Simulation of opamps in Cadence

Again, these are fake (non-silicon, just how "real" when there's nothing to "fit"?) devices / models, right? I advised a closer look at FET I-Vs to see if the problem is "from above".

A thing to look at, is whether the S, D diodes have any model properties populated, and whether individual devices have junction area and periphery props set, to scale them for C and (you wish) leakage. Also, a realistic FET will have channel leakage from the surface states (NFS in older models, dunno what yours look like). If your sub threshold slope looks "too good to be true" then maybe it is.

• There is no proper connection in current mirror
• Transistors are biased by voltage
• The circuit is suppose to be a high gain OTA, while no feedback is present.

All above means it is not working and it is normal behavior.

dick_freebird said:

Again, these are fake (non-silicon, just how "real" when there's nothing to "fit"?) devices / models, right? I advised a closer look at FET I-Vs to see if the problem is "from above".

A thing to look at, is whether the S, D diodes have any model properties populated, and whether individual devices have junction area and periphery props set, to scale them for C and (you wish) leakage. Also, a realistic FET will have channel leakage from the surface states (NFS in older models, dunno what yours look like). If your sub threshold slope looks "too good to be true" then maybe it is.

Click to expand...

Good afternoon, dick_freebird! I really appreciate both of your responses. To be honest, I am not entirely sure what do you mean by the sentence: "A thing to look at, is whether the S, D diodes have any model properties populated, and whether individual devices have junction area and periphery props set, to scale them for C and (you wish) leakage." Can you please explain in little bit more detail what do you mean by that? As you mentioned, the I-V characteristics are the first thing I haven taken a look at even before testing this very circuit. (To be honest these ones I tested for gpdk090 and not for this one). They look a the one I would expect yo see from a short-channel devices.

Dominik Przyborowski said:

• There is no proper connection in current mirror
• Transistors are biased by voltage
• The circuit is suppose to be a high gain OTA, while no feedback is present.

All above means it is not working and it is normal behavior.

Click to expand...

Thank you, Dominik, for your response! You are absolutely right regarding the CM connection - I was just stacking on transistors for this technology to see if Spectre gives any reasonable dc op for the analysis. That might actually be a problem which is sometimes really hard to detect when one focuses on the cascode but not the basics. However, I can not really agree on two other notices regarding the circuit. Yes, transistors are biased by voltage rather then a current. The reason comes from the previous thread. The voltages I have peaked up has been generated through a successfully-tested beta-ratio multiplier for gpdk090. The sizing for the other technology, as well as bias voltages and supply stays the same. I do not want to say that I would expect 45nm tech behave the same as 90nm even with the same sizing - just to troubleshoot the error in spectre or model files by switching to the other technology. Regarding the third bullet point I would rather partially agree then disagree. The reason for that is that I would like to see the open loop gain of the opamp first before putting in in a feedback configurations. Even though open-loop gain is tested by stb analysis for a fully-differential configuration, which is the case for me, the first thing to do before starting on checking the specs is a simple dc op, which, again, I have been trying to do here. I would like to see some reasonable overdrive across all the devices in cascode and the output slopes to get a zero-order's estimation for the gain. Or have you meant the common-mode feedback?
Anyways, thank you so much for help!

My thinking is that a circuit should still "solve" to "something" even if hooked up wrong. The convergence problem says maybe too little conductance somewhere, insane gain or polystable circuit operation (hysteretic, latching).

Maybe the issue-set is changing shape as we go. But gross convergence problems are bad news for design progress and maybe a manifestation of "GIGO".

theguardian2001 said:

Yes, transistors are biased by voltage rather then a current.

Click to expand...

MOSFETs are biased by current through current mirror. This is the only way to bias any MOSFET properly. Even simplest CS amplifier has to be biased by current through current mirror, while signal is DC blocked. By voltage, you can bias BJT not MOSFET.

theguardian2001 said:

The reason for that is that I would like to see the open loop gain of the opamp first before putting in in a feedback configurations.

Click to expand...

It is not possible to get OL gain with no feedback configuration as OTA cannot be biased in proper operating point.

theguardian2001 said:

the first thing to do before starting on checking the specs is a simple dc op, which, again, I have been trying to do here. I would like to see some reasonable overdrive across all the devices in cascode and the output slopes to get a zero-order's estimation for the gain.

Click to expand...

Again, with no feedback (both differential and CMFB) you cannot expect any results. The input range of differential pair is around 50mV (depending to it OP). With 80dB OL Gain you have to set differential voltage between inputs with 1µV accuracy only because of gain. Any difference will strongly affect current in both OTA branches results in different OP of OTA transistors. You can play like this for long time getting nothing valuable.

