gm/gds , intrinsic gain plot for transistor using spectre/ADEL

This has come up countless times before (I'm sure you can find this info with a bit of searching), but here's a very quick outline.

1. Outputs->To be saved->Select OP Parameters
2. Click on the transistor - you'll see in the ADE window a new tab showing "Save Operating Points" and you'll see a row with that transistor.
3. You can then type in the list of operating point parameters you wish to save in the "Operating Points" box for the row containing your transistor (e.g type 'gm gds' (without the quotes, space separated).
4. Alternatively click on the "..." button, click "Get from simulation" which will run a rapid simulation to retrieve the available operating point params that you can select from a lost
5. Set up your dc sweep (assuming you're doing a dc sweep)
6. Run the simulation, and then in the calculator use the "os" (if dc) or "ot" (if transient) buttons, click on the transistor and then pick "gm" or "gds" from the list, and build up your expression - e.g. OS("/M0","gm")/OS("/M0","gds")
7. You can click on the "gear" icon with a green left arrow to send the expression back to the ADE outputs so that it can be plotted automatically

Andrew

Thanks for the reply Andrew, this is very helpful. I was able to replicate the steps you have mentioned.

Only thing that remains now is to have VGS-VTH on the X-axis instead of VGS that I have presently in the DC sweep.

As of now I am doing the DC sweep against the DC voltage source on schematic with DC voltage variable as VGS

any suggestions on how can I make the X axis as VGS-VTH ?

May depend on the models being used as to the parameter name, but suggest you also save vth as well as gm and gds for the transistor. Then create a second output in ADE called (say) VGS_VTH with an expression like this:

xval(OS("/M0" "vth")) - OS("/M0" "vth")

The xval will give you the swept variable (VGS in this case) and you're then subtracting vth from the transistor from it. Plot the two curves, and you'll get gmOverGds and VGS_VTH both versus VGS. Now move your cursor over the x-axis, and click right mouse->Y vs Y. Choose "VGS_VTH" as the trace and plot in a new sub window. This is the curve you want. If you want to have it as an output in ADE to be plotted automatically, you can build the waveVsWave expression like this:

waveVsWave(?x VGS_VTH ?y gmOverGds)

and then add that as an ADE output.

Andrew

Thank you very much Andrew, this is very helpful .

one last thing in terms of plotting -

I am trying to generate plots like the following :

You should be able to use an expression such as pv("/M0" "w" ?result 'instance) to get the width (check in the results browser under the instance results database to see what the parameter names for the transistor are - it shows wt on the schematic, but it might have been mapped to something else). Then you can build the expression for ID/W in a similar fashion to VGS-VTH and plot versus that.

Andrew

thanks a lot Andrew, this was very helpful

Hi Andrew,

is there something similar to "OS " & "OT" for AC analysis ?

sidm said:

is there something similar to "OS " & "OT" for AC analysis ?

No, because that would make no sense. The AC analysis results are from a linearised representation of the circuits around an operating point, so showing the operating point parameters during an AC sweep would be pointless (since they don't change). I guess in theory they could change if you swept something that affected the operating point and ran at a single frequency, but then you could do the same thing with a DC sweep to get the operating point parameters.

In the email notification it was also asking about this expression 

(mag(i("/T0:d" ?result "ac")) / mag(i("/T1:d" ?result "ac")))

but you seem to have deleted that from the post now. The first thing to have checked (and you may have done that now) is to check the individual results before trying to divide them. In this case you're mixing schematic names (which begin with a "/" and use "/" as a hierarchy separator, and netlist names (which use "." as a hierarchy separator, and ":" for currents). So that will always fail. You should probably have used either:

(mag(i("/T0/D" ?result "ac")) / mag(i("/T1/D" ?result "ac")))

or

(mag(i("T0:d" ?result "ac")) / mag(i("T1:d" ?result "ac")))

(the first is a guess as to whether the pin names are D on the symbol).

This also depends on you having saved the currents through the terminals too.

Andrew.