X-Y ascii file from Spectre

Hi,
I am trying to figure out how to get the data from a spectre simulation
in X-Y ascii format.
Using the -f psfascii I can get a dc.dc file in ascii, but still that
file is in a very cumbersome format.
Why can't a get a strightforward X-Y format?
By using wavescan I can export a X-Y graph but I want to do all this on
the coomand line so that I can post process the IV data.
If some one has a solution plz plz let me know.
Thanks much
mayank


my deck looks something like this
// Design cell name: diode_t
// Design view name: schematic
simulator lang=spectre
global 0
include
include "./diode.pm"

// Library name: CAD_TEST
// Cell name: diode_t
// View name: schematic
D0 (p 0) default l=12u w=400n m=25
V0 (p 0) vsource dc=VBIAS mag=1 type=dc
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12
temp=25.0 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5
maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
sensfile="../psf/sens.output"
ac ac start=1K stop=1G annotate=status
dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
dcOpInfo info what=oppoint where=rawfile
dc dc dev=V0 param=dc start=-3.6 stop=0.8 step=10m oppoint=rawfile \
maxiters=150 maxsteps=10000 annotate=status
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
save V0
saveOptions options save=allpub

 

You could:
* Use ocean to postprocess your data
* ocnPrint
* Roll your own
* Use the secret tool psf
* psf -help (other than this no help no manual)

 

Thanks for the reply Bjerken,
But I really dont believe that this can be the only possible solution.
I can't even get the ocnprint to work.

 

no, it is not the only solution. Doing some searching of your own before
asking _is_ the only solution. This very same question was posted less
than 2 weeks ago by "vivian" and answered. Probably many time before as
well.

 

In this case, it is probably good to mention http://groups.google.com
which is the name of the place where all USENET posts are archived in
case your NNTP server does not store the articles for long time, and
thus _the_ place. It is an excellent search tool for USENET articles.

In answer to the fact that you can't get ocnPrint to work, I can only
say: "Oh, dear, what a pity. Would you care to share what you did in
order to fail?" Mind reading is difficult enough within the same room,
and almost impossible across the net.

 

Hi Svenn,
Thanks for your reply and words of advice.
I will try to learn something here. Any way
A colleague for mine gave me the right pointer. Using

spectre -format nutascii circuitfile.scs

changes the file to ascii columnar format. In the file generated the
first term is the line number then X-Y sweeps.
One can get ride of the line number by a simple perl script, or better,
just import in to excel and delete the column.

Hope this helps other people in the future.
BR
Mayank

 

It would not be possible to use this solution with the analog design
environment. (at least according to my experience) This is a command-
line simulation solution. The fact that you simulate on the command line
could also be the reason why ocnPrint didn't work for you.

 

When I first posted my question, I really wanted to this on the
"coomand" line (shh.. that should have been command)
And this solution would work for any one wanting to do the same.
Thanks
Mayank

 

repost of my answer to vivian:

- use a veriloga module with a strobe() , such as the "voltmeter" cell
in the ahdlLib
- use the "psf" executable to turn a binary psf into ascii
- use the "option" card from spectre to specify the output format. You
can use ascii and nutmeg.

Mayank,
do you have a solution now ? If so, post a follow up plz.

 

Hi Fogh,
Very frankly I am a beginner in the world of Spectre, so when you
mention options like using veriloga with strobe(), I get very vary of
using them. I had a very simple DC Sweep file and the option that I
mentioned

spectre -format nutascii circuitfile.scs

worked perfectly for it.
I do appreciate your detailed answer to my query.
Best regards
Mayank Gupta.
Hi