Do things in proper way. You are getting errors in simulations not because something is wrong with gpdk (both gpdk090 and 45 are mature and well tested even if they are not real process) or simulator, but because testbench is wrong.

Start from single ended version in unity gain configuration. Then expand it to fully differential.

Dominik Przyborowski said:

MOSFETs are biased by current through current mirror. This is the only way to bias any MOSFET properly. Even simplest CS amplifier has to be biased by current through current mirror, while signal is DC blocked. By voltage, you can bias BJT not MOSFET.

It is not possible to get OL gain with no feedback configuration as OTA cannot be biased in proper operating point.

Again, with no feedback (both differential and CMFB) you cannot expect any results. The input range of differential pair is around 50mV (depending to it OP). With 80dB OL Gain you have to set differential voltage between inputs with 1µV accuracy only because of gain. Any difference will strongly affect current in both OTA branches results in different OP of OTA transistors. You can play like this for long time getting nothing valuable.

Do things in proper way. You are getting errors in simulations not because something is wrong with gpdk (both gpdk090 and 45 are mature and well tested even if they are not real process) or simulator, but because testbench is wrong.

Start from single ended version in unity gain configuration. Then expand it to fully differential.

Click to expand...

That makes sense. I am completely agree that transistors should be biased with a curret rather then a voltage. However, I am not really sure if that makes a difference for the simulator. Please correct me if I am wrong: When a current is passing through a diode-connected device, it generates the gate-source voltage needed for this device to maintain the same current; thereafter this gate-source voltage can be applied to the gate of the other device one can expect the second transistor to reproduce the mentionedd current. The voltages I am applying to the gates were previously generated by this circuit, which has been successfully tested.
I tried to remove this circuit from the cellview and expected that it might be easier for cadence to converge the solution.
So, my question can be rather formulated like the following: Does it make the difference in that very case if one inserts the full bias circuit to the opamp's schematic or if one just inserts the dc sources with dc voltage equal to the corresponding ones from the bias circuitry?
Anyway, I will actually start the verification with the steps that you have mentioned. Thank You a lot, Dominik!

Hello, everybody! I have tried to start the simulation by connecting the opamp in unity-follower configuration with the single-ended output and using the biasing circuitry instead of constant dc sources. I tried to do it with gpdk090 since I had a biasing circuitry for this technology sucsesfully tested from before. However, Spectre faces even more convergence problems with such a setup compared to the version with constant sources. I am not really sure what I am doing wrong in that case

Based on the log file I would guess that the problem spectre is facing is instability to find a suited operating point. At the same time one knows that a follower configuration is the worst one for stability and one may not use the opamp as a buffer. So I would pretend to say that having an unstable opamp in a buffer-connection does not automatically mean that it can not be used with some other feedback (f. e. resistive), isn't it?

Attached netlist is incomplete.
You are using global nets in subcircuit but not on the top level, so there is no supply connection in the instance I10. At least according to attached screenshots.

Something is fishy also, as in log spectre is complaining on lack of dc path between net Vip and 0. Looks like some nets are floating for some reason. It might results with some strange conditions for model, what could end up with shorts.

1. Make supply nets global
2. add nodeset for your biasing circuit (startup circuit is working in transient, not in dc)
3. and please attach full netlist

Dominik Przyborowski said:

Attached netlist is incomplete.
You are using global nets in subcircuit but not on the top level, so there is no supply connection in the instance I10. At least according to attached screenshots.

Something is fishy also, as in log spectre is complaining on lack of dc path between net Vip and 0. Looks like some nets are floating for some reason. It might results with some strange conditions for model, what could end up with shorts.

1. Make supply nets global
2. add nodeset for your biasing circuit (startup circuit is working in transient, not in dc)
3. and please attach full netlist

Click to expand...

Good afternoon, Dominik and thank you for your reply! Yes, the supply connections have been messed up. I changed all of them to global ones which can be seen from the netlist. This time I extracted the whole one

I have also added a nodeset and removed the start up circuitry from the bias cell. I have checked with one of my previous simulations of the bias circuitry before and set nodes according to the derived op. However, after these manipulations the output log file looks exactly the same with the only exeption for an instance name of a bias cell since it has been modified. I am completely agree with you regarding the lack of dc path even though "Check and save" has not shown any missing connections/floating nodes. Plese see the full netlist and updated log file in the attachements.

As always, I would be happy to hear anny suggestions.
Thamk you in advance.

There is something fishy.
If you could try fix the dimensions (Length and Width parameters does not help in netlist readability as they are forcing netlister to print all model conditional equations).
→ I am not sure if model is in proper w,l range.
The design is using 1V devices, while the VDD in netlist is set to 1.8V. If you would lower it to 1V.
There is only V0 source present in netlist, it means that gate of PM1 is floating. It might be also reduced to ground, but it is not clear. What voltage is suppose to be set on Vip net? If not 0, then try to set instance preservation to all (in GUI can be found in high-performance simulation → simply enable instance preservation and use * for all).

