FERRITE_SMT-1500R[100M' has library errors. Unable to transfer to Allegro.

#2   ERROR(302) Device library error detected.

Problems with the name of device 'SINGLERESISTOR_0402-220K,1%,63MW': 'name too long'.

Device 'SINGLERESISTOR_0402-220K,1%,63M' has library errors. Unable to transfer to Allegro.

#3   ERROR(302) Device library error detected.

Problems with the name of device 'POLAR_CAPACITOR_RADIAL-ELECT,100UF,6.3MMX7MM,10V,A': 'name too long'.

Device 'POLAR_CAPACITOR_RADIAL-ELECT,10' has library errors. Unable to transfer to Allegro.

#4   ERROR(302) Device library error detected.

Problems with the name of device 'MOSFET_PCHANNEL_SOT23-1R3,0.18A,60V,NDS0605': 'name too long'.

 

  • malcs

    Rob,

     Create a system variable ALLEGRO_LONG_PACKAGE_NAME and give it the value TRUE.

     Cheers,

    M.

  • archive

    That cracked it!!

     What can I say? Malcs, you are a star.

     Thanks a lot.

     Rob

     

  • Pieman

     I have just moved to Windows 7 and am having that same issue.  At first it would not even try to create a netlist, then I saw a thread that said I had to launch Orcad Design Entry as an Administrator (RM on Orcad Design Entry then choose - Run as Administrator).

     When I try to create a netlist with the configuration Device/Net/Pin/Name Char Limit set to anything above 31 I get the "Name too long" error.  I have tried to set a system variable as follows without success:

    set ALLEGRO_LONG_PACKAGE_NAME = TRUE

    set ALLEGRO_LONG_PACKAGE_NAME TRUE

     

    I must not have the correct syntax.

     

    Please help if you can.

    My email is mlaw@cardaccess-inc.com

     

    Thank you.

    Marvin Law

  • fxffxf

     The env variable, ALLEGRO_LONG_PACKAGE_NAME, onlyapplies to 15.x releases. Starting with 16.0 the variable, ALLEGRO_LONG_NAME_SIZE, is used to set the design name length used when for new designs (including symbols and padstacks).

         set  ALLEGRO_LONG_NAME_SIZE = 255

    Depending on your manufacturing processes, you may wish to use a smaller value then 255.

    For existing designs, you can changed the length by picking Menu Setup-> Design Parameters (or prmed cmd), selecting the Design tab and changing the "Long Name Size" value.

  • Sachin Tiwari

      Rob,

     I am getting a error "Unable to find pinname in adfncpin"

    I found that this might be because of the number of characters in pin name. Let me know how i can change the character length, whose default value seems to be 31 (not sure).

    I am guessing that by chaging this default value to 255 can make it work.

     Similar to what you had done before. Creating a system variable ALLEGRO_LONG_PIN_NAME and give it the value TRUE

     I am not sure how to do it. Kindly let me know the steps to create this variable. Meanwhile I am using cadence 15.7 version.

     Regards

    Sachin

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.