Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Need help with Pspice

  1. Apr 8, 2007 #1
    I need help plotting the VTC of a given circuit. I tried dividing the output signal by the input signal put that does not work. Is there a function I can use to achieve this? I'm using Orcade Capture Lite by the way.

    Thanks in advance.
    Last edited: Apr 8, 2007
  2. jcsd
  3. Apr 8, 2007 #2
    Are you you using actual pspice code or the OrCad GUI ?
  4. Apr 8, 2007 #3
    I'm using the GUI. They haven't really gone over the code in depth.
  5. Apr 9, 2007 #4
    Configure your simulation as either a DC or parametric sweep. After running the simulation you should be able to add a trace with the output node voltage divided by the input node voltage.
  6. Apr 9, 2007 #5
    Is it a single output variable or do I have to use an operator or analog function to divide the two signals? I can't find anything that resembles the VTC of this circuit. :confused:
  7. Apr 9, 2007 #6
    I have not done this specifically before but I might still be able to help you. I apologize if I am over-simplifying your problem.

    I am assuming that you are looking for a "Transfer Characteristic" for your circuit. I am also assuming that you have defined input and output nodes of your circuit. You just need to know which nodes you are interested in, they don't need to be labeled or anything.

    After you enter your circuit in Capture you need to set up a simulation profile. Since you are plotting a voltage vs voltage curve you are going to need to sweep a voltage source to collect data points.

    Make sure that the input node of you circuit has a VDC supply with the positive terminal connected to your input node and the negative terminal grounded. Configure your simulation to perform a DC sweep analysis through a range of values at specified intervals. Since it is your input voltage, the range of values will correspond to your desired X axis.

    You do not need any probes on your circuit.

    Run the simulation and it will bring up the PSPICE A/D window. You can then click on Trace > Add Trace. Narrow the results to voltages and select the output node. Enter a "/" to divide and then select the input voltage. When you add the trace you will have the input voltage on the X axis and the output voltage on the Y axis.

    If you are still having problems you will need to give me more detailed information.
  8. Apr 9, 2007 #7
    Thanks! I haven't tried it yet, but I will in a bit once I get some time.
  9. Apr 9, 2007 #8
    I just tried it, and I was able to plot the output vs. the input. Unfortunately the plot did not come out looking correct. It might be the circuit that's causing the problem. I won't be able to mess around with it until tomorrow but I'll see if I can get it looking right then.
  10. Apr 10, 2007 #9
    What type of circuit are you trying to model? You could post a screen capture of the circuit and the results if you like.
  11. Apr 10, 2007 #10
    Here's the circuit
    here's the output for vout/vin
    and vin/out

    It's just a regular BiCMOS logic inverter. I'm pretty sure the circuit is correct. I used the same parts that were suggested in the lab manual. i thought I'd also post what vin/vout looks like since it more resembles the VTC than the first plot.
    Last edited: Apr 10, 2007
  12. Apr 10, 2007 #11
    Was missing a 100k Resistor between the output and ground. I just tested it with the resistor and I'm still getting the same output plots. :confused:
  13. Apr 11, 2007 #12
    I am not familiar with that type of circuit. I was hoping someone with some more electronics experience would check it for accuracy.

    Are you sure that all of the circuit junctions are correct? Also, are the characteristics of the model components that you selected comparable to their real-world counterparts?

    It looks like your sweep simulation is properly configured so I would almost assume that the issue is with your circuit or the components.
  14. Apr 11, 2007 #13
    The lab manual mentions no need to change and of the model parameters. Well I appreciate your efforts in helping me.
  15. Apr 14, 2007 #14
    Two things:

    - Define Vout as Net Alias of the output node, run a DC Sweep with V5 as sweep variable, and add a trace of Vout

    - Looks like the curse of the p-MOS FET in Orcad haunts you. Looks like the source and drain terminals on M1 (the IRF9140 one) are swapped. Do a Mirror Vertically of that transistor.

    I did this with a stock demo version of Orcad 9 and arrived to a decent VTC.


  16. Apr 20, 2007 #15
    Thanks! One more thing, when taking the derivative I can just use the D() function correct? I just need to find the corresponding Noise Margins. I guess I can just 'eyeball' it or whatever, but I'd rather have a nice accurate value.
  17. Apr 20, 2007 #16
    With the stock models of transistors, the VTC that OrCAD produces is very "squarish". I think you could take values of VIH and VIL accurate enough from the corners of the charasteristic.

    However, the true VTC of a BiCMOS inverter is "rounder" and, in the case of arriving to a "rounded" VTC, you better use the D() function.
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook

Have something to add?

Similar Discussions: Need help with Pspice
  1. PSpice help! Needed (Replies: 1)

  2. PSPICE Help (Replies: 2)

  3. PSpice help! (Replies: 1)

  4. PSpice help (Replies: 1)