Noise analyses in Cadence for differential Op-amp

One way would be to have a source across the differential input (provided the common-mode level is set correctly for the differential inputs), or you could use voltage-controlled voltage sources (vcvs) to apply the same input signal to both differential inputs but with one inverted (you might need in that case to have a gain of 0.5 on each of the two vcvs to avoid doubling the magnitude of the input signal). Then in the noise analysis measure the output noise across the differential output, and tell it that the input source is your single-ended voltage source.

Andrew.

Dear Mr. Andrew

Thank you very much for your reply, I attached you the image of the setting according to your explanation so you can see it please.

do you mean by the Source is an AC source ? if its yes then what should be sitting of this source or it doesn't matter.

What about if I connect the two differential inputs only to the common mode voltage and tell the simulator it is my source of noise.

As I understood from your kind explanation that I only need to run the noise analyses in cadence.

But I am sorry I didn't understand why I should set the gain to 0.5 of my VCVS, if you look please to my image where I usually set the gain to -1 so I get two equal and out of phase signals to the input of the operational amplifier, if I make it 0.5 the signals will not be the same

Thank you very much once again

That would work. It doesn't matter what the source setting is (you might set it to be an ac source for an ac analysis, or a sine source for a transient analysis; for the noise analysis it really doesn't matter though). Setting the gain to 0.5 was only a suggestion because otherwise the signal amplitude between the left ends of the two R1 resistors will be twice the magnitude of the input source, and so if you're input referring the noise back to the input source, there's potentially an extra gain factor of 2. Of course, if you use your circuit as-is, then you can't use gain of 0.5 because then you'll have a larger signal going into the negative input than the positive. To have a gain of 0.5 you'd have to have a vcvs on each of the two inputs and have your input source separated from the rest of the circuit. 

You can't just use the common-mode source as the input source because otherwise the input referred noise would be computed by finding the output noise of the circuit and dividing that by the common-mode gain. The purpose of identifying the input source when computing noise is to allow the transfer function from that source to the output to be computed, and then the output noise is divided by that to find the input-referred noise.

Regards,

Andrew.

Dear Sir,

Thank you very much for your explanation, It is very clear for me now the input setup of the circuit.

Your suggested connection of two VCVS will be very useful for me when I do transient analyses, if for example when I want to measure the closed loop gain from the transient I have to subtract Vin+ from Vin-, but with this connection there will be no need when I refer to the source signal directly.

I just plotted the circuit again according to your explanation.

Please Sir I have related two other questions, in fully differential amplifier do we refer to the noise for each output separately ? or there must be an expression for them together as like when we express the fully differential gain we refer to (Vo1-Vo2), but here in the noise simulation setup we are only telling him one output

my second question is what is the worst gain configuration for simulating the noise (IRN).

Thank you very much once again

These setups might be simplified by using the ideal_balun component from the analogLib library, which is described in the paper "A Test Bench for Differential Circuits".

Unknown said:

Please Sir I have related two other questions, in fully differential amplifier do we refer to the noise for each output separately ? or there must be an expression for them together as like when we express the fully differential gain we refer to (Vo1-Vo2), but here in the noise simulation setup we are only telling him one output

my second question is what is the worst gain configuration for simulating the noise (IRN).

Since you can specify a pair of nodes in the noise analysis, you'd specify the output noise as being across the two outputs not the two outputs separately (relative to ground).

I don't know what the worst case gain configuration for noise in your circuit would be - that's likely to be circuit dependent.

Andrew.

Dear Mr. Frank,

Thank you for your reply,

For the moment I would like to continue using the VCVS as I didn't find the balun in my analogLib,

I read the attachment you send and I think I cam make an equivalent to the output balun by connecting another VCVS to the output with gain = 1.

Still please I am wondering about my other questions in my former post.

Thank you once again

ideal_balun has been in analogLib since at least IC614 (I don't have older versions to test at hand) but it wasn't in the very old IC5141 release. Perhaps you're using that - this is why we ask people (in the forum guidelines) to specify which tool versions they are using.

I think you posted about the same time as my last response so you may not have seen my answer to one of your questions.

Andrew.

Dear Sir,

Thank you very much for your response, 

for my case the Balun instance is located at rflib, I can see it from server but I don't know how to add it to the library manager, However I will search to do it.

Now the setup is clear for me, as you said, if I am simulating the noise for single ended then I will specify one output node, for the fully differential I will specify the two outputs in the noise simulation setup as two output nodes.

It means my application tell me which gain I should consider as my worst case, but by any way the noise analyses only performed under closed loop condition

Thank you very much once again

Add this into your cds.lib

DEFINE rfLib $(inst_root_with:tools/dfII/bin/icfb)/tools/dfII/samples/artist/rfLib

This is if using IC5141. For IC61X you'd replace "icfb" in the above with "virtuoso". The component in rfLib (balun_ideal) is not quite the same implementation as ideal_balun in analogLib, but it would have the same effect. That said, there's no particular benefit over using the vcvs approach that you've used right now.

Regards,

Andrew