Home > Community > Forums > PCB Design > Subcircuit Newbie question


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Subcircuit Newbie question 

Last post Thu, Feb 11 2010 11:36 PM by ACENGR. 2 replies.
Started by ACENGR 10 Feb 2010 10:45 PM. Topic has 2 replies and 3242 views
Page 1 of 1 (3 items)
Sort Posts:
  • Wed, Feb 10 2010 10:45 PM

    • ACENGR
    • Not Ranked
    • Joined on Wed, Feb 10 2010
    • Posts 2
    • Points 25
    Subcircuit Newbie question Reply

     I am having a problem implementing a subcircuit. Everytime I run the simulation I get the following warning:

    "WARNING [NET0093]   No PSpiceTemplate for TRANSORB, ignoring" 

    The subcircuit I would like to implement is a circuit for a transorb that I found here: 


    The steps I followed to implement the subcircuit are the following:

    1)  Created an Hierarchical block and named it TRANSORB (the same name as the subcircuit found on the above link) and added it to my circuit.

    2) Created two Hierarchical bidirectional ports and labeled them Anode1 and Anode2 to corespond to the nodes names described in the nodelist of the subcircuit. Also gave them sequence properties of 1 and 2 repectively and connected TRANSORB to the rest of my circuit.

    3) Tried to create subcircuit netlist as it says in the cadence instructions by going to Pspice -> create netlist (didn't see a create subcircuit netlist option like it says in the instructions) then I cut and pasted the subcircuit code from the link above at the beginning of the netlist for the rest of the circuit (before all of the other netlist code) and ran the simulation when I got the error. I know their is something I am not doing correctly and I am hoping someone can help.

     Thanks in advance.

    • Post Points: 20
  • Thu, Feb 11 2010 3:33 PM

    • oldmouldy
    • Top 10 Contributor
    • Joined on Tue, Jul 15 2008
    • Woking, Surrey
    • Posts 1,445
    • Points 24,590
    Re: Subcircuit Newbie question Reply

    OK, thinkgs have become a little confused here. First off the model text, this is the subcircuit definition, tidied up version below:

     * Transorb Model from Cadence Website
    * Parameters:
    * IRM maximum leakage current VCL max maximum clamping voltage
    * VBR nom nominal breakdown voltage Ipp max peak pulse current
    * VBR max maximum breakdown voltage Cjof zero bias capacitance
    * IR Test current @ VBRnom ISBF saturation current to fit capacitance
    * NBF emission coefficient to fit capacitance
    + IRM=5u VBRnom=19 VBRmax=13 IR=1m
    + VCLmax=27.7 Ipp=54.2 Cjof=1200p
    + ISBF=1f NBF=1
    Drev1 A_int1 Cathode TRANSR
    Dfwd1 Anode1 Cathode TRANSBF
    Dr1 A_int1 Anode1 DTRANS
    Drev2 A_int2 Cathode TRANSR
    Dfwd2 Anode2 Cathode TRANSBF
    Dr2 A_int2 Anode2 DTRANS
    ***** REVERSE BEHAVIOUR *****
    + IS={IRM/2} RS={(VCLmax-VBRmax)/Ipp}
    + BV={VBRnom} IBV={IR}
    + IKF=1000 Cjo=1p M=.3333 VJ=.6
    + ISR=1p TT=1u )
    + IS={ISBF} N={NBF} RS=1u IKF=1000
    + Cjo={Cjof} M=.3333 VJ=.6 ISR=1p
    + BV=1000 IBV=100u TT=1u )
    + IS=1n N=.01 RS=1u IKF=1000 Cjo=1p
    + M=.3333 VJ=.6 ISR=1p BV=1000 IBV=100u
    + TT=1u )

    Copy this text into the Model Editor. Start the Model Editor from the PSpice Accessories program group with the mail program group. Use File>New, then Model>New to get a new model going, pick a diode and give it a name, any will do since this will only be transient data. When the model is created, use View>Edit Model to get the model text displayed, select all the text and delete it, then paste in the Transorb model text, save the data, you will be prompted for a new file name / location for the LIB file. Use File>Export to Capture Part Library, this will create a "black box" for the part that you can place in the schematic - you can edit the graphic later but the symbol will be fine for testing. Exit the Model Editor.

    In the schematic, place the part just created after adding the OLB file. Then Edit the Simulation Profile, PSpice>Edit Simulation Profile, Configuration files tab, select Library on the left, use the Upper Browse button to browse to the LIB file saved from the Model Editor and use the Add to Design button to add the LIB file to you design for simulation. Configure any other simulation parameters and close the simulation profile. Complete the circuit and run the simulation.

    Using SPICE text models is also covered in Appendix C of the PSpice Users Guide, pspug.pdf in the doc\pspug directory of teh installation.

    • Post Points: 20
  • Thu, Feb 11 2010 11:36 PM

    • ACENGR
    • Not Ranked
    • Joined on Wed, Feb 10 2010
    • Posts 2
    • Points 25
    Re: Subcircuit Newbie question Reply


     You are the best! Your instructions were clear, consise and accurate. I had no problems implementing this solution. Thanks so much.



    • Post Points: 5
Page 1 of 1 (3 items)
Sort Posts:
Started by ACENGR at 10 Feb 2010 10:45 PM. Topic has 2 replies.