What is "Corners simulation" ?

Hi..everybody

Can someone tell me what is corners simulation and how it works？

Thanks for your help！

^.^

Corners simulation takes into account the loading in the Power Supplies, Temp changes and changes in the process. You design a circuit in the typical case (VDD=typ, T=27 and typical process parameters) and then you check by changing the supply voltage, temperature and the process parameters to see how your circuit performance is affected.

In the SS Case (SS = Slow Slow) Temp = 125 and VDD = 90% of supply along with process files

FF --> Temp = 0, VDD = 110% and process changes

NSPF--> N Slow and P Fast

NFPS --> N transistors Fast and P slow

There is also Monte Carlo mismatch analysis to check the circuit operation when you deliberately introduce mismatch in Vth, W, L of all transistors and check for the results.

Hope this helps!

Good answer!

The temp should be low -50

For DIGITAL circuits, you usually use three corners, FAST, SLOW & NOMINAL (or typical) and that is considered good enough.


For ANALOG design, using a Monte-Carlo analysis is a better idea. If you are trying to be rigorous, there will be a lot of simulation going on. Sweeping every parameter with every combination of other parameters till the cows come home. But some work can be reduced with good design practices listed below. Experience cannot be replaced here.


Usually for analog design, the circuits are designed so that

1) there is a bandgap referenced biasing scheme that takes care of temperature

2) there is a DLL-type or PLL-type interface that relies on a crystal to setup a frequency that is close to the desired frequency and then using a frequency to voltage converter to set up a voltage, if necessary. This takes care of the process variations to some extent. This is also being used to test the analog chips increasingly. Check out Self-Biasing techniques by Prof. Maneatis on the Xplore.

3) Using a power supply circuit that is referenced to a bandgap as well. In general, if it is not possible, one can use inductors (or LC filters) (right value!) to make sure that interference from the supply is rejected especially for ring VCOs.
AND/OR
use differential design to ensure a high CMRR.
AND
using heavy decoupling on the supply, (internal and external).

Another technique is to use double split guard rings to make sure that interference from other parts of the circuit is not transferred to analog or critical circuits.


e.g.
An opamp that is fully differential, using a temperature stabilized biasing scheme driven by a bandgap reference, enclosed in a double-split guard ring and using a secondary feedback from a crystal oscillator controlled PLL to reduce variations on its own supply and using a common-centroid layout stands to succeed!

Hope it helps.

for TSMC process
there are 5 corners: tt,ss,ff,sf,fs.

hello, im trying to do a corner simulation, currently i set the ff,ss, fs, sf, temperature and power supply variation manually. it is very tedious and time consuming.
how can i use the corner simulation i cadenece tools. how do i set the models, parameters?

thanks

surreyian said:

hello, im trying to do a corner simulation, currently i set the ff,ss, fs, sf, temperature and power supply variation manually. it is very tedious and time consuming.
how can i use the corner simulation i cadenece tools. how do i set the models, parameters?

thanks

Click to expand...

U need a license to run the corner analysis, in case u want to automate it !!

The cheaper way is to write an ocean script which loops on the corners