Can I find out the output resistance (rds or gds) of MOSFET directly from Spectre simulation (w/o us

thanks!

 

If it's a DC operating point, you can get this directly.

If it's a transient analysis, then create a file, put:

save M1ppoint

or

save M1

or

save M1:gds

where M1 is the instance name of the component in the netlist - may be hierarchical,
for example I1.I2.M0.

Then specify this file as a "Model File" (they don't have to be model files - any spectre
syntax file can be included here).

Run the simulation, and then using the results browser, you will be able to navigate down
to the transistor in question in the transient results, and find the gds (or any other
operating point parameter). The exact list of parameters can be found by looking
at "spectre -h bsim3v3" (if it is a bsim3v3 model; use the appropriate model type).

Regards,

Andrew.

 

Andrew,
If that's a DC operating point, how can I get the gds(rds) directly
(BTW, I think most of the time peopel only care the DC value of gm and
gds for linear ckt.)? From the simulator ouput (Spectre.out), all the
operating point info is just about voltage or current. I was using DC
sweep and parametric analysis.
I did choose "Save all" from "ouput" in the Analog Enviroment menu.
thanks for your help!
Jay

 

Andrew,
Got it from psf->Run1->dcOpInfo-info
I thought this could be directly back-annotated into the schematic.

As you suggested method, I also successfully plotted the gds vs. Vds
from pdf->Run1->Mn->gds. But I got some more questions (can't find
much info about these in Cadence's cdsdoc), how is the psf tree
organized? What exactly do dc-dc, dcOp-dc, dcOpInfo-info etc mean?
Seems to me they act differently to mouse click...

many thanks for your valuable time!

Jay

p.s.: If I use Spectre (w/o the SPICE translator), all the statements
etc in other simulation files (include file, difinition file and
stimulus file ...) should follow native Spectre syntax, right?

 

Jay,

If you look in the netlist produced by ADE, typically it will include things
like:

dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
dcOpInfo info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile

Each of these is writing out a "rawfile", and the file name will be
called (by default) instanceName.analysisName.

The first (dcOp.dc) will contain the DC node voltages etc.
The next few are "info" analyses - see "spectre -h info" for more
details. dcOpInfo.info is going to contain the operating point information
(gm, gds, vdsat etc for each device).
I think the next few are fairly self explanatory?

You can access this data using OCEAN functions. For example:

pv("/M1" "gds" ?result 'dcOpInfo)

Some will be scalar, some will be vector. For example, if you're doing a DC
sweep, it doesn't normally save the device operating point info - but it would
if you use the save statements I mentioned with transient - in that case, if
you did a sweep, you can get the vector (waveform) using:

getData("M1:gds" ?result 'dc)

say.

Regards,

Andrew.

p.s. Yes, they would all be in spectre syntax. See my recent post about various
syntaxes used by spectre.