I am trying to get an idea as to what a device model parameter represents.
Can anyone please suggest where i can get the list for it.
I am specifically looking for the parameters like mobility, Cox,
subthreshold factor, TC of threshold voltage, Vth0 of the device etc.
Also i am trying to plot the threshold voltage of a device as per my DC sweep parameter. Can anyone please tell me how should i do that?
Did you consider reading the documentation? There's a whole manual on the device model equations, plus documentation on the parameters available for each mode. Run "cdnshelp" from <MMSIMinstDir>/tools/bin to get to the documentation.
If you want to plot the threshold voltage, the best thing to do is to create an include file, called (say) save.scs with the contents:
and then reference this file from Setup->Model Libraries or Setup->Simulation Files. Then you can see this parameter from the Results browser after your dc sweep. Of course, change M1 to be whatever the device name is in your case.
In reply to Andrew Beckett:
I went through this thread and am interested in plot vth through DC sweep. But I received this warning：
WARNING (SPECTRE-8282): `M1a' is not a device or subcircuit instance name.
WARNING (SPECTRE-8287): Ignoring invalid item `M1a:vth' in save statement.
WARNING (SPECTRE-8282): `M6' is not a device or subcircuit instance name.
WARNING (SPECTRE-8287): Ignoring invalid item `M6:vth' in save statement.
I am sure the name is correct and is copied from schematic instance name field.
Do you know how to fix it?
In reply to Alex Liao:
Presumably the name is not correct, or you've not given the correct hierarchical path to the instance. Look at the netlist itself - that's the best bet.
You can refer my snap cut. The naming is correct. I do not know how to check that hierarchical path. But the netlist is enough I think.
The transistors you're trying to save the vth for are inside the _sub0 subckt, and you didn't tell it the hierarchical path to them. Since there is only one instance of that subckt, ie instance I0, you'd need:
(assuming that the model pch is not a subckt itself).
In my case I have seen that subckt _sub0. But wher is the instance info? As you exampled, the instance I0, what is the only instance name in my design from previous snapshoot?
All I did was read your netlist in your post. It's not difficult!
I have no warning now. I assume that I have saved vth of M6 by including "save I0.M6.vth". But this thread mentioned plot this variance by DC sweeping. How can I plot it with the help of result browser. You can point it out direct in this figure .
Firstly it would be "save I0.M6:vth" (note the colon) - check the spectre output as it will tell you if you have got it wrong.
Secondly, you're looking at the dcOp output there, not the dc sweep output. That's the (initial) DC operating point. You'd need to look in the "dc-dc" output in the results browser, and then you should be able to plot a waveform of I0.M6:vth versus the swept parameter.
Thank you so much. Now I have my desired plot.
I am trying to plot Vth vs L like the same manner as described in your post. I gave a variable name in length field of transistor and chose dc analysis. In that i selected design variable as sweep variable and added the variable name. But when im running the simulation i am getting the following error. Even if i give save M0:vth , im getting error and in the results browser (dc-dc) there is no Vth of the tansistor. Please help me in this regard.
In reply to Arjun RP:
Please read the forum guidelines - these tell you not to double post (especially when you already have your own thread on this subject). I answered your other post here.