parametric sweep in PSpice

[Brian Leibowitz]

I finally figured out how to perform sweeps (and nested sweeps) of design
parameters in PSpice. It was very non-trivial, so I am sending this to the
class in case anyone wants to use PSpice for the homework (it is very
helpful in a lot of ways, but requires a bit of getting used to). If you
have never used PSpice before, you probably won't want to try it for the
first homework, but it can be a huge time saver in the long run. If there
is a large demand from people who have never used PSpice before, I might
arrange an hour or two to show people the basics.

Hope this helps.

Brian

Example:
========
We want to generate a family of Id vs Vds curves for several different
device lengths.

Solution:
=========
1) Create the schematic and a global parameter called "length".
- I assume you are familiar with schematic entry in PSpice
- Place an instance of "PARAM" from the parts library, this is necessary
to create parameters in PSPice.
- Double click on the "Parameters" instance in the schematic, and enter
"length" for name1 and "0.35u" for value1 (no quotes). This is
equivalent to ".param length=0.35u" in HSPice.
- Double click on the transistor you want to control. Enter all
numerical attributes normally, but for the L attribute enter
"{length}".
IMPORTANT: you must use the curly braces!! This took me a very long
time to figure out (it was not documented - I just made it up).

2) Set up the nested sweep.
- From the menu, choose Analysis->Setup and then click on "DC Sweep".
- Enter the information for the inner sweep first (i.e., the Vds sweep).
To do this, select "Voltage Source" as the sweep type, then enter
the name of the voltage source at the drain and the sweep parameters
in the appropriate fields.
- Click on the "Nested Sweep" button to enter the outer sweep (device
length) info. Select "Global Parameter" as the sweep type, then
enter "length" (no quotes or curly braces this time) in the name
field and the rest of the sweep parameters below.
IMPORTANT: make sure you check the "Enable Nested Sweep" box.
Also make sure the "Enabled" box next to the DC Sweep button is
checked in the main analysis type box.

3) Run the simulation and display results.
- Choose simulate from the Analysis menu and PSpice will run and the
Probe program will start to analyze the results.
- In Probe, press the insert key or choose Trace->Add from the menu.
Select ID(M1) if the transistor was called M1 and press return.
The desired family of curves should appear.