How to plot device parameters from transient sims.

Hi,

if these parameters are stored in the results / psf folder, you can use the OCEAN commands to plot them. Therefore you have to do the following steps:

Open the results:

    - e.g.  openResults("/myAbsolutePath/...../...../psf")

Select the results:

    - e.g.  selectResults('tran)

    - you can use results() to display the selectable relults --> (dc tran ac)

Get the waveform Id:

e.g.  wId = getData("net0815")  --> waveform Id drwave:24234545

Plot the waveform:

e.g. plot("wId")

If you have to calculate the parameters, you can use the OCEAN waveform calculator command described in the OCEAN reference.

Regards

haiko

 Hi haiko,

  Thank you for your response.  Unfortunately it does not answer my question.  Let me try to be more specific:

I already know how to open results, view and plot voltages and  currents in ocean and analog artist.

I want to plot the small signal parameters of the BSIM4 model of some transistors during a transient sim.  Particularly, I want to track how the gm, cgd, and cgs change as a function of time.  These are transistor parameters, not voltages and currents.

How do I:

1) save these in simulation

and 

2) plot them as a function of time.

And just to be completely clear, I am NOT interested in the operating point of these devices at a single time step like you can access using the menu: Results -> Print -> Transient Operating Points  OR the calculator expression: OPT("/dut2/MNP" "gm") which only give me these parameters at a SINGLE point in time, not as a waveform in time.

This is a trivial thing to do in HSPICE, so I assume it must be a trivial thing to do in Spectre and Analog Artist.  I just can't find it.

Thank you,

Eric.

 Nevermind,

  Found it in SourceLink solution number 11003524.

It turns out you need to create a text file that contains:

save M1:oppoint M2:oppoint

etc. for all the transistors and then access the data through the results browser.

Not as easy as I expected it to be, but at least it's possible.

Eric.

Hi Eric,

I'm did not understand completely, what you want. The save statement "save M1:oppoint ..." seams to save the final operating point parameters. If you want to access theses values you can do this using the following way:

\i results

\o  (tranOp subckts instance "tranViolations-violations" model "tran-info" variables output designParamVals tran primitives)

\i selectResults('tranOp)

\o  stdobj@0xc36030c

\i outputs

\o --> a huge list with all possible outputs :)

\i  m0Id=getData("I8_0.M0")

\o dr:0xbb45018

Now you can access the final operating point parameters (gm, gds, cgs ....) using the squiggle operator:

\i m0Id~>cgs

\o  -4.857316e-15

Here you just have one value for the final operating point. You can carry out a parametric analysis to get an parameter plot e.b. cgs vs. Vds.

Is this what you want?

Regards

haiko

Hi eric,

I am also facing the same problem , can you please tell me weather you got solution of this problem or not.

Thanks & regards

Prateek jain

The Forum Guidelines tell you not to post on old threads (and this one was VERY old - more than 4 years old).

And anyway, the answer was given by Eric in the thread, including a reference to a solution number on Cadence Online Support. This has been covered on numerous occasions on this forum too.

Andrew.