noise sim always report 0% of Total

Please contact customer support.

Andrew

You have so many small noise contributions that each of them is 0.00% of the total noise power when you round the percentage to two decimal places: (3.31025e-8/5.68804e-6)^2=3.38685e-5=0.00338685%

Thanks Frank - I should have spotted that.

Andrew

Hi, Frank, thanks.

Now I understood what's happening. I have 7 ployR resistor, each resistor has 999 segments and in the noise analysis above, somehow, each of the segments are separated into 4 sub-segments again. So it's total 4*999*7 segments

sqrt((3.31e-8)^2*999*4*7)=5.54e-6, which is close to total of 5.68e-6 V noise as shown above.

Here is two following up questions.

1. is there a way to combine the small segments together in display? For example, combine the 999*4 segments belonging to R44 report as one row instead of 999*4 rows, I tried the setting in the noise summary page but was not successful

2. I tried to set the % of total from 2-digit to 4-digit using the command below, but as you see, I have the error. Let me know which is the right command to do it.

Dear monglebest2,

monglebest2 said:

1. is there a way to combine the small segments together in display? For example, combine the 999*4 segments belonging to R44 report as one row instead of 999*4 rows, I tried the setting in the noise summary page but was not successful

I am not aware of a way to combine resistor segments. There are ways to combine currents for a mult-fingered MOS device, but I have not seen anything similar for combining the noise contributions of resistor segments from an extracted view based netlist. Off hand, this seems quite difficult as the extracted view will also contain segment speciifc via and trace resistances associated with a given resistor segment that will add to the noise of each resistor. It seems they should be included in the net resistance noise. I am not sure how spectre has sufficient information to be able to combine the parasitic resistance elements of each segment with the resistor segments.  However, there are others who follow these forums with far more knowledge than I who might have an answer to this question.

monglebest2 said:

2. I tried to set the % of total from 2-digit to 4-digit using the command below, but as you see, I have the error. Let me know which is the right command to do it.

I think you might be missing a backtick in your "int" syntax if I managed to read your screenshot from the CIW. I do not see one prior to "int". . However, one is required as detail in the On-line support article at URL:

https://support.cadence.com/apex/techpubDocViewerPage?xmlName=explorer.xml&title=Virtuoso%20ADE%20Explorer%20User%20Guide%20--%20Plotting%20and%20Printing%20-%20Noise%20Summary&hash=pgfId-1048767&c_version=ICADVM20.1&path=Explorer/ExplorerICADVM20.1/chap9.html#pgfId-1048767

So, for example, to set the number of digits to 4, the CIW version of the syntax is:

envSetVal("asimenv.noiseSummary" "percentDecimals" ’int 4)

Shawn

Thanks, Shawn. It turns out the command I copied from Cadence help, which shown below, has that backtick in front of int wrong. I missed that information. Thanks for your insight. 

envSetVal("asimenv.noiseSummary" "percentDecimals" ?int 4)

Dear monglebest2,

monglebest2 said:

t turns out the command I copied from Cadence help, which shown below, has that backtick in front of int wrong. I missed that information.

Great! At you made at least 50% progress towards your two posed problems! Thank you letting us know!

Shawn

There is now an option to consolidate the noise from iterated instances, but I don't think that's the situation here - the main issue is that the tool doesn't really know there's a relationship between all these resistors that should be summarised in some way.

Andrew