Stats

  • Locked Locked
  • Replies 7
  • Subscribers 125
  • Views 31268
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

How to save transient operating point?

BaaB

This is an old answer to saving DC operating points. I am wondering if there is a similar way to do that with transient analysis. I would like to save all transient operating point parameters and then plot them with time.

I tried the solution here but that doesn't work. The transient directory doesn't have the needed info.

I am using IC6.61-64b.500.9 and MMSIM13.1.1.049 64 bit.

QUOTE: Answer by Andrew:

This is a very commonly asked question.

Create a text file (called, say, saveop.scs) with the following contents:

// include file to save op point data
save M0:all

where M0 is the name of the mosfet. See "spectre -h save" for more details on the save statement.

Then, in Setup->Model Libraries, reference this file (I gave it a .scs suffix so it is interpreted in spectre syntax).

Run your DC sweep, and then you can access the results via the results browser - or just use an expression such as:

getData("M0:vdsat" ?result 'dc)

This will then show vdsat versus the swept parameter. 

The same approach will work if you want to save operating point during a transient - you can always just save the specific op point information by doing:

save M0:gm M0:vdsat

for example.

Best Regards,

Andrew.

 

Parents

  • You select the transistor, and then either type in the name of the oppoint parameters you wish to save, or hit the "..." button:

    If you hit the "Get from simulation" button, it will run a short sim and extract the available parameter names and populate the list to pick from. Because you're setting this up before simulation, it doesn't yet know what the available parameters are.

    This inserts the following line in the netlist:

    save I0.I0.PM0:gm I0.I0.PM0:vdsat 

    (I had selected gm and vdsat). 

    These results appear in the results browser in the appropriate place in the hierarchy. You can also use the "plot" checkbox on the ADE form to get them to be plotted automatically, or you can use the ot button in the calculator to retrieve the results. Or you can use the results browser.

    If they're not in the "tran" output, and the tran "folder" is empty (which seems strange to me), then maybe you have some strange settings on the Outputs->Save All form, but I can't see how you'd do that either!

    The spectre output log should record some information about the number of things saved too - so maybe you need to look at that too.

    Regards,

    Andrew.

Reply

  • You select the transistor, and then either type in the name of the oppoint parameters you wish to save, or hit the "..." button:

    If you hit the "Get from simulation" button, it will run a short sim and extract the available parameter names and populate the list to pick from. Because you're setting this up before simulation, it doesn't yet know what the available parameters are.

    This inserts the following line in the netlist:

    save I0.I0.PM0:gm I0.I0.PM0:vdsat 

    (I had selected gm and vdsat). 

    These results appear in the results browser in the appropriate place in the hierarchy. You can also use the "plot" checkbox on the ADE form to get them to be plotted automatically, or you can use the ot button in the calculator to retrieve the results. Or you can use the results browser.

    If they're not in the "tran" output, and the tran "folder" is empty (which seems strange to me), then maybe you have some strange settings on the Outputs->Save All form, but I can't see how you'd do that either!

    The spectre output log should record some information about the number of things saved too - so maybe you need to look at that too.

    Regards,

    Andrew.

Children
No Data

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.