Noise figure of differential signal

First of all, you do not need to specify the RF input port as a large signal input (in fact you shouldn't) - that will be generating the noise figure in the presence of an interfering large signal. So keep it as DC. You need a port because the port generates noise (because of the resistor in the port - I can't see if you've altered the impedance of the port, but if you set that to 0 or messed with the noise temperature that could also impact whether the port generates noise. The signal part (for signal to noise) is OK, because the noise analysis essentially calculates the noise at the output of the circuit in response to all the noise contributors in the circuit (including the port). Since you also told it where the input was, it can also compute the transfer function to the output from the port - with this, it (effectively, because it doesn't really compute it this way) can compute the ratio of the signal to noise at the input (for an arbitrary signal level) to the signal to noise at the output (i.e. the arbitrary signal level multiplied by the transfer function to the noise at the output).

However, I think the fundamental problem is that this is a mixer, and you're using the noise analysis. That's not going to give you any useful answer with a mixer as the noise analysis computes the noise from a DC operating point. This circuit doesn't have a useful DC operating point where the mixer is actually operational - you would need to simulate a period of the LO with pss or hb, and then compute the noise using pnoise or hbnoise. You'd specify the output and input port as before (still a DC source), and specify the reference sideband on the pnoise/hbnoise as 1 (you can choose this by frequency, but it's to specify that the input frequency is at 10.1GHz and that's the transfer function it uses). The output noise sweep would be from 1Hz to 10GHz (or maybe a little less than 10GHz because you'll potentially get infinite flicker noise at an exact multiple of the LO).

You should then use the Direct Plot->Main Form too to compute the noise figure. 

This is covered in the workshops I pointed you to before in your last post.

Regards,

Andrew.

Andrew Beckett said:

First of all, you do not need to specify the RF input port as a large signal input (in fact you shouldn't) - that will be generating the noise figure in the presence of an interfering large signal. So keep it as DC.

i have a DC source  separately Biasing the transistor as shown bellow. 

if i understand you correctly for NF calculation purpose i  have defined my RF port  as DC small signal (100mv) port as shown bellow.

after that 

Andrew Beckett said:

you would need to simulate a period of the LO with pss or hb, and then compute the noise using pnoise or hbnoise.

I have defined my PSS simulation to work on both LO signals. over 1 (100psec) period with 10 harmonics(you said previously that 5 is not enough for square wave)

as shown bellow.

after that i did hbnoise  and i got a PSS response but the NOISE FIGURE option is disabled, as shown in the end.

where did i go wrong?

Thanks

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**********************************************************************************************************************************************************************

**************************************************************

Several problems (did you look at the tutorial I suggested? I don't think so from what you're doing here):

1. You cannot mix pss and hbnoise. You have to use pnoise with pss, and hbnoise with hb. This would have been clear in the simulator log file which would have told you that the hbnoise couldn't be run. It would have shown:
   

   Error found by spectre.
   ERROR (SPCRTRF-15225): The hbnoise analysis was skipped because a HB analysis must be run first.

   Analysis `hbnoise' was terminated prematurely due to an error.

2. The number of harmonics is more critical with hb analysis (or PSS in harmonic balance mode) because it's a frequency domain analysis and it controls the size of the solution. With harmonic balance, the number of harmonics is the number of harmonics in the fourier series representing the solution. Shooting PSS uses a time domain approach and represents the solution as a time domain waveform which will naturally follow the signal - the number of harmonics then mainly controls the number of output harmonics if you look at the PSS solution in the frequency domain - it doesn't really affect the accuracy significantly.
3. For the RF analyses you always use the Direct Plot->Main Form. The Noise Figure on the Direct Plot menu is only for standard non-periodic "noise" analysis. However, it won't show up either in this case because the hbnoise will have failed to run. You would expect to see "hbnoise" or "pnoise" on the Main Form (or similar) to see the noise figure.

Please do work through some of the tutorials - this forum cannot be a training class on how to use the tools. RF simulation is always more complex than non-RF simulation and so it's important to get some training (ideally) or read the documentation/tutorials to better understand how to do things properly.

Regards,

Andrew.

Yes, i have been working with several manuals the one you recommended and similar to them.

the best manual that also fits the way you advised me is in the linked manual.

but it contradicts your advise ,because you  said that i should convert my RF port into small signal DC port.  as shown bellow.

i have succeeded creating a Noise figure plot , and i got the result i planned for.  but i am not sure regarding the DC source.

because we actually eliminate the RF source of the mixer and put a DC source instead . so how its still the same

the 10.1 doesnt show anywhere? we only have the LO , LO _not source and the DC port source?

Thanks

(setting the input port source type  to DC disables the production of waveforms for the large signal analysis)

Tran,pss qpss,hb

**************************************************************************

*****************************************************************************

I'm not sure why you're trusting a random manual on the internet which is not applicable in your case. I keep pointing you to our tutorial which is maintained, current, and tells you how to do the simulation for a mixer. The manual you were looking at was specifically for an amplifier, and was talking about measuring the noise figure when the input signal is large enough to cause nonlinear behaviour - similar to what you might do when you have a large signal blocker.

Usually you measure the noise figure assuming that the input signal is small (i.e. small enough to be well below, say, the 1dB compression point) - that way it will not saturate the circuit and cause a difference in noise response. 

In that (usual) situation, you would not have a large signal input to your mixer, and only have the LO enabled in the PSS simulation. As I have said before, you do not need your 10.1GHz input signal to be present. If you look at the noise figure at 100MHz, that is telling you the noise figure assuming an input signal at 10.1GHz because that would be refsideband*PSSfund+Fout (so 1*10G+100M). There is no need to have a large signal present in the simulation for this to be done.

Since the noise figure is Sin/Nin (at the input) divided by Sout/Nout (at the output), if we multiply the top and bottom of the input S/N by gain (where gain is the transfer function to the output at a specific frequency that you want to measure), then that is:

(Sin*gain)/(Nin*gain) / (Sout/Nout)

Since Sout is Sin*gain (it's the signal at the output), that would be:

(Sin*gain)/(Nin*gain) / ((Sin*gain)/Nout)

Rearranging and cancelling, that ends up being Nout/(Nin*gain). The simulator already computes the output referred noise from each noise source (including the input port), so that's straightforward - although it only includes the noise coming from the input port at the desired input frequency (that's why it needs the reference sideband to get the correct noise contribution). There's no need to have a time-varying input signal present to do this calculation.

Regards,

Andrew.

Andrew Beckett said:

There is no need to have a large signal present in the simulation for this to be done.

Hello, my RF port is not large signal.its sine amplitude is 100mv.

only my LO signals are large signal, i will be glad to know what is your definition to large signal to avoid misunderstanding.

i am using the following spectreRF workshop which title shown bellow.

Thanks

So your signals are almost certainly small enough that you do not need to specify it as a sine source for the pnoise/hbnoise analysis, as I've said several times already.

You appear to be using a pretty old version of Spectre (if that workshop is from the spectre version you're using). That will have been release about 13 years ago - which makes no sense. I'm slightly confused as you were using harmonic balance earlier, and that was not available in that version of Spectre. I would strongly recommend using the workshop from the version of spectre you're actually using (since it's in the installation). If you're really using MMSIM6.0, please use a newer version - we don't release a new major version every year just for the fun of it!

Regards,

Andrew.

Got it :-) thank you very much.