Cadence Monte Carlo Simulation

[eryilmazcg]

Cadence Monte Carlo Simulation - PTM Model

Hi,

I am trying to make monte carlo simulations with PTM model files. As attached to this post,
I have added this quoted lines to my model file. The cellNMOSwidth is the parameter for the width
of the bottom nmos of regular 6T sram cell, as can be guessed. This is working and results are
as expected. BUT, If i put for example toxe (which is parameter defined for nmos in model file,
it can be checked from attachment ) to place of cellNMOSwidth, it does not work, I cannot make it.
It gives me error "toxe is not a parameter". Yes I know indeed it is not in the parameter list, it is obvious when I create my whole netlist.
But I need to play with those parameters, and I dont know how to make it work.

Secondly,
My aim is to play with oxide thickness... and I thought toxe or toxp are related to oxide thickness.
Can anyone also inform me whether I am true or not?

statistics{
process{
vary cellNMOSwidth dist=gauss std=12 percent=yes
vary cellPMOSwidth dist=gauss std=12 percent=yes
}
mismatch {
vary cellPMOSwidth dist=gauss std=24 percent=yes
}
}

Many Thanks
-CG

 

[erikl]

I guess you've seen the Cādence Monte Carlo simulation tutorial?

Try the method described with nmos_rgfac on pp. 9..13 with nmos_toxfac and pmos_toxfac as multipliers for toxe.

BTW: toxp is the physical gate oxide thickness, toxe the electrical gate oxide thickness, adapted to best fit the analyses.

 

[eryilmazcg]

I guess you've seen the Cādence Monte Carlo simulation tutorial?

Try the method described with nmos_rgfac on pp. 9..13 with nmos_toxfac and pmos_toxfac as multipliers for toxe.

BTW: toxp is the physical gate oxide thickness, toxe the electrical gate oxide thickness, adapted to best fit the analyses.

Well.. the thing is, in that example in the tutorial, a nmos is defined -modeled- with its resistance, and that nmos_rgfac is chaged to approximate resistance values of drain, source, etc.. this is what I understood from it.
Here i dont use formulas, i give required width and lengths, other than that nothing. cadence just compiles according to model file and simulates. but for some transistor i want to change toxe value which is they are synthesized, to accomplish parameter variations as can be guessed...

I am kinda stuck right now...
Any other suggestion?
Thanks for the reply btw

 

[erikl]

I meant like the nmos_rgfac example shown. First, create the parameters

parameters nmos_toxfac=1.0
parameters pmos_toxfac=1.0

Then, within the process and/or mismatch sections, use:

        vary    nmos_toxfac     dist=gauss  std=0.10
        vary    pmos_toxfac     dist=gauss  std=0.10

For std always use values <1 .

Then, in the PTM model file, change the toxe parameters in the nmosx & pmosx models to

toxe = 9.5e-010 * nmos_toxfac
resp.
toxe = 1e-009 * pmos_toxfac

Hope this helps!

 

[eryilmazcg]

Thanks, now i got it working. I did not think that I could change -multiply- model parameter with a variable. Thank you.
Yea I know I should use less than 1, i was using percentage scale.
Many Thanks
-CG

 

[eryilmazcg]

Erikl, there is one more question. I tried to find the parameter definitions for the ptm model. So far I could not find the info.
I need to know which parameter is related to dopant densities. Is there a list for the parameters, and the definitions for it?

Thanks
CG

 

[erikl]

Re: model parameters' explanation

I need to know which parameter is related to dopant densities. Is there a list for the parameters, and the definitions for it?

Try the BSIM manuals!

 

[eryilmazcg]

Re: model parameters' explanation

Lately I have a big concern of reliability of this technique. I mean is it totally correct to apply such a technique to have process variation?

This question has been rosen because of the fact that some of the professors that I know have suggested that this type of process variations cannot be done perfectly in spectre.
Those professors are mostly working on physics of transistors and researching about them.

All in all, my concern is correctness of this type of application in cadence.

Thanks in advance Erikl
-CG

 

[erikl]

I mean is it totally correct to apply such a technique to have process variation?

If the fab/foundry provides process variation figures for their process, this will usually be the result of a long experience and extracted measurements on many wafer lots - otherwise those figures wouldn't make much sense.

... the professors that I know have suggested that this type of process variations cannot be done perfectly in spectre.

Always ask: why? They should give you a reason for their opinion.

And there's no reason why SPECTRE couldn't do it - it's just another type of simulation tools which all can fiddle with MC simulations.

Perfectly is another thing: tools can just work as well as the figures are which they are fed with.

Those professors are mostly working on physics of transistors and researching about them.

Then they should know!