I have a problem with the use of RFDE mom symbol view in Cadence schematic. The image is attached below for reference. The momentum block is basically a MOM capacitor for coupling ac input . In theory, there should not be any drop in the 3KOhms resistance connected to the gate of the transistor in one end and the capacitor on the other end. This entire block works fine if I simply remove the MOM model with an ideal capacitor from analoglib. In that case, I see no drop across the 3K Ohms resistance. But when using the MOM model, it simply destroys any gate biasing that I try to put. What is the problem here? and how can I get a work around it?
This is a dc analysis and shows the current and voltage at each node.
Given that Momentum is a tool from Keysight (not Cadence) and I don't know which version of Virtuoso, Momentum, or Spectre (assuming that it's spectre you're using as the simulator - you didn't say that either), it's quite hard to give a definitive answer.
So, assuming that the simulator is spectre, can you post what the lines in the input.scs look like for I741 (the highlighted component above)? Also can you mention the versions of the tools you're using?
This is a fresh simulation where I removed everything else. I am using ADS 2016.01, MMSIM15.10.627 and IC6.17.704
Here is the spectre simulator data from the input.scs file for the below schematic
PORT0 (net70 0) port r=50 num=1 type=sine freq=100G dbm=0
R3 (net70 net03) resistor r=1u
R2 (net06 net42) resistor r=1u
R1 (net42 net010) resistor r=3K
R0 (Amp_Vdd Drain_device) resistor r=100
V4 (net010 0) vsource dc=550.00m type=dc
V0 (Amp_Vdd 0) vsource dc=Vdd type=dc
I405 ( net03 0 0 0 net06 0 0 0) nport interp=linear \
and the mommdl/text.text file is an S parameter file generated for the momentum block I405 (schematic below)
Please let me know if you need any other data.
1. The MoM component does not have an option for interpolation method. I just get a warning when running the DC analysis. It says "Risky extrapolation to DC of data given in S-parameter file". I tried the nport from the analogLib with the "bbspice" as the interpolation method and also selecting the option "Extrapolate to DC". The problem still persist and I still see a drop across the resistance connected to the gate.
2. As it takes a long time to simulate, the lowest point is at 80 GHz. Like you suggested, there is no DC point in the file. Is there anything that I could add into the S Parameter file?
3. I did the simulation with linear sweep and a step size of 1GHz.
4. It does not throw any complaint about passivity or causality.
Well, I think it's a little optimistic for any model to be built which will simulate at DC and in the time domain if the lowest simulation point you ran in Momentum was at 80GHz! How the spectre is supposed to know that the capacitor is open circuit at DC (after all, it doesn't know it's a capacitor - all it has is the s-parameters). I nearly fell off my chair when you said the minimum frequency is 80GHz!
A 1GHz step is pretty big too.
I'm not sure we can help much more without seeing the data, but to be honest I think the main problem is that the s-parameter data is missing too much low frequency and even high frequency data, plus is too sparse.