Should I change the stimulus file, and group them in the loop as describe here http://www.cadence.com/Community/forums/p/23667/1315087.aspx ?
Actually I don't know too much about the stimulus file because normally I run with ADEXL, the stimulus file is set automatically. If anybody can explain something about the "stimulus file"?
Thanks.

Jacki wrote on Mar 21^st, 2014, 10:51am:

I don't know. I suggest you try Code:

alter 

in the spectre netllist.
- B O E

boe wrote on Mar 31^st, 2014, 4:27am:


Hello B O E,

   Thank you for your comments. I will try it.

You should sort this out with your adminstrator.

There's nothing enormously sensitive about that solution, so I will post it here:

Problem

You wish to have a vpwlf voltage source with parametric file name.

By doing this, you can use a single schematic to run several simulations which differ in the PWL file used to drive the circuit.

Is this possible?
Solution

This can be done relatively easily.

1.    Take a copy of vpwlf from analogLib into your own library
2.    CIW Tools->CDF->Edit
3.    Set the CDF type to "Base", and fill in the lib name and cell name of your vpwlf.
4.    Go to the simulation information tab. Choose spectre as the simulator.
5.    Add "file" to the instParameters and remove "file" from the stringParameters.
6.    Go to the "Component Parameters" tab, and click on the row for the parameter fileName.
7.    Set parseAsNumber to "yes" and units to "don't use".
8.    OK the Edit CDF form.

What this will do is mean that if you get a design variable name in the file name field for your vpwlf source, it won't netlist it with "" around the name. So, if you specify the filename as myfile, and then add a design variable in ADE called myfile with value "myfile.pwl" (and you need to include the quotation marks in the design variable value), it will end up netlisted something like this:

Code:

simulator lang=spectre
global 0
parameters pwlFile="myfile.pwl"

// Library name: test
// Cell name: testvpwl
// View name: schematic
V0 (net3 0) vsource file=pwlFile type=pwl
R0 (net3 0) resistor r=1K 

and spectre will quite happily simulate that.

Step 7 in the instructions above will do two things. First it will allow the design variable to be found if you do a Variables->Copy from CellView in ADE. Second, it will show the evaluated filename if you use the Edit->Component Display to evaluate the parameters for the vpwlf instance in "Full" mode. Whilst it isn't actually a number field, so parseAsNumber is not entirely appropriate, it does allow these two additional features to work.

The above will only affect spectre netlisting; for other simulators, similar modifications in the simInfo for that would be necessary - assuming that the simulator supports string parameters. If not, you may want to delete the stopping view for that cell to prevent any problems.