Home
  • Products
  • Solutions
  • Support
  • Company
  • Products
  • Solutions
  • Support
  • Company
Community PCB Design PSpice UC1825 Unencrypted TINA-TI Transient Spice Model

Stats

  • State Suggested Answer
  • Replies 4
  • Answers 1
  • Subscribers 13
  • Views 298
  • Members are here 0
More Content

UC1825 Unencrypted TINA-TI Transient Spice Model

mmartin2
mmartin2 16 days ago

I'm using Cadence Allegro Design Entry CIS 17.4-2019 S035.

I downloaded the UC1825 Unencrypted TINA-TI Transient Spice Model library file from Texas Instruments website.

I created a .OLB file from it and imported it into my simulation schematic.

I receive the following errors when I attempt to run pspice simulation.

Reading and checking circuit

ERROR(ORPSIM-16362): Name on .ENDS does not match .SUBCKT

ERROR(ORPSIM-15461): Incorrect number of interface nodes for X_U53.XU8.XU5.

ERROR(ORPSIM-15461): Incorrect number of interface nodes for X_U53.XU1.XU1.

Circuit has errors ... run aborted

See output file for details

INFO(ORPROBE-3188): Simulation aborted

I cannot determine where the syntax error is. Everything appears fine when i look at the .LIB file.

  • Reply
  • Cancel
  • Cancel
  • TechiEE12
    0 TechiEE12 15 days ago

    I found this article on support.cadence.com which might help

    ERROR(ORPSIM-16362): Missing .ENDS in SUBCKT (cadence.com) 

    • Cancel
    • Up 0 Down
    • Reply
    • Verify Answer
    • Cancel
  • retiredEE
    0 retiredEE 15 days ago

    In the UC1825 library there is a subcircuit named COMPARATOR_3 whose name doesn't match the name given in the .ENDS command.  That name is COMP_BASIC_GEN but should be COMPARATOR_3. The other two errors involve the passing of a local subcircuit node into another subcircuit which uses this node only in a VALUE expression.  See DPST_SWITCH_0 called from RC_CLK_0 and SPDT_SWITCH_0 called from ERRAMP_0.  I'm not sure this is valid.  See the section in your PSPice User guide "Net names and device names in ABM expressions".

    • Cancel
    • Up 0 Down
    • Reply
    • Verify Answer
    • Cancel
  • retiredEE
    0 retiredEE 6 days ago in reply to retiredEE

    I've been obsessed with this problem since the syntax at first glance seems normal.  However, a closer look at subcircuits DPST_SWITCH_0 and SPDT_SWITCH_0 reveals their PARAMS: keyword has a space between M and : which causes PARAM to be interpreted as a node.  This results in the "Incorrect number of interface nodes" errors.

    • Cancel
    • Up 0 Down
    • Reply
    • Verify Answer
    • Reject Answer
    • Cancel
  • mmartin2
    0 mmartin2 4 days ago in reply to retiredEE

    Thank you for catching those syntax errors. I removed many other spaces in PARAM. There were also many other spaces removed after .subckt <name>. I also found the D_D10 and D_D11 in .SUBCKT DFFSBRB_SHPBASIC_GEN had incorrect syntax. I'm able to get my simulation running after fixing all of these errors. However, now it appears there is no closed loop regulated control. 

    • Cancel
    • Up 0 Down
    • Reply
    • Verify Answer
    • 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.

© 2023 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information