PSpice error: Not a valid parameter for model type

[pisoiu]

Hi,
I want to make an ac sweep type simulation using parametric sweep over a simple analog circuit (orcad pspice 9.1). At parametric sweep option, I want to sweep the value of a capacitor betweet two limits (sweep variable: Model parameter). I have to enter in the parametric sweep window CAP at Model type, C2 at Model name (this is the cap I want to sweep), Value at Parameter name, and at Sweep type: linear , start value 1p, end value 100p, step 0.01p. Even if all these seem correct, I get always the same error msg from pspice: "ERROR -- Not a valid parameter for model type". Can anyone help me plz? Thanks.

 

[Humungus]

pspice not a valid parameter

I don't know much about PSpice (but quite enough of spice), but first question is: are you using a special capacitor model or just an ideal capacitor?

What about if you left blank where you put CAP as model?

In crude spice what you want to do would be

.param valuecap=1p

C2 x y valuecap

.ac ac_sweep_type np fstart fstop SWEEP valuecap LIN 1p 100p 0.01p

I hope it helps you

 

[pisoiu]

error -- not a valid parameter for model type

Hi,
It is the cap from *rcad pspice 9.1 simulation library, nothing special at it. I cannot leave blank at CAP model, because it is a dropdown menu, not a text field..I must choose something. My pspice text output looks like this:

*Analysis directives:
.DC LIN V_V2 -5 5 0.1
.STEP LIN RES R9(Value) 400 500 10
-----------------$
ERROR -- Not a valid parameter for model type
.PROBE
.INC "simulation-SCHEMATIC1.net"

this time it is from a dc sweep analysis, but the idea is the same, I want to sweep the parameter of a certain component, in this case R9.

Thanks in advance.

 

[Hughes]

dc sweep simulation in pspice 9.1

Hi, pisoiu,

I didn't use pspice but has some experience in hspice. I reviewed pspice reference and found the possilbe reason as follows.

The syntax of your .STEP statement is
.STEP LIN <sweep variable name>
+ <start value> <end value> <increment value>

In your case, as i think, <sweep variable name> should be a global parameter defined in .PARAM statement, instead of a model parameter.

Your .STEP statement,
.STEP LIN RES R9(Value) 400 500 10
shoud be used to sweep a resistor model. The model name is R9 and one of a model parameter is 'value' -- as I know, resistor model doesn't have such model parameter. So, your netlist should rewrited as

Rxxx a b R=R9
.....
.DC LIN V_V2 -5 5 0.1
.STEP LIN PARAM R9 400 500 10

Please see if 'Model type' has a option of 'PARAM'. And see pp 79-81 of
**broken link removed** for more information. Good luck!

 

[gitarrelieber]

pspice 9.1 simullation

Hi pisoiu,
To solve your problem, follow the steps below:
1. Add a part which names "PARAM" to your schematics. This part is located in the library "special.olb" under the folder of "...\capture\library\pspice".
2. Double click the PARAM component; add a new property to the PARAM component by clicking the button "New Column" in Property Editor. Fill the consequent dialog with "CAPACITY" and "0.1p"
3. Replace the value of your capacitor in the schematics with "{CAPACITOR}" by double-clicking the value near the capacitor symbol.
4. Invoke the simulation setting dialog, enable the "parameteric sweep", choose "global parameter" in the dialog, fill the blank "Parameter Name" with "CAPACITOR"
5. Simulate!
good luck!

 

[babyice]

spice parametric sweep

I didn't use pspice but has some experience in hspice. I reviewed pspice reference and found the possilbe reason as follows.

The syntax of your .STEP statement is
.STEP LIN <sweep variable name>
+ <start value> <end value> <increment value>

In your case, as i think, <sweep variable name> should be a global parameter defined in .PARAM statement, instead of a model parameter.

Your .STEP statement,
.STEP LIN RES R9(Value) 400 500 10
shoud be used to sweep a resistor model. The model name is R9 and one of a model parameter is 'value' -- as I know, resistor model doesn't have such model parameter. So, your netlist should rewrited as

Rxxx a b R=R9
.....
.DC LIN V_V2 -5 5 0.1
.STEP LIN PARAM R9 400 500 10

Please see if 'Model type' has a option of 'PARAM'. And see pp 79-81 of
pspice reference for more information. Good luck!
_________________

 

[mukeshk]

simulation rl with pspice 9.1

U can also list the values of the parametrer using following command
.step <param name> LIST <value1> <value2>..