Plotting gm while sweeping the temperature

[tmozdzen]

I'm using analog artist version 5.1.41 and would like to be able to plot gm as the temperature is swept.

I can get a single value for gm when I go into the calculator, request info, select op, click on the transistor, choose gm from the pull down menu.

I've tried adding M0:gm to the list of outputs, but it doesn't seem to like that either.

Any help is greatly appreciated.

Tom

 

[PaloAlto]

When you do a temperature sweep, the OP is calculated only once. Then some equations are used to see how different values would change with the temp dependency, but the transistors are considered to be in the same OP, so, same gm

That is why this simulation is so fast.

What you have to do is parametric analysis. Select as variable to be changed temp and put a number of points, then in every point, a new OP is calculated

After that you can plot gm vs temp

 

[malizevzek]

What you have to do is parametric analysis. Select as variable to be changed temp and put a number of points, then in every point, a new OP is calculated

After that you can plot gm vs temp

@PaloAlto: Are you sure you are talking about simulating in Analog Artist?

 

[PaloAlto]

I'm positive.

A DC sweep is just one OP analysis and on top of it you sweep one particular parameter like temp, or some dc voltage.

On a parametric analysis, you repeat the analysis that you have selected in ADE (OP, tran,...) for every value of the chosen variable.

In fact it is the same as selecting in ADE setup-->temperature, changing it and simulating again

 

[malizevzek]

OK, that is all correct.
Can you please tell me then how to plot gm as a function of temp? I still don't see how you can select gm to be plotted as a function of sweeping parameter, in this case temperature.
I don't see the list of results for gm in Results Browser either - there is only one gm value, probably for the last swept temp value.

 

[PaloAlto]

When you select the analysis type, you cannot choose DC sweep (temp). You have to do only save DC operating point and then go in ADE to tools-->parametric analysis and in the field variable name type "temp" add the values that you want and voila!

 

[malizevzek]

Voila indeed!!!

 

[tmozdzen]

Awesome!
voila for me too.
Thanks a ton.
Tom

 

[Areky_qin]

I think you can get the value,
nomally, I use the hspice run simulation,
i use .probe lx7(device name), the the wave form will show the gm of the mosfets. I think the spectre should have the same feature.

hope it it help for you, good luck.