# Plotting MOS device parameters as function of time (revisited)

From Prakash I received comments on two older posts with respect to the plotting of transistor small-signal parameters as function of time. I think it is worth mentioning them in a separate post. His e-mail is posted at the end of this post.

The concept is generally speaking that we want to plot the transistors transconductance as a function of time. Why? Well, normally we do a lot of characterization at the DC point; we linearize the operation of our nonlinear circuit and investigate its properties at that point. However, in reality, the voltage levels and operating points vary a lot with different conditions, modes and time.

Some people might solve this by doing DC sweeps and plot the transconductance as a function of the different DC values. This gives the designer a pretty good view of what’s happening with the gm and gain of the amplifier over different conditions.

In other cases, there might be more dynamic components and we might have to investigate the gm as a function of time (which also opens for the option to do XY plots for the gm as function of gds or other obscure things like that.

There were two old posts on the topic (deliberately no pretty-printed links):

And I have taken the liberty to do a couple of edits to the original e-mail (not marked).

Hi Jacob,

For my dynamic comparator circuit, I was trying to plot the MOS device parameters (gm, cgd) against time for transient simulation. I found one method for that in your blog (https://mixedsignal.wordpress.com/2010/12/09/cadtransient-gm).

The method described in the blog uses the ‘infotimes’ option in the transient analysis form in ADE. For that we need to run a script to generate the list of time instants. Also in this case, the oppoints of all devices in the schematic are saved are the specified time instants.

An easier and more convenient way is to use the same technique as described in another post on your blog (https://mixedsignal.wordpress.com/2009/12/28/oppoints/). But in this post, the use of the technique for Transient Simulation is NOT emphasized.

I have used the following method to get device parameters for the transient simulation:

1. Create an `.scs` file which specifies the devices for which oppoints are to be saved. One needs to be careful while specifying devices in subcircuits. In my file, I use

``` save HSDoubleTailComp.MnInpP.m1:oppoint ```

Dots are used to traverse the hierarchy of circuits. Depending on the PDK `'.m1'` may or not be required.

2. Add this `.scs` file to your path using `ADE->Setup->Model Libraries`
3. After running the transient simulation, one can get to the required parameters in `'tran-tran'` section of the Results Browser. For e.g, the gm is obtained as
```getData("HSDoubleTailComp.MnInpP.m1.gm" ?result "tran-tran") ```
4. One of verifying this result is to use infotimes option and plot the gm value using OPT
` OPT("/HSDoubleTailComp/MnInpP" "gm") `

Curves from step 3 and step 4 should now match.

For getting device parameters from transient simulation, the `*.scs` file option is more convenient than the infotimes method since

• a) It avoids running/modifying a script to generate list of time instants, especially if the duration of transient simulation undergoes frequent changes
• b) It saves only the oppoints of the required devices. This will help to save disk space when large schematics are being simulated

Regards

Prakash

This site uses Akismet to reduce spam. Learn how your comment data is processed.