V0 source is trying to pull 65TA (tera!) of current, so circuit behaves as ideal short on voltage source. This current is then generating huge voltage drop on every resistance in the circuit and simulator is lost. It might be caused by:

1. input to the model which is beyond it range (too small or too large dimensions)
2. Vdd beyond range of model
3. something else

Try to limit current by adding 1Ω resistor in series between V0 source and VDD! net.

These kinds of things are why I recommend that
OP spends the effort to validate the models given.
Especially, that a lonely transistor doesn't "blow up"
when terminal voltages are overranged.

I thought it might be possible that a 1V device
-would- blow up outside where anybody might've
looked.

You could try (say) making all devices 1.8V and
if that changes the outcome, maybe leads you
somewhere.

Back when I worked for a RFIC company I watched
Cadence and UC Berkeley bicker for months over
whose fault it was, that the BSIMSOI compact
model would "blow up" when our FDSOI "I type"
FETs reversed voltage. When voltage passed
through zero the FET code divided by zero.

Held up our switch design teams for months
while they played a blame game.

Trust? Can't trust the top dogs, with manpower
and money like mad. I'll be holding onto doubt
about academic teaching exercises and whether
they drive out all error before it gets to you.

Dominik Przyborowski said:

There is something fishy.
If you could try fix the dimensions (Length and Width parameters does not help in netlist readability as they are forcing netlister to print all model conditional equations).
→ I am not sure if model is in proper w,l range.
The design is using 1V devices, while the VDD in netlist is set to 1.8V. If you would lower it to 1V.
There is only V0 source present in netlist, it means that gate of PM1 is floating. It might be also reduced to ground, but it is not clear. What voltage is suppose to be set on Vip net? If not 0, then try to set instance preservation to all (in GUI can be found in high-performance simulation → simply enable instance preservation and use * for all).

V0 source is trying to pull 65TA (tera!) of current, so circuit behaves as ideal short on voltage source. This current is then generating huge voltage drop on every resistance in the circuit and simulator is lost. It might be caused by:

1. input to the model which is beyond it range (too small or too large dimensions)
2. Vdd beyond range of model
3. something else

Try to limit current by adding 1Ω resistor in series between V0 source and VDD! net.

Click to expand...

Hi, Dominik! Thank you for your reply. I have actually taken a look at the netlist and saw that the voltage at the gate of PM1, which is the plus input terminal of the opamp, is missing. Even though the voltage source remains on the schematic, it does not apper in the netlist even after recreating it from ADE Explorer window. I have also set the supply voltage to 1V, which I have tried to do before, it does not reduce the ammount of warnings in the log file and I do not see any significant difference between these two cases. I have also found high-performance simulation by going to SetUp in ADE Explorer->High-performance simulation and I see this window:
I am not entirely sure if that is what you've meant? To be honest I have not heard about these options before and I should probably try to read documentation on what it is doing. Also attaching the updated log file in case one sees any improvements. I am also not sure regarding the model dimensions that you have mentioned. I am sure that dimensions can not do below that the minimum width or length specified by the technology itself (f.e. the one I see for 90nm - 100nm is the minimum dimension). All the ratios are scaled with respect to this number and intuitively I would say that ratios 90/5; 45/5; 5/1 present in my circuit are pretty usual for sub-micron designs, aen't they?

dick_freebird said:

These kinds of things are why I recommend that
OP spends the effort to validate the models given.
Especially, that a lonely transistor doesn't "blow up"
when terminal voltages are overranged.

I thought it might be possible that a 1V device
-would- blow up outside where anybody might've
looked.

You could try (say) making all devices 1.8V and
if that changes the outcome, maybe leads you
somewhere.

Back when I worked for a RFIC company I watched
Cadence and UC Berkeley bicker for months over
whose fault it was, that the BSIMSOI compact
model would "blow up" when our FDSOI "I type"
FETs reversed voltage. When voltage passed
through zero the FET code divided by zero.

Held up our switch design teams for months
while they played a blame game.

Trust? Can't trust the top dogs, with manpower
and money like mad. I'll be holding onto doubt
about academic teaching exercises and whether
they drive out all error before it gets to you.

Click to expand...

Hi, dick_freebird and thank you for your reply! The thing is that me and other students have been working with this technology before and nobody faced any errors as far as I remember. I remember sucsesfully designing an opamp with gpdk090 even with 5V supply and not using any cascodes (which I guess is even worse in terms of "blowing up" the transistors since more voltage has to fall on an individual device between Vdd and gnd). The only difference for me now is (maybe) the version of the technology and cadence version (6.15 vs 6.17)