Noise analysis

[dan1988]

Hello,

When using the noise analysis to determine the noise for a potential divider consisting of two 100k resistors in series the results obtained were as expected.

 When using the noise analysis to determine the noise for a potential divider consisting of a 100k resistor in series with a 200k resistor the results were not as expected (100k connected to power supply, 200k conneted to ground). We would expect the 200k resistor to have V_N²  double to the 100k. It is actually shown as half. When the 200k is swapped for a 300k it is a third smaller than the noise voltage for the 100k when we would expect it to be triple. The figure for the 100k is what we expected from our hand calculations using the formula V_N² = 4KTBR.

 All resistors have the same temperature and all settings on the noise analysis are default other than the bandwidth being adjusted to 1Hz - 1MHz. The input noise reference source is VV1 (the only power supply in the circuit), output node is between the two resisters and the reference node is 0.

Further inconsitancies appear when using a power supply connected to a 100k connected to a 200k connected to a 300k connected to ground. When the output node is selected between the 300k and 200k the results are all as expected but when the output node is betwwen the 100k and the 200k the results are all very strange. (or the other way around, the point is they're inconsistant)

 We are not saying the figures are wrong as we have limited experience in this field and were using it as a learning exercise, but the figures are not what was expected, can this be explained? or corrected by changing the configuration/ options of the analysis?

Best regards,

Dan

[Maxish]

Hello,

Please attach your circuit and specify the exact numbers you expect

Thanks,



 

[dan1988]

Using V_N² = 4KTBR

Bandwidth 1-1MhZ in multisim. I just used 1 x 10^6 in my calculator but this will not effect the results in the way experienced.

Temperature = 300.15K

Output node = 1

Reference node = 0

Input noise reference spurce = vv1

Expected results:

Inoise_total_rr1 = 1.657 nV²

Inoise_total_rr2 = 3.314 nV²    (so double the noise for r1 as would be expected before even puching the figures into a calculator, in my opinion)

Inoise_total = 4.971 nV²          (noise values for r1 and r2 added together)

Onoise total = 2.209nV²  (standard potential divider calculation on sq.root of Inoise_total then squaring again to get V² format multisim provides)

Mutlisim results:

Inoise_total_rr1 = 1.658 nV²     (as expected)

Inoise_total_rr2 = 828.787pV²    (half of r1 not the double I was expecting)

Inoise_total = 2.486nV²    

Onoise total = 1.105nV² 

I ran through my method of calculating using multisims individual component noise conrtibutions and came out with the same inoise and onoise totals.

Best regards,

Dan

[Maxish]

Hello,

Your analysis is incorrect. Check out

http://ecircuitcenter.com/Circuits/Noise/Noise_Analysis/res_noise.htm

its a great example of how noise analysis in SPICE works.

For your values:

Power_noiseR1=1.656e-9
Power_noiseR2=3.312e-9

The noise power at output is the sum of individual noise sources.
Power_output=Power_noiseR1 * Gain1^2 + Power_noiseR1 * Gain2^2

where Gain1 is gain from R1 noise source to output and Gain2 is gain from R2 noise source to output

Power_output=1.656e-9 * (2/3)^2 + 3.312e-9 * (1/3)^2= Multisim result

note that "noise_totalR1" is not simply R1's noise source

[KostasB]

Hi Dan

The tutorial that Max sent explains very well the noise analysis in SPICE, however I noticed that in Multisim the results are not as expected.

I am in contact with the EWB support with regard to the issue and I will get back to you as soon as I hear from them.

Regards,

KostasB

Applications Engineer

National Instruments UK & IE

[dan1988]

Hello,

Thanks a lot for your help. Could i just clarify a few things please.

I understand how to find the output noise now, I was going about it the wrong way.

If I wanted to find the individual noise powers how would I get multism to show me? I thought that was what onoise_total_(resister name) would tell me.

How would I get multisim to show me the total noise for the circuit? I thought onoise_total would show me this, if it is how would I calculate it? if it isnt what is it actually telling me?

Mant thanks,

Dan

[KostasB]

Hi Max

Just to clarify:

Output variables "onnoise_total_RES" and "innoise_total_RES" are not simply the noise source equations for the respective resistor. They refer to that noise source reflected to either the Output in case of "onnoise_total_RES" or to the Input in case of "innoise_total_RES". Therefore, the simulation results are correct.

If you want to calculate custom expressions rather that the ones already built in Multisim, you can use the Simulate>Postprocessor

after you run a simulation.

I hope that helped,

KostasB

National Instruments UK & IE

[dan1988]

Hello,

Sorry, I know it was a while ago now, but would you be able to tell me what results from multisim weren't as expected. Was it the entire noise out for the circuit or the individual noise conrtibutions?

Using the method suggested my noise out matched that provided by multisim, so I just wanted to check that result was ok.

Best regards,

Dan

[dan1988]

Apologies for that, I have re-read your later replies and seen "Therefore, the simulation results are correct".

Thank you

[swsw]

Hi,

I am trying to do a noise analysis just like what is shown from the noise analysis example from the help menu in multisim. I followed exactly the same process as what is shown. However, when I simulate my circuit, I do not see the noise spectral density plot as what is shown from the example. I got an empty graph with just the printed values. Can anyone help me?

Thanks,

Marlin