Designer’s Guide Community

Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.

Jul 19^th, 2024, 12:37am

‹ Previous topic | Next topic ›

Pages: 1

output format in analog design environment (Read 12965 times)

arsenal_he Junior Member Offline Posts: 14	output format in analog design environment Mar 02^nd, 2007, 11:04am hi, i wanna know how to set the output format of spectre in analog design environment, such as psf or sst2? thanks arsenal
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: output format in analog design environment
Reply #1 - Mar 3^rd, 2007, 2:11am

The default these days is sst2 for transient, and psf for everything else (sst2 can only represent time domain data).

If you want to set it to psf all the time, you can use the SKILL function (in the CIW, or in your .cdsinit):

envSetVal("spectre.envOpts" "simOutputFormat" 'string "psfbin")

before starting ADE.

Why do you want to change it? By the way, don't have freedom to use all of spectre's output formats, because presumably you want the ADE waveform tool etc to be able to plot the results - and that only supports psf or sst2.

Regards,

Andrew.

IP Logged

arsenal_he

Junior Member

Offline

Posts: 14

Re: output format in analog design environment
Reply #2 - Mar 5^th, 2007, 10:05am

THank you very much, Andrew,
The reason i wanna switch to psf is that the dump interval of sst2 is much bigger than that of psf for a big design although it cannot be detected when for a small scale simulation. And since i dont know where to set the data-dumping interval, the only alternative is to switch back to psf bcoz i can see the results at the first sevel tens of ns instead of waiting for hundreds of nano-seconds to get the results of sst2.

thanks a lot
arsenal

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: output format in analog design environment Reply #3 - Mar 5^th, 2007, 11:04am Ah, the flushing problem with sst2. Yes, there's a PCR for that. Andrew.
Back to top	IP Logged

arsenal_he Junior Member Offline Posts: 14	Re: output format in analog design environment Reply #4 - Mar 5^th, 2007, 11:07am hi andrew, what does pcr stand for? where can i get it? thanks arsenal
Back to top	IP Logged

Geoffrey_Coram Senior Fellow Offline Posts: 1999 Massachusetts, USA	Re: output format in analog design environment Reply #5 - Mar 5^th, 2007, 11:37am pcr = product change request, I think; that is, someone's already requested a fix, but it's not available (you can't get it yet).
Back to top	If at first you do succeed, STOP, raise your standards, and stop wasting your time. IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: output format in analog design environment Reply #6 - Mar 5^th, 2007, 1:17pm Sorry I used internal terminology. Didn't think before I posted. Anyway, if you were to log a service request with Cadence, the relevant PCR numbers (at least) are 4015013 and 886334 (these are the reference numbers for where this has been reported before to Cadence R&D). Regards, Andrew.
Back to top	IP Logged

arsenal_he Junior Member Offline Posts: 14	Re: output format in analog design environment Reply #7 - Mar 5^th, 2007, 1:53pm hi Andrew, Thank you very much. arsenal
Back to top	IP Logged

ywguo Community Fellow Offline Posts: 943 Shanghai, PRC	Re: output format in analog design environment Reply #8 - Sep 19^th, 2007, 12:21am Hi, Can I convert a transient simulation result in sst format into psfbin/psfbinf format? Thanks Yawei
Back to top	IP Logged

JoRobins

New Member

Offline

Give and it shall be
given unto you!

Posts: 6
San Diego, CA

Re: output format in analog design environment
Reply #9 - Sep 29^th, 2007, 7:44am

As far as I understand, no! And why/how do I know this?

One of the features that I've been trying out is the savestate feature in the transient analysis of Spectre. This allows one to run a tran simulation to a certain time point and then run a new simulation using the previous sim's final transient state (actually, it could be anywhere in the previous run as long as you've saved the state) as the starting point. Unfortunately this creates two different sst2 sim data files - one each for the 2 runs. If you try to plot the data in the second run, the starting time will not be from 0s but rather from the last time point of the previous simulation and there is no way to stitch together two sst files. However there is a way to stitch together two psf files (a sourcelink solution explains this) and if there was a way to convert from sst2 files to psf, I could have had a workaround. Unfortunately, no sst2 to psf conversion exists (at least according to the Cadence AE). They filed a PCR to at least allow stitching together of sst2 files... :-/

IP Logged

Pages: 1

‹ Previous topic | Next topic ›