How to plot OP parameter with sweep variable in Spectre?

[peterlau1984]

spectre transconductance

Hello everyone,
I am confused how can i plot the operation point parameters with sweep variable in Spectre?

For example, how to plot transconductance of a MOSFET versus Vgs?

Thank you so much!

 

[iamxo]

using sweep command for spectre

Hello everyone,
I am confused how can i plot the operation point parameters with sweep variable in Spectre?

For example, how to plot transconductance of a MOSFET versus Vgs?

Thank you so much!

As i know, use the belowing:
set vgs as a variable, sweep vgs, set plot as OP("/M0","gm")

 

[mengcy]

+spectre +info +oppoint +file

iamxo is right.

 

[peterlau1984]

plot dc sweep parameters,spectre

Thanks for your reply.

I did the setting as you mentioned, and run the dc simulation. However, I only can get a value of gm correspond to the value of Vgs set in variable tab, instead of a waveform.

Is there any other methods?

 

[saro_k_82]

spectre sweep parameter

You need to save the parameter of the transistor before running the sim. The operating point info is not saved by default for dc sweep. You can do that by creating a .scs file with the command
save M0:gm
and then add that file as a stimuli file in ADE or manually include that line in the input.scs file

 

[oermens]

spectre operating point at different dc sweeps

if youre using MMSIM6.2 and up, try save *ppoint to save all swept parameters

 

[tanguaner]

how to plot operating point information spectre

first,you should save operating points in a dc analysis,then do parameter sweep,after that,you can do as iamxo says.

 

[peterlau1984]

operation point mosfet spectre

I did it as tanuuaner said, and it works.
but it seems to waste a sweep variable, because the dc sweep and the parametric analysis use the same seep variable.
Is there any other methods?
thanks!

 

[iamxo]

spectre plot parameter

Thanks for your reply.

I did the setting as you mentioned, and run the dc simulation. However, I only can get a value of gm correspond to the value of Vgs set in variable tab, instead of a waveform.

Is there any other methods?

Use the Parametric Analysis to get the waveform.