Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Monte Carlo Analysis in Cadence

Status
Not open for further replies.
S

suria3

Full Member level 5
Joined
Mar 5, 2004
Messages
300
Helped
17
Reputation
34
Reaction score
5
Trophy points
1,298
Activity points
3,028
Hi Guys,

I like to check the mismatch analysis effect on the folded cascode opamp. In the
Monte Carlo analysis, how do i run the mismatch analysis in correct way. Is that i simply put the number of runs, let say 1000 and click run, or there is option on define
correlation and select the differential input transistor and set the mismatch ratio to 0.5. Which is the correct way on running mismatch analysis. Pls explain.

Thanks,
Suria
 

you can set correlatin coefficient between dedicated mosfets by using the menu option "Simulation/Define Correlations" ...

Anyway I'm wondering how you determine the correlation coefficients ? (or how you geuss them on a first appraoch ?)
 

HI avt,

What i know, when we set the correlation coefficent to 1, meaning the pair devices is perfectly matched. If 0.5, means there is a mismatch. To set the correlation coefficient, let say in differential amplifier, i choose the two input MOS as a device parameter to be matched.

Suria
 

you need to set the coefficients as default parameters if you change anything then the simulation results and the silicon results will differ.
 
kumard35b said:
you need to set the coefficients as default parameters if you change anything then the simulation results and the silicon results will differ.
Click to expand...

Hi,

If i set the coefficient to default, what does it mean? Is that the default means it does taken into consideration of the device parameter mismatches. I'm not sure of this, but what i was told, when we personally set some value, means we are introducing the mismatch actually and check the reliability of the cirucit that we design. Please clarify.

Suria
 

U don't need to set correlation coefficient, because mismatch models provided by foundary have been measured for perfectly matched devices (see actual recomendation from foundary at the bottom). Also u need to prepare schematic to Monte Carlo Simulation. Never use m-factor and number of gates more then 1. Change such devices to multiply parallel device connection(or use notation like <0:9> in instance name).
I hear 100 runs correspond to 10% error tolerance in results.

3.1 Usage of m or ng instance parameters
----------------------------------------
It is not allowed to use multiplication factors like "m" or "ng" when simulating
matching monte carlo.
The device instances in the schematic must be placed in the same way as they
will be in the final layout.
Multiplication factor MUST be 1 for each device instance!
E.g. a device which used m=2 should be changed to two equal devices in parallel
with m=1.
It may be necessary to adjust ad, as, pd, ps for this group of devices.

Attention: If the m factor is used, matching simulation will be eroneous!

The additional effort seems tolerable because matching should be commonly
simulated for only a small amount of devices.


3.2 Be careful
--------------
All matching parameters are measured using test structures with perfect
designed layout. This means that these parameters can only be reached with a
special optimised layout.
Some effects, which are not included in the spice models, may have
a larger influence to device matching as the modeled mismatch.
Some keywords are: dummy structures, placement, length of connections,
metal coverage, temperature gradients and so on.



3.3 Running the matching simulation
-----------------------------------
Two identical designed elements are not identical during the simulation run.
The statistical mismatch of identical designed devices is modeled.
 

    S

    suria3

    Points: 2
    Helpful Answer Positive Rating
DenisMark said:
U don't need to set correlation coefficient, because mismatch models provided by foundary have been measured for perfectly matched devices (see actual recomendation from foundary at the bottom). Also u need to prepare schematic to Monte Carlo Simulation. Never use m-factor and number of gates more then 1. Change such devices to multiply parallel device connection(or use notation like <0:9> in instance name).
I hear 100 runs correspond to 10% error tolerance in results.

3.1 Usage of m or ng instance parameters
----------------------------------------
It is not allowed to use multiplication factors like "m" or "ng" when simulating
matching monte carlo.
The device instances in the schematic must be placed in the same way as they
will be in the final layout.
Multiplication factor MUST be 1 for each device instance!
E.g. a device which used m=2 should be changed to two equal devices in parallel
with m=1.
It may be necessary to adjust ad, as, pd, ps for this group of devices.

Attention: If the m factor is used, matching simulation will be eroneous!

The additional effort seems tolerable because matching should be commonly
simulated for only a small amount of devices.


3.2 Be careful
--------------
All matching parameters are measured using test structures with perfect
designed layout. This means that these parameters can only be reached with a
special optimised layout.
Some effects, which are not included in the spice models, may have
a larger influence to device matching as the modeled mismatch.
Some keywords are: dummy structures, placement, length of connections,
metal coverage, temperature gradients and so on.



3.3 Running the matching simulation
-----------------------------------
Two identical designed elements are not identical during the simulation run.
The statistical mismatch of identical designed devices is modeled.
Click to expand...


Hi Denismark,

Thanks a lot for your valuable feedback. So, according the replies, if any of my design has the number of m and gate connection more than 1, i should changed it back to 1 and that will be the final schematic for layout as well. Then, i do not need to set the correlation efficient to any value,just run the simulation by choosing the two pair input transistor without any value.

I'm not very clear on the explanation of item 3.3, please explain.

Thanks,
suria
 

I am agree, but i add some comments.
Many designers draw their schematic without using "m" or "ng" for further Monte-Carlo Simulation. In Virtuoso u can place N instances in parallel by simple changing NAME of instance to "NAME<1:N>".
U don't need to set correlation coefficients. And don't choose any pairs, it isn't requered.
3.3. - Don't mind about, it is only text from foundary, it means the same as Monte-Carlo Simulation concept.
 

thank you denis - but can I find the correlation coefficients that are "delivered" by the foundry also in plain text somehow in the simulation files ?
 

Hello Dennis,

Well if you don't define correlation how is the simulator expected to match any pair of devices for that matter. For example if device X&Y are matched in layout you need to set the correlation value, unless you do that simulator assumes all devices as mismatched (this seems reasonable) but if you don't it seems you are implying that it assumes that all the devices are correlated (this is absurd). Please clarify on this.

Thanks,
Eda
 

Hi Denismark,

Thanks a lot for your valuable feedback. So, according the replies, if any of my design has the number of m and gate connection more than 1, i should changed it back to 1 and that will be the final schematic for layout as well. Then, i do not need to set the correlation efficient to any value,just run the simulation by choosing the two pair input transistor without any value.

I'm not very clear on the explanation of item 3.3, please explain.

Thanks,
suria
Click to expand...

hi suria3
i have a little comment confusing for me,
i think the parameter ng which needs to be equal to 1 is not the number of gate contacts but the number of gates , may be it's exactly the same thing as the m-factor , but with different name according to specific DK, because i understand that m should be equal to 1 and schematic and layout match, but it doesnt make any sense for me to force ngcon (# of gate contacts ) to 1 , because it changes complettly the device especially if you are worried about gate resistance
pls comment on my post, i am running monte carlo simulation and what you said confused me
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top