Stats

  • Locked Locked
  • Replies 13
  • Subscribers 66
  • Views 20152
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Group noise contributors

seppo2

Hi guys,

When you do print->noise summary after a noise sim or pnoise sim, is there a way to group noise sources together; either by block or device?

In the case of an extracted list, if you have a number of fingers for a transistor, the noise simulation gets broken down into each individual finger. It's difficult to read what a device contribution is if it is broken down into 100 individual sources of noise!

 The same idea would be handy to work out the total contribution from a block.

 Perhaps it is about time you update the noise summary feature in ADE... :) 

Cheers,

Seb 
PS: While I am at it, could you also include noise summaries for input referred noise!  

  • Dear Seppo,

    If you are simulating your circuit with APS from the ADE, there is an option in the ADE under the Setup->High Performance Simulation dialog box with an option called "Preserve Instance". You can select "None" "All" or "Selected". When "All" or "Selected" (choosing your device of interest) is selected this will group the parallel devices together I believe and report the operating point data for the combined device.

    I have not recently tried the option  with a noise analysis, but ypu might consider it.

    Shawn

  • I've tried that and it doesn't help. It also depends on how the extraction deck deals with transistor fingers, so if it is netlist that way in extraction then it doesn't matter what you do in the simulator.

    If anyone has any other ideas, please share!

    Where do you place PCR?
    I really think it's about  time Cadence updates ADE to support a better noise summary. They've had the same thing since I first started using Cadence...

  • Actually we are introducing a hierarchical noise summary (grouping by subckt, at least) in IC616 ISR7/MMSIM13.1 ISR7. We had planned to introduce this some time ago but there was a problem with the implementation and it got put on hold until recently.

    For other things, asking for enhancements in a public forum won't help you. You need to go to customer support at http://support.cadence.com and then we can file an enhancement with R&D on your behalf.

    Regards,

    Andrew. 

  • Thanks Andrew!
    Good to hear.

    Hope all is well.

    Cheers,
    Seb
     

  • Yes thanks Andrew. Grouping by subckt will be a very useful feature. I look forward to trying this out.

  • Hello all, I am not an RF designer but I am looking for the noise grouping function in Cadence for mixed-signal design as well. I am able to plot output noise PSD [V^2/Hz] with the VN2() function. I am also able to plot a noise PSD of individual contributors to the output noise, if these contributors are single devices in the schematic using for example VNPP("/R1" "total"). But when I try to apply the VNPP function to a schematic block, I get a 'noise data not available' message. How can I plot a PSD of noise contribution of a chosen schematic block to the total output noise PSD? Thanks.

  • Hi Peter,

    The hierarchical noise summary information has been implemented, but it's only available via the Results->Print->Noise Summary form. The way it works is that you specify the hierarchy level number, and it then calculates the sum of the noise contributions for each subckt and puts this in a new output database - the noise summary form then uses this to give the spot noise or integrated noise for the instances at that level.

    So you can't use VNPP because it doesn't create the noise sums for all instances in the hierarchy - it's done on-demand and only for an individual level of hierarchy.

    You should contact customer support for a way to do this cleanly, but if you want to plot the noise power spectral density for a particular instance, bring up the Results->Print->Noise Summary form, and then set the "hierarchy level" in the filter to 1 or above (the default is blank). If you set it to 1, you'll get all the top level instances, and on. All you need to do is pick the hierarchy level, and then the result database is updated - no need to OK the form.

    Then you can either use the results browser to navigate to the "noisesummary" database and you can find the instance and within it you'll find a "sum" item that you can plot.

    You can then also use the expression: getData("I0.I1:sum" ?result "noisesummary") in the calculator.

    However, remember that this database only gets generated when you've picked the hierarchy level on the noise summary form - it won't happen automatically at the end of a simulation. It's a workaround at least though!

    Regards,

    Andrew.

  • Hi Andrew,

    thanks for the reply. Maybe I have an older version of Cadence (this is IC6.1.6-64b.500.5).

    If I do ADE ->Print->Noise Summary I see settings available for the choice of types of instances for the filter (include all types/include none) and include/exclude instances. I do not see the 'hierarchy level' setting.

     

    Peter

  • Hi Peter,

    That's ISR5 - if you look up the thread, you'll see that I mentioned that this was introduced in ISR7 (so that would be IC6.1.6.500.7). You'd need to move to a later hotfix to access this functionality.

    Kind Regards,

    Andrew.

  • Hi Andrew,

    I switched to IC6.1.6-64b.500.8 now and still can not see the 'hierarchy level' setting in the filter in ADE -> Print -> Noise Summary.

    Is the functionality implemented only for 500.7?

     

    Thanks.

    Peter

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.