You can add additional commands to extract and plot this. In my example, I am extracting this from device M3 which lies inside subckt X_OPAMP1. Here is the syntax.
.EXTRACT DC LABEL=GM_OVER_ID_M3 GM(X_OPAMP1.M3)/ID(X_OPAMP1.M3)
.PLOT EXTRACT EXTRACT(GM_OVER_ID_M3)
Here is a screen shot of the dialog box.
Sorry, it has been awhile since I've been able to get back to this. I'm still having issues. My netlist is painfully simple:
.CONNECT GROUND 0
* Component pathname : $ONC18/devices/default/nmos1p8v [ELDOSPICE]
* .include /opt/onc18_1_10p3/onc18/devices/default/nmos1p8v/onc18__nmos1p8v
* MAIN CELL: Component pathname : $ONSEMIEVAL/test/gm_id
X_MN1 VIN VIN GROUND GROUND onc18__nmos1p8v lg=0.18 wg=10 ng=1 ss=0
+ sd=0 sf=1 lg2ctd=0.16 lg2cts=0.16 ad=0.202 pd=1.8 as=0.202 ps=1.8 custom_ds=0
+ matched=1 analog_prec=0 mult=1 parasitics=1 m=1
Now, if I try to enter in a similar expression as to what you have:
.EXTRACT DC LABEL=GM_OVER_ID GM(X_MN1)/ID(X_MN1)
.PLOT EXTRACT EXTRACT(GM_OVER_ID)
I get the following error:
Warning 916: Unable to parse expression . OBJECT "X_MN1" not yet defined.
I get it for each time I use X_MN1.
What am I doing wrong?
Your instance is named X_MN1. That leading "X" means it is a subcircuit. Your include statement is probably including a subcircuit model for an NFET. That will complicate things a bit.
First, confirm that your onc18__nmos1p8v model is a subcircuit. Assuming it is, chances are that there's a MOSFET and a few sources, capacitors, and whatnot inside the subcircuit. Take note of the instance name of the MOSFET in this subcircuit model. I'll pretend it's got a really original name like nmos1.
So, assuming you've confirmed you are using a subcircuit model, you'll need to modify the statements a bit. You'll want to use the subcircuit drain port current for ID. Take note of what your subcircuit model calls the drain port; hopefully, it's sensibly callled d. Using the names I'm assuming, the extract statements you need should look more like this:
.extract dc label=gm_over_id gm(x_mn1.nmos1)/i(x_mn1.d)
.plot extract extract(gm_over_id)
Take a look and hope you don't have to deal with series or parallel devices in the model.
Thanks for the advice! I'm new to Eldo and hadn't used a flavor of Spice in quite awhile, so I forgot that X indicates a subcircuit. That was indeed my issue, and now I'm able to simulate what I need to.
Thanks for the tip Vernon. Most devices models are now subckts and you have to use the syntax that references the actual device inside the model. I am glad that you got this working. Please come back again if you need further help.