Is there a way to run simulation using command line and view

[Allen]

I need to run some simulatoins using command line, since the netlist
needs to be modified. However it's not convient to view the results
using wavescan, is there a way to view results using Vertoso Analog
Design Environment GUI? Thanks a lot.

Best,
Allen

 

Allen wrote:

using wavescan, is there a way to view results using Vertoso Analog
Design Environment GUI? Thanks a lot.

Allen,

I don't know if this is what you're looking for or not, or if there's
an
MDL equiv for this (this is awd-centric...), but FWIW, here's
something I came up with for one of my designers. You'll
find SourceLink references to this if you look hard enough.


-Jay-

Stand-alone Spectre Waveform Viewing with AWD
---------------------------------------------
Fri Jan 7 19:14:55 PST 2005 jayl

SUMMARY: run awd, center-click "Create ROF", Commands->Refresh, and
your results are in the .raw directory.

By default, spectre writes a waveform results format called "binary
PSF", which awd knows how to read (and precious little else does,
AFAIKT).

In the Artist environment, there is a bunch of other baggage sprayed
around in the netlist and psf subdirectories to help awd understand how
to handle the PSF file. When you run spectre stand-alone (not from the
Artist GUI), some of this is missing. Here's what you do.

1) If you ran spectre on netlist "mysim.sp", you should have ended up
with a new subdirectory "mysim.raw". This should have one or more
PSF files (named "mysim.raw/analysysOP1.dc", or
"mysim.raw/tran.tran"). There should also be "mysim/logFile".
That's essential. Great. Stay right here where you are and run
awd:

% awd &

2) The Browse Project Hierarchy window will come up with a default
entry of ".", which is what you want, hit OK.

3) You'll see the "mysim.raw" directory in the Results Browser. Do
a center-mouse-button pull on mysim.raw and select "Create ROF".

4) Do a Commands->Refresh.

5) Left-click on the "mysim.raw" directory, and bada-bing you've
got simulation output.

 

[Satya]

Allen wrote:

I need to run some simulatoins using command line, since the netlist
needs to be modified. However it's not convient to view the results
using wavescan, is there a way to view results using Vertoso Analog
Design Environment GUI? Thanks a lot.

Just open the Analog Design Environment for the view you simulated. Then go
to Results->Select. Browse to the appropriate result and Select. Voila! The
results are as if you simulated from ADE.

Satya


--
Posted via a free Usenet account from http://www.teranews.com