How to plot gm vs id in cadence

For transistor characterization how to plot GM Vs ID curve

This has been discussed before and there are quite a few guides. See for example

* https://www.edaboard.com/attachment.php?attachmentid=61585&d=1316222659

* https://www.edaboard.com/showthread.php?158838-how-to-plot-gm-id-vs-id-in-cadence

or others outside this forum (cadence forum itself, for example).

Hi,

check the links in the "similar threads " box below.

Please next time do a forum search before asking a question.

Klaus

hi

I had gone through the above thread and the manual.In the manual how to obtain gm /id is explained.But how to set x axis to id is not mentioned.I can see in image(attached one as given in manual) as vs id.Is it possible to provide vs in calculator.I tried,but plot was not obtained.In the thread its mentioned rightclick x axis to change property plot vs.But can't find an option like that,due to which I am unable to get plot vs id

Before you click, make sure you plot both I and g_m as function of whatever variable you have. Then click on x-axis and select I instead of "independent variable" or whatever it might say

Thanks for your reply sir.I did it.I plotted iD and gm vs vgs .Then for X AXIS, using Y vs Y option ,I chose iD. Now I can plot gm vs ID .
Now I am stuck with another problem.My technology library is UMC180.When I use UMC_N_18_MM (MEDIUM MODE Transistor), I obtain all the Dc parameters like gm,vgs,vth etc in Results browser.But for UMC_N_L_18_W_500_RF transistor, which is the one I require for RF design,after the dc analysis result browser window dc info doesn't list gm,vgs,vth etc.Since I can obtain drain current from schematic,I am plotting Id vs Vgs and taking derivative to obtain gm.Then to obtain gm by id ,I change x axis as done previously.I would like to know whetehr there is any means to list out these dc parameters in results browser window,whereas if I do prit dc operating point of RF transistor,I can see all these.But they are not available in dc Result browser,to use them in calculator or graphs.To obtain graphs with vgs-vth as x axis i need these dc parameters in dcinfo.They are obtained for MM transistor ,but not for RF transistor.

I do not have that particular flavour of the process installed. Sometimes, though, the RF models are a "two-level" device with a transistor instantiated inside a model with RC-interconnects such that high-frequency behavior can be simulated a bit more accurately.

In your results browser, don't you do not see a sub-transistor? Called something like m0 or so? That could contain the results for the transistor. Rather than getting OP("/MN1" "blahblah") you get something like OP("/MN1.m0" "blahblah") ?

It's a bit strange though, that you can print the DC operating points... Check the print-window, what does the expression say? What's the name of your transistor there?

I Have saved dc operating point of RF transistor save M0:all. After the dc sweep in print Dc operating point and dcop info in Result browser I can see instantaneous dc values of all parameters.But under dc in Result browser from which parameter can be sent to calculator or to plot window,I cannot obtain gm,vgs,vth etc.What I obtain in dc in Result browser is attached in figure above.When I do the same for MM transistor ,it list out all parameter in dc is shown in this attachment

Isn't the information you want stored under dcOpInfo ? And then go to transistor M0.main (which is the subtransistor)? The _MM transistor will not have a ".main" option.

Thank you very much .Problem is solved.I saved operating point as save M0.main.all.Now I am able to plot gm of RF transistor.