You have to switch models of all the device types to mc (Monte Carlo) section (in case of Spectre) or use special MC models. It depends  on the design kit. Sometimes  MC model is a section of a transistor spectre model and sometimes it is  kept in separate file. Check up the design kit documentation.

Thanks a lot for your reply. I am using UMC 65nm RF CMOS technology and they have specialized MC models. I am adding that in model file before MC analysis.

The MC model use "sigma" variable. The variable have to be defined by user.

One more remark.

Generally, there can be following reasons of your problem:

Hello Zbigniew,

I have used sigma=3. I checked the model file, MC model has got separate mismatch and process file and that are coded. So I checked in detail → print statistical parameters. In that I checked for few samples in which I could see it is taking different values for Vth and mobility under process and mismatch variations. So model point of view I think it's fine. Yet I am asking for few clarification regarding MC analysis.

1> How do we go about MC analysis? Whether we have to start from some definite seed, where we have to do some trial and error and find out which seed gives the best? I think in my case, it may be generating all those samples which are very close, so all the samples' response is concentrated in one point.

2> What is child analysis? Whether every general analysis such as DC, AC, Tran, SP etc. are called child analysis?

3> How samples are taken when I have selected a child analysis. Ex: When I am varying temperature from -10 to 100 Deg C, each other samples are considered at which temperature? It is important because response is a scalar quantity and don't know those responses are w.r.t which temperature value.

4>How to plot or record responses for AC, Tran, SP etc for different samples ? Ex: I want my resulted current to be plotted w.r.t temperature along the x-axis but for different MC samples.

5>What is “number of bins” means in histogram plot? 

Thanks & regards,

Vinay Rao.

HI,

Well, I suggest you look into the Cadence documentation. If you cannot find there an answer to your question you may try Cadence Forum:  http://community.cadence.com/cadence_technology_forums/f

Concerning the number of bins: http://en.wikipedia.org/wiki/Histogram

Regards.

hi,

what are the model files for montecarlo simulations file need to inculde. If any idea about the path then please let me know.

Hi, the problem is, as you can see in your figures, there are some outliers. So the bin with is too large and all your correct samples are summed together in the first bin. I suggest to check the cases, where the current is above 20uA. You can do that by looking up the point number in the "detail" view on the results tab in adexl. Than just simulate this point again. You can do that by setting the "starting run number" in the monte carlo options.

hi vinay rao,

can you please explain how u r using sigma =3. in virtuoso ADE i m not getting where to set sigma for montecarlo run.

@Zbigniew: Yes it solved many of my doubts. Thanks for your reply. Here is the cadence forum link where Andrew and I discussed about those issues.

http://community.cadence.com/cadence_technology_forums/f/38/t/31490

@Marko: Thanks for your reply. I could figure out why I wasn't getting Gaussian. Out of 100, 2 samples fell far outside from the mean that made all the other 98 samples (which are near to mean) to fall in a single bin. When I have selected sigma=2.5, those two samples were ignored and then I got the gaussian form.

@Shilpi singh: Which foundry you are using? Check out the foundry document for that particular transistor which you are using to see what type of file they are providing for MC simulation.

@Sauvagya: It is just a normal variables add.

Go to ADEGXL -> Tests -> ADE XL test editor -> variables -> Name (you type as sigma) -> Value (type as 3) -> add -> ok.

hi vinay,

thank u fr ur information, can u send some pdf assisting montecarlo simulation to set sigma value in cadence

Sauvagya: You might be interested in the following video.

https://www.youtube.com/watch?v=CyiiB4jbl5c

Hi,

It seems that the statistical distribution of the models is not turned on.

In the documentation that goes with the Process Design Kit (PDK) that you are using (Model Reference Guide, README file where models are located, Design Manual, or similar document), there should be a description on what variables have to be set in order to use the statistic variations of the models parameters. 

If you write what technology/PDK you are using, somebody who is familiar with it may be able to give more specific directions.

Thank you!

@Dobromir Georgiev: Thanks for your kind reply. As I stated, I could figure out why I wasn't getting Gaussian. Out of 100, 2 samples fell far outside from the mean that made all the other 98 samples (which are near to mean) to fall in a single bin. When I have selected sigma=2.5, those two samples were ignored and then I got the gaussian form.

Hi Vinay,

Sorry, I didn't see that there are actually additional columns in the attached PDF as the hits were so little, and obviously didn't read your description carefully.

I cannot be sure what is happening, but here is a guess:

In the Monte Carlo analysis the inputs usually are generated using a Gaussian distribution, but this doesn't necessarily mean that the output will also be Gaussian. i.e. if we consider running MC analysis on a plate capacitor, where the distance (d) between the plate is varied, the capacitance is C = e0*er*A/d;

As e0, eR and the area (A) are actually constant we can simplify:  Cnom = c0/d. Cnom is the nominal value of the capacitance, c0= e0*er*A and 'd' is the distance between the plates.

If we take two points equally spaced from the nominal value of "d" - (d-0.5d) and (d+0.5d), C is not equally spaced:

C(-)=c0/(d-0.5d)=c0/0.5d=2*Cnom - this gives 100% increase from the nominal C. 

as opposed to

C(+)= c0/d+0.5d)=c0/1.5d=0.66*Cnom - this gives only 33% decrease of the nominal C.

And if we consider the extreme case of d-d and d+d, we get

C(-)=c0/0=infinity, C(+)=c0/2d=0.5*Cnom.

So in his case the histogram for C is skewed, and the skew is greater as the standard deviation 'd' increases.

I suppose that in your case, for a certain value of T, you hit such a case where the function that is monitored has extremes. 

From your MC results you can check for what temperature you get the large unexpected deviation, and run analyses on your circuit for that temperature, to figure out what may be wrong.

Thanks!