The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Problem in corner simulation with ADE
https://designers-guide.org/forum/YaBB.pl?num=1267690860

Message started by Yutao Liu on Mar 4^th, 2010, 12:20am

Title: Problem in corner simulation with ADE
Post by Yutao Liu on Mar 4^th, 2010, 12:20am

Hello everyone,
I sweep the channel length of MOSFET and check the threshold voltage with "dc" analysis in different corners.
And the expression in the measurement is v("M0:vth" ?result "dc-dc"). But it shows an error that "Invalid expression for Corners print".
How should I correct my expression in measurement?
BTW, I copy the expression from the "Output setup" in normal simulation.

Thanks for helping!
Yutao

Title: Re: Problem in corner simulation with ADE
Post by pancho_hideboo on Mar 4^th, 2010, 12:51am

I assume you use Cadence Spectre.

Confirm available data in PSF using "Result Browser".

The followings are general notes for you.

- Always describe vendor's name which you use as tool or simulator.
- Don't do multiple posts which are same content.
- Don't request source code or behavioral model without any efforts.
- There are many simulators which have analyses called as PSS, PAC and Pnoise.
- Describe in detail with using correct terminologies.
- Warnigns are different from Errors.
- ADS is not name of simulator.
- There is no tool which name is Cadence.
- Don't use Direct Plot of Cadence ADE blindly without knowing definition.
- All gains in Direct Plot of Cadence ADE are "right", "true" and "practical" voltage gain.
- Don't mix up Simulation with Post Processing. They are completely different phase.
- MATLAB are different from Simulink.
- Learn measurements using actual instruments. Not "EDA Tool Play

Title: Re: Problem in corner simulation with ADE
Post by Yutao Liu on Mar 4^th, 2010, 1:25am

Yes, I use Cadence Spectre.
First, I include a file with statement "save *:oppoint" in "model file", and plots of operating point parameters are available when running normal dc sweep. The parameters can be found in "dc-dc" in PSF.
Second, no operation point parameter can be found in "dc-dc" in PSF when doing corner analysis. And I think this is the reason for the error.
Is it impossible to plot operating points versus variable in corner analysis?
Or I miss some setting when doing corner analysis?
Thanks!

Title: Re: Problem in corner simulation with ADE
Post by pancho_hideboo on Mar 4^th, 2010, 1:37am

Yutao Liu wrote on Mar 4^th, 2010, 1:25am:

Is it impossible to plot operating points versus variable in corner analysis?
Or I miss some setting when doing corner analysis?

Simulation launching scheme is different in "Corner Tool" compared to other tool such as "Parametric Sweep".

I think "save *:oppoint" is not included by some reason.

You can confirm setting of "Corner Tool" as text file.

BTW, do you set "Save DC Operating Point" in "DC Analysis setting" ?

Title: Re: Problem in corner simulation with ADE
Post by Yutao Liu on Mar 4^th, 2010, 3:57am

I do set "Save DC Operating Point" in "DC Analysis setting".
Could you tell me more detail about "Corner Tool"? How can I get this file?
There is no corner tool setting file in my PDK. Is is written by myself?
Thanks!

Title: Re: Problem in corner simulation with ADE
Post by pancho_hideboo on Mar 4^th, 2010, 4:07am

Yutao Liu wrote on Mar 4^th, 2010, 3:57am:

Expect answers from Cadence guy, e.g. Sheldon or Andrew Beckett.

Title: Re: Problem in corner simulation with ADE
Post by Andrew Beckett on Mar 4^th, 2010, 5:06am

The question is a bit confusing. It would probably help to know how you're running the corners. Is this IC5141 or IC61X? Are you running Tools->Corners from ADE, or using Corners within ADE XL within IC613/IC614? Or are you using VSDE from IC5141 to set up your corners? Or are you using some custom tool to do this?

How are you setting up the corners - how are they defined?

Generally speaking, if you're using the corners tool (in, say, IC5141), then that will be responsible for defining which model files and sections are being used. So if you're adding your file as an additional model file in ADE, then it probably is not being included. I think if you add it as a "definition file" (under Setup->Simulation Files in ADE) then it will get included.

But this is just guess work - I don't know what version of anything you're using, or which tools, so it's really hard to give a precise answer.

Best Regards,

Andrew.

Title: Re: Problem in corner simulation with ADE
Post by Yutao Liu on Mar 4^th, 2010, 6:14am

Thanks for Andrew's suggestion. The method works!
The additional model file has to be included in "definition file" under Setup->Simulation files in ADE.

Best regards,
Yutao