The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> How to run Ocean with ADEXL for many loops.
https://designers-guide.org/forum/YaBB.pl?num=1395339788

Message started by Jacki on Mar 20^th, 2014, 11:23am

Title: How to run Ocean with ADEXL for many loops.
Post by Jacki on Mar 20^th, 2014, 11:23am

Hi All,

I have a question about the Ocean run in IC6.1.5 (ADEXL). Now I have 128 source files (.txt) and import them one by one through "vpwlf". Each time, I can only run one source file, and get one result. It is boring that I have to run 128 times to get all of the results.
Is it possible I write a Ocean script and run the loop, every time the settings in the simulation is fixed, only needs to change the source file e.g. ./Cadence/sourcefile1.txt ./Cadence/sourcefile2.txt ... ...., actually every time the netlist should be updated as well.
Any comments?
Thank you.

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Jacki on Mar 20^th, 2014, 11:35am

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.

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Jacki on Mar 21^st, 2014, 10:51am

I check the Ocean reference manual, it seems the for loop is only for parametric sweep. Is it impossible to import many signal source files (.txt) by pwlf automatically one by one, and do the simulation respectively?

Title: Re: How to run Ocean with ADEXL for many loops.
Post by boe on Mar 31^st, 2014, 4:27am

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

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Andrew Beckett on Apr 7^th, 2014, 12:36pm

This solution on Cadence's support site http://support.cadence.com/wps/mypoc/cos?uri=deeplinkmin:ViewSolution;solutionNumber=11366978 explains how to create a version of vpwlf which allows the fileName to be a variable, and then you can control the fileName with a desVar(). You can then use a foreach loop in your OCEAN code to change.

Kind Regards,

Andrew.

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Jacki on Apr 10^th, 2014, 1:24pm

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

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

Hello B O E,

Thank you for your comments. I will try it.

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Jacki on Apr 10^th, 2014, 1:26pm

Andrew Beckett wrote on Apr 7^th, 2014, 12:36pm:

Hello Andrew,
Thank you for your link, but my account of Cadence on-line support is disabled by our administrator. I cannot log in to check the information one the website you sent. Can you show me some information here?
Thank you.
Jacki

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Andrew Beckett on Apr 16^th, 2014, 12:43am

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.

Title: Re: How to run Ocean with ADEXL for many loops.
Post by Jacki on Apr 18^th, 2014, 9:03am

Hello Andrew,

Thank you very much.
Jacki