Stats

  • Locked Locked
  • Replies 9
  • Subscribers 165
  • Views 18551
  • 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

how to simulate time varying capacitance in Orcad ?

reddytinku

 Hi

I have a circuit which has piece-wise time varying period capacitance- how to simulate this type of circuit in OrCAD?

Thank You

  • Use a Voltage controlled Capacitor, VC_CAP, and drive it with a VPWL.

  •  hi thanks for the reply

    i looked in to VC_CAP and VPWL. I have one more doubt, VPWL has input for only 8 time instances , how to increase these and howto make it as a periodic source ? what wil be the VPWL value after T8 th time ?

     

    http://postimage.org/image/8nwx1k3vf/

     

    Thank You

  • VPWL uses linear interpolation between the specified points, the "T8" value will remain till the end of the simulation,. If you need more points, use a VPWL_FILE source, this takes time / value tab demilited pairs from a file. There probably is some limit to the number of points but it must be large. Take care with manually edited data that time remains "monotonic", always going forwards, the simulator is going to baulk at trying to reverse time! You can get an idea of the required format by exporting results from the Probe window, select / display a single waveform in the Probe window, from the menu, Edit>Copy, open a text editor and Edit>Paste into the text editor, the text values for the points in the waveform will be pasted as text.

  •  thanks :)

    got the concept. can we enter the time and voltage values in a simple text document or do we need to use any text editor ? how to upload this file to the VPWL_FILE source ? I tried through property editor of it, bt couldnt able to do it

    And my Orcad doesnt has Spice_elem library(which has VAR_CAP) so I downloaded the library and added to the Orcad capture, so when I started to run the circuit I am getting an  error  ''ERROR(ORPSIM-15108): Subcircuit AWBVC_CAP used by X_U1 is undefined '', how to over come this ?

    Thank you very much for your time, pease forgive me if I am troubling you.

     

  • Any editor that makes "plain" as apposed to "formatted" test will work, like Notepad, NOT Word. VPWL_FILE has a File property, this takes the full path and file name for the pwl file created, you can use .\pwlfile.txt to use a file called pwlfile.txt in the current directory.

    It sounds like you have the graphical library, OLB, for the spice_elem, you need the simulation library, LIB, and then add it to the Simulation Profile libraries so that the simualtor can find it.

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.