How to change mosfet model in cadence

[macg84]

gummel symmetry

Hello,
I use for my RF simulation the BSIM3 model, i guess that in dadence there are other ideal model olso. My question is this: how can find this model in cadence and how can i change this model??? Is there in PRIMLIB the ideal mosfet???

Thanh you for your attention

 

[erikl]

cadence change parameters

... how can find this model in cadence and how can i change this model??? ... Thanh you for your attention

If you have Cadence' analogLib, use its nmos & pmos models - and copy & modify them, if necessary.

 

[macg84]

cadence nmos model

Thank you erikl, so if I well understand the nmos and pmos are ideal mosfet and they don't follow the model bisim 3, is it true? How can i change the model of this mosfet?? I want to do an ideal switch, to skip the problem of the model bsim3 and 4 in Vds=0.

Thank you

 

[Mr.Cool]

cadence change model name

macg84, how to change the NMOS/PMOS model is described in the documentation for PSpice. it tells you which parameter can be accommodated and what each one means.

HOW to modify it? you add the parameters that you want simulated. that's how.

 

[erikl]

cadence mos idea model

Thank you erikl, so if I well understand the nmos and pmos are ideal mosfet and they don't follow the model bisim 3, is it true?

Yes, they use the mos2 spectre model.

How can i change the model of this mosfet??

You can't change the model, just its parameters. To do this, copy the Cadence model (just the views you need, e.g. spectre & symbol) to a new model name and save them where you have rw access - (if necessary, extend your Library path to make sure the model can be found). Then edit its CDF to change the parameters. You can find more info in $CDS_INST_DIR/doc/anasimhelp/chap3.html (search for nmos).

I want to do an ideal switch, to skip the problem of the model bsim3 and 4 in Vds=0.
Thank you

You cannot get rid of the gm 2nd derivative's discontinuity at Vds=0, because it's physically inherent Berkeley's SP model achieves this by a mathematical tric.

 

[macg84]

ads sp pb model fet

So i will find this problem in nmos and pmos too. So to realize an ideal mosfet i can describe it with verilog-A. According to you can be it a good idea?

Thank you erikl

 

[erikl]

case insensitive cadence

So i will find this problem in nmos and pmos too. So to realize an ideal mosfet i can describe it with verilog-A. According to you can be it a good idea?
Thank you erikl

Sorry, no, this is a misunderstanding. You won't be able to describe an ideal mosfet which comes any close to that what a real transistor does. Of course you can describe a simple switch (the simplest is already in the ahdlLib: sw), but by no way this will give you realistic simulation results (and that's what you probably want).

The only way to avoid the gm derivative's discontinuity @ Vds=0 is to throw away the velocity saturation mechanism description, which is quite important for the strong inversion region, or to use the true surface potential method (the SP model).

Write your own model? Forget about it! Don't forget that models like mos2, mos3, BSIM3v2, BSIM4 (and SP) need quite a lot of pages for their MOSFET description. And in the Cadence environment, you cannot change the original models. Why? Because all foundry PDKs rely on their originality. Of course it is possible to add another model (SP e.g.), but then the foundry MOSFET models (i.e their parameters) in the PDK would have to be updated to it.

I don't know, if the next Cadence release will include the SP model - and which foundries will support it.

My suggestion: try to (somehow, I don't know your application) avoid the Vds=0 situation, perhