Output resistance of current mirror - Simulation Setup

[melkord]

I usually use small signal formula to calculate output resistance (method 1).
But now want to find a simulation setup to measure it (method 2) so I do not need to input the expression of rout.
A good discussion I found from here and here.

I still do net get the same result between method 1 and method 2.
Could someone give me their correction to my setup?


Result.

The testbench.

The output transistors.

 

[solidstate]

M0 is in triode, I suppose that should be fixed first.

Then, are you sure you can use ±1.2V bipolar supplies here? It looks to me like those are 1.2V devices.
M1 Vdb might be way too high at the moment?

 

[melkord]

M0 is in triode, I suppose that should be fixed first.

Then, are you sure you can use ±1.2V bipolar supplies here? It looks to me like those are 1.2V devices.
M1 Vdb might be way too high at the moment?

Here is the simulation result when both transistors are in saturation.
Still I got different results.

 

[solidstate]

And how about the second point?

 

[melkord]

And how about the second point?

The bulk is connected to -1.2V, that is not a mistake.
Here is the simulation when VBS of cascode transistor = 0V and VB of bottom transistor = 0V.
Still the results are not the same.

 

[solidstate]

Thanks! The small signal calculation looks reasonable. Not sure what is going on.
Could you try to remove L0, C0 and V0 (the current source), apply an AC stimulus to V1 and re-run the sweep? Then, take 1/i(v1) as your output impedance and compare?

 

[melkord]

Thanks! The small signal calculation looks reasonable. Not sure what is going on.
Could you try to remove L0, C0 and V0 (the current source), apply an AC stimulus to V1 and re-run the sweep? Then, take 1/i(v1) as your output impedance and compare?

Still, they are different.
This setup seems make sense, but I do not understand where I did the mistake.

 

[solidstate]

At this point, I also don't understand.
Can you annotate gds? It is worth checking that gds = 1/rout
Also, can you post the full schematic of Current_Source?

 

[melkord]

At this point, I also don't understand.
Can you annotate gds? It is worth checking that gds = 1/rout
Also, can you post the full schematic of Current_Source?

Confirmed that gds = 1/rout.
The ideal opamp is from VerilogA.

 

[solidstate]

Oh boy... I hope you're not trolling? The gain of the amplifier improves the output impedance... search for regulated cascode or gain-boosting...

Here I was expecting to see some basic cascode bias stack...

 

[melkord]

Oh boy... I hope you're not trolling? The gain of the amplifier improves the output impedance... search for regulated cascode or gain-boosting...

Here I was expecting to see some basic cascode bias stack...

Ooops..honest mistake. I am not trolling and was not aware that the output impedance was multiplied.
I know regulated cascode for TIA and didnt thought it is the same case here.
I will derive the small signal analysis tomorrow.
Thank you!

 

[solidstate]

No worries, glad we cleared it up.
One other thing you could look at is increasing the target Vds and/or the L of the bottom devices.
Right now, the Rout of your cascode is higher than that of the current source itself -- I think that's quite unusual.