CMRR, PSRR Simulation

[Gundam]

Hi all, just quick question here. I am using the simulator Spectre. I
am wondering if there is any direct setting or build in function to
simulate CMRR and PSRR for an amplifier design. The way I did is to
set up common mode and differential mode signal source to simulate and
have their gain ratio. Similar way is for PSRR. Is there any other
faster or more automatic method in Cadence? The other quick question
is to simulate input referred noise. I plot the input noise
distribution throughout the whole frequency band, and I just integrate
over the frequencies of interest to get a number. Does it make sense
or there is another better way in Spectre simulator? Thanks for all
feedback.

 

[Riad KACED]

Hi Gundam,

I'm not aware of any calculator/ocean built-in function that does the
measure of the rejection ratios as you are looking for.
The automated way I could see to make this is to write an ocean script
and measure the gain of your output at the desired frequency.
Let's see what others would go for ...

Cheers,
Riad.

 

[Andrew Beckett]

Riad KACED wrote, on 09/17/08 23:05:

Hi Gundam,

I'm not aware of any calculator/ocean built-in function that does the
measure of the rejection ratios as you are looking for.
The automated way I could see to make this is to write an ocean script
and measure the gain of your output at the desired frequency.
Let's see what others would go for ...

Cheers,
Riad.

I would strongly recommend using "xf" analysis to do this rather than "ac"
analysis. With xf analysis you specify the output nodes (or current probe) and
it will allow you to access the gain from each source in the circuit - so in the
same simulation you can see the gain from the power supplies and from the input
signal. There's no need to set an "ac magnitude" on any source.

If you do it via "ac" analysis, you have to keep changing the source which has
got ac magnitude (often set to "1") in order to find the gain from that point to
the output.

Then computing the rejection ratios should be a relatively straightforward
calculation.

Regards,

Andrew.

 

On Sep 18, 6:45 am, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:

I would strongly recommend using "xf" analysis to do this rather than "ac"
analysis. With xf analysis you specify the output nodes (or current probe) and
it will allow you to access the gain from each source in the circuit - so in the
same simulation you can see the gain from the power supplies and from the input
signal. There's no need to set an "ac magnitude" on any source.

If you do it via "ac" analysis, you have to keep changing the source which has
got ac magnitude (often set to "1") in order to find the gain from that point to
the output.

Can you adapt somhow "xf" analysis to compute rejection ratios in a
fully-differential architecture?
I am right now using "ac" analysis because I have to compute among
others:

; CM input
vsc = (VF("/vs+") + VF("/vs-"))/2

; CM and DM outputs
vod = VF("/vo+") - VF("/vo-")
voc = (VF("/vo+") + VF("/vo-"))/2

; Common-mode gain
Acm = voc/vsc

; Common-mode-to-differential-mode gain
Acmdm = vod/vsc

Thanks.
Kind regards,
Marco

 

[Andrew Beckett]

marcoballins@gmail.com wrote, on 09/24/08 18:48:

On Sep 18, 6:45 am, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm
wrote:
[...]
I would strongly recommend using "xf" analysis to do this rather than "ac"
analysis. With xf analysis you specify the output nodes (or current probe) and
it will allow you to access the gain from each source in the circuit - so in the
same simulation you can see the gain from the power supplies and from the input
signal. There's no need to set an "ac magnitude" on any source.

If you do it via "ac" analysis, you have to keep changing the source which has
got ac magnitude (often set to "1") in order to find the gain from that point to
the output.

Can you adapt somhow "xf" analysis to compute rejection ratios in a
fully-differential architecture?
I am right now using "ac" analysis because I have to compute among
others:

; CM input
vsc = (VF("/vs+") + VF("/vs-"))/2

; CM and DM outputs
vod = VF("/vo+") - VF("/vo-")
voc = (VF("/vo+") + VF("/vo-"))/2

; Common-mode gain
Acm = voc/vsc

; Common-mode-to-differential-mode gain
Acmdm = vod/vsc

Thanks.
Kind regards,
Marco

Hi Marco,

This could be done - but you'd need to have single signal sources that you could
use to represent vsc - a matter of how you organize your testbench. Also, you'd
probably need a vcvs to get the "voc" equivalent (vod is no problem, because the
xf output is a pair of nets).

In other words, providing you have a source to set the common mode level, and
maybe a source for the differential input, it should be doable. But you might
find it easier to do with AC in this case, although you then have to keep moving
your "AC" source between runs.

Normally the problematic case for xf/pxf type analyses is when you have
quadrature inputs, rather than differential, as you can't really reformulate
them into single signal sources.

Regards,

Andrew.