i want to perform monte carlo simulation for finfet adders using PTM -MG file and Hspice tool.Can anyone worked / working in this field help me ?
Monte Carlo can be performed using Micro-Cap. At Emerson we paid $4,000 for every Micro-Cap program! There are no other electronic SPICE modeling programs even close to Micro-Cap capability.
Andy Thompson, owner of Spectrum Software, has retired. He is making Micro-Cap free => http://www.spectrum-soft.com/index.shtm => Download.
Micro-Cap does worst case analysis, changing the tolerances of components, changing the temperature, Monte Carlo, etc. (Analysis > DC > Run > Monte Carlo ). And it is easy to use.
I have used Micro-Cap for all of my electronic designs since 2001. When I tested prototypes, the prototypes worked exactly as the model predicted.
The website https://NDAcademy.FoxPing.com/ => 2.8 Electronic Cascade RC Filters --- and --- 7.2 Electronic SPICE Models --- provide some examples.
If you add the Monte Carlo command in the *.sp file, it won't work.
You need to add this command to the library and run your *.sp file.
use sweep monte command with ac analysis,
decide which parameters you want to test and use gauss command,
you can find these things in Allen and Holberg and Jacob Baker book.
You have to go to its library and change the parameters on which you intend to simulate Monte Carlo and put a variable in its place, then use them in your netlist with Monte Carlo commands and do the simulation.
In your library file, put variable instead of value for each parameter that you need to check its effect on your circuit performance. for example;
Vth0=0.49 =>>>>>>>> Vth0='Vth0n_MC' *** for NMOS
Vth0=-0.49 =>>>>>>>> Vth0='Vth0p_MC' *** for PMOS
Now, include the following commands in your netlist:
.OPTION MEASFORM=3
*** .PARAM xx=GAUSS(nominal_val, rel_variation, sigma)
.PARAM Vth0n_MC=gauss(0.49,0.1,3)
.PARAM Vth0p_MC=gauss(-0.49,0.1,3)
.TRAN 10p 100n SWEEP MONTE=10000
However, this way generates randomly one Vth for all NMOS transistors and one Vth for all PMOS transistors in every single iteration. So, after making the required changes in your library, write a subcircuit and then use it for the definition of your main circuit. In this modified way, each transistor gets a unique Vth.
.SUBCKT NMOS D G S B Width=16n Length=16n
.include ...... **library
.PARAM Vth0n_MC=gauss(0.49,0.1,3)
M1 D G S B NMOS (W='Width' L='Length')
.ends NMOS
.SUBCKT PMOS D G S B Width=16n Length=16n
.include ...... **library
.PARAM Vth0p_MC=gauss(-0.49,0.1,3)
M1 D G S B PMOS (W='Width' L='Length')
.ends PMOS
Now start your main circuit.
- Badges
- Science topic
- Similar topics
- Correction