Designer’s Guide Community

lunren

Community Member

Offline

Posts: 82
Asia

Anyone who is familiar with cadence ADE 5.0.33.144
May 24^th, 2006, 11:39pm

Dear all,

1. I used pss+pnoise to simulate the phase noise of my VCO in cadence ADE 5.0.33.144. However, after the simulation finished, I can not find a proper way to view the phase noise curve. Because according to the paper "VCO Design Using SpectreRF Application Note", I should "click Results--Direct Plot--Main form", but in ADE 5.0.33.144, there is no "Main form" in Results menu. So I resorted to Results Browser and Calculator in Tools menu. I got a phase noise curve. But the Y axis unit is dBm. How can I get a dBc/Hz unit for the phase noise curve?
2. Normally, what's the rational magnitude order of VCO phase noise, for example should be less than...?

Back to top

Best Regards,

Lunren

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Anyone who is familiar with cadence ADE 5.0.33
Reply #1 - Jul 24^th, 2006, 1:37pm

There should be a Results->Direct Plot->Main Form menu. If not, somebody has customized your Analog Design
Environment menu.

That version is quite old - IC5033 is no longer supported, and the version you have is the Base release of it (i.e. with no hotfixes applied).

You didn't explain how you used the calculator to get the results, so we have no way of knowing what calculation you did.

And I didn't understand your 2nd question.

Regards,

Andrew.

Back to top

IP Logged

smlogan

Community Member

Offline

Posts: 52
Boston, MA

Re: Anyone who is familiar with cadence ADE 5.0.33
Reply #2 - Jul 29^th, 2006, 7:21pm

Hi Lunren,

After running the pss and pnoise simulation, use the ADE menu item Tools->Results browser. Navigate to the /schematic directory below the ADE. If you highlight schematic, you will then see the subdirectory /psf. Beneath psf, there is a directory listed "pnoise-pnoise". Highlighting this directory will show an output "out". If you import this into the calculator by clicking on "out", you may obtain and plot the phase noise (in dBc/Hz) by using the function "20dB" and clicking on "Plot" in the calculator. To add the phase noise output to ADE, use the menu Outputs->Setup... and in the resulting dialog box, click on the button "Get expression" alongside the "Calculator". This will import the function and output from the calculator. You may then name it something like "Phase noise" and hit the button "Add". This will add the phase noise output to your existing list of outputs.

In answer to your second question, there is no one "good" value of phase noise at a particular offset frequency to shoot for. The requirements of your circuit and its system requirements will dictate the required phase noise through its phase jitter , BER or other system parameter specifications. The analysis to derive the required phase noise at a specific offset frequency may not be unique. There may be many phase noise templates that achieve the required level of system or circuit performance.

Let me know if I've managed to understand your questions! Feel free to ask for clarifications!

Shawn

Back to top

Shawn

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: Anyone who is familiar with cadence ADE 5.0.33
Reply #3 - Jul 31^st, 2006, 12:47pm

Shawn,

The method you describe is not calculating the phase noise. It is calculating the output noise in dB - you have not taken into account the magnitude of the carrier. So it will only be phase noise if you happen to have a carrier with 1V RMS amplitude (I think that's right, from memory).

That is what the phaseNoise() function does. It divides the output noise by the RMS amplitude of the output signal, and then does db20 on that.

Regards,

Andrew.

Back to top

IP Logged

smlogan Community Member Offline Posts: 52 Boston, MA	Re: Anyone who is familiar with cadence ADE 5.0.33 Reply #4 - Jul 31^st, 2006, 12:58pm Hi Andrew, Thank you. I stand corrected! Shawn
Back to top	Shawn IP Logged

tumeda

Community Member

Offline

Posts: 37

Re: Anyone who is familiar with cadence ADE 5.0.33
Reply #5 - Sep 7^th, 2006, 9:47am

lunren
In the old version, I also use the following formulation to get the phase nosie. I am not sure whether it works in 5.0.33. The function in calculator is
# phaseNoise(1, "pss-fd.pss", ?result "pnoise-pnoise") #
BTW, the method posted by smlogan is the way to get output noise.

Andrew Beckett:
I have also similar problem in Cadence IC5.1.41USR2 version.
In the main windows, I can only plot output noise. If I try to plot phase nosie, there is error message
" *Error* Evaluating expression (phaseNoise(1 "pss_fd" ?result "pnoise")).
*Error* ("difference" 1 t nil ("*Error* difference: can't handle (drwave:204771448 - nil)")) "

From the error message, the above formulation seems to be changed to
# phaseNoise(1 "pss_fd" ?result "pnoise") #.
I also tried to use the function phaseNoise in calculator, it didn't work also.
Could you give me some tips, how to get the phase noise through Calculator in the IC5.1.41USR2 version.
Thanks a lot in advance!

Back to top

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: Anyone who is familiar with cadence ADE 5.0.33 Reply #6 - Sep 12^th, 2006, 1:25pm The method I always recommend (mainly because I can never remember the right expression), is to use the direct plot form, and then use the "add to outputs" checkbox/button on the form. Then you can steal the expression used from the outputs pane in ADE... Andrew.
Back to top	IP Logged