Plotting transistor parameters against time

Hello all! I am in the need of plotting the variation of some
transistor model parameters (like gm, vth and the like) in a transient
simulation, as a function of time. In a past post (http://
groups.google.com/group/comp.cad.cadence/browse_thread/thread/
1158a64d7923b3be/679182c31ec4cdb8) Andrew states that it should be
possible to use the Results Browser, navigate to the devices of
interest under the "tran-tran" tab and access these parameters.
However, when I do this for my transistors I can only find the drain
current "D" available.

I think I might be missing some switch or option to save these
parameters during the transient simulation; I would be really
grateful if someone could please explain in detail how to access these
parameters (preferably by using just the results browser and avoiding
the manual creation of auxiliary files). Please note that I am
interested in the whole set of transient operating points against
simulation time, not in single points at definite instants.

Thanks in advance for any help!

Cheers,

Jorge.

 

Sorry...I really need to search better before asking... I found the
missing info in the Cadence community forum; here it is for
completeness.

SourceLink solution #11003524
How to save and plot oppoint of Spectre transient simulation

Solution:
You have to tell Spectre to save the needed information. This is done
by adding the
correct save statement to the netlist. Say you are interested in
plotting the
operating information for a bipolar device name Q1. Add the following
statement to
your netlist:

save Q1ppoint

To add a save statement in the Analog Design Environment you need to
create a file,
myop.scs, and add the line above into it. You can include the file by
pointing out
the file as a model using: Setup->Model Libraries...

After a successful Spectre transient simulation you can now plot the
results from the
Results Browser, invoked using: Tools->Results Browser... or from the
Calculator.
If you are are running Spectre from a command line you need to invoke
'awd' to plot
the results.

Find the results directory and click on the transient directory. Click
the device Q1 and
a list of operation point parameters are shown. Right-click the
parameter of
interest to plot it.

 

Just one further doubt: Is it possible to add an expression/output/
whatever in the ADE window in order to have these parameters plotted
automatically after the simulations are finished?

For instance, say I am interested in plotting the transconductance of
instance M1 against time. Following the method described in the post
above, I go to the results browser, navigate to the desired instance,
find the model parameter "gm", and then right-click "new subwin" to
plot it; this creates in Wavescan the desired waveform and labels it
"M1.gm". My question is then, what (if possible) should I enter as an
expression or whatever in the "Outputs" sections of the ADE window so
as to plot this transconductance automatically along with all the
other transient waveforms?

I was thinking maybe I could I use the calculator to first construct
an expression to load the desired results (more or less equivalent to
picking them from the Results Browser) and then pass it to ADE, but I
haven't been successful...

Thanks again for any clues!

Jorge.

 

spectrallypure wrote, on 12/02/08 11:38:

Hi Jorge,

In addition, with versions of spectre since MMSIM62, you can now use wildcards
in the save statement, so do things like:

save *ppoint

See "spectre -h save" for more details. There's lots of options to control matching.

Anyway, in order to get the signal in the outputs pane, you'd select the item in
the results browser, and send the signal to the calculator. Then in the
Outputs->Setup (also an icon in ADE) you can get the expression from the
calculator, and arrange for it to be plotted automatically.

Regards,

Andrew.