Stats

  • Locked Locked
  • Replies 4
  • Subscribers 165
  • Views 13350
  • 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

parameters as an expression

SolarStudent
Hi Guys,

Hopefully this is in the correct forum.  Using Capture/PSpice to simulate the dynamic response of solar cells from changing radiation conditions.

I want to set the saturation current of a standard diode to equal an expression, eg. IS = {(a*b) + c}

I've setup the values of a,b,c as parameters for the sub-circuit.  Have gone into "edit model" for the diode and attempted to write the expression in "value" cell for the IS property.  However I get this message

 The parameters made editable cannot have NULL values.  Please enter a valid value in the field.

 I have had a go at making a new model (based on the standard diode).  But the field clears before I can input the full expression.

 So far all the instructions for modifying "models" are for when you are just using PSpice code, not Capture.

 
Thanks in advance

Matt
Using Capture/PSpice lite - v16.5.13D
  • Alok Tripathi
    You need to edit the parameters in text mode. It seems that you are using template based model and editing the parameter in table view. I would suggest trying “Device Characteristics Curve based” model and editing the IS parameter in “View>Edit Mode” mode (this would be text view).
  • SolarStudent

    Hi Alokt, So I created a new model using device characteristic curves. I've copied the model text below. 

    *BeginSpec
    *IF:
    *JC:
    *RL:
    *RB: Vz=0 Iz=0 Zz=0
    *RR: Trr=0 Ifwd=10.000E-3 Irev=10.000E-3 Rl=100
    *EndSpec
    *BeginTrace
    *IF: 1,0,.4,1.2000,1,3,0,0,-1 (27)
    *JC: 0,1,.1,10,1,3,0,0,-1 (27)
    *RL: 0,0,1,100,1,3,0,0,-1 (27)
    *RB: 0,1,100.00E-6,1,1,3,0,0,-1 (27)
    *RR: 0,0,-5.0000E-9,20.000E-9,1,3,0,0,-1 (27)
    *EndTrace
    *BeginParam
    *IS=10.000E-21
    *N=1 (.2,5,0)
    *RS=1.0000E-3 (1.0000E-6,100,0)
    *IKF=0 (0,1.0000E3,0)
    *XTI=3 (-100,100,0)
    *EG=1.1100 (.1,5.5100,0)
    *CJO=1.0000E-12 (10.000E-21,1.0000E-3,0)
    *M=.3333 (.1,10,0)
    *VJ=.75 (.3905,10,0)
    *FC=.5 (1.0000E-3,10,0)
    *ISR=100.00E-12 (10.000E-21,.1,0)
    *NR=2 (.5,5,0)
    *BV=100 (.1,1.0000E6,0)
    *IBV=100.00E-6 (1.0000E-9,10,0)
    *TT=5.0000E-9 (100.00E-18,1.0000E-3,0)
    *EndParam
    *DEVICE=Diode_Cell_2,D
    * Diode_Cell_2 D model
    * updated using Model Editor release 16.5.0 on 11/07/11 at 21:41
    * The Model Editor is a PSpice product.
    .MODEL Diode_Cell_2 D
    + IS= {(a*b) + c}
    + RS=1.0000E-3
    + CJO=1.0000E-12
    + M=.3333
    + VJ=.75
    + ISR=100.00E-12
    + BV=100
    + IBV=100.00E-6
    + TT=5.0000E-9

    So I think that I've created a new model and changed the IS to equal the expression {(a* b)+c}. Do I need to also change IS to an expression in the "begin prams" section too? Also how do I know when I run the simulation that it is using my new model for the diode and not the original? There doesn't seem to be anyway to check.

    Thanks again.

  • Alok Tripathi
    No, You need not change that in PARAM section. Any line starting with * is treated as comment in PSPICE/SPICE, so you can ignore those.

    PSpice picks up the model based on it’s name. Model name “Diode_Cell_2 “ selected by you is unique and model with this name is not supplied with PSpice, thus chances of simulation is done with another model is zero, unless you have developed other diode models with same name and configured that in simulation setting.

    You can turn on the “LIBRARY” option under Options output file in simulation setting. This will list down library and models used in current simulation in simulation output file.
  • SolarStudent
    Excellent, I think I got it to work. I doesn't list Diode_Cell_2, but it does list "idealcell.lib" which I think contains the information for the modified diode model. Cheers Alokt
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.