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.
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".
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.
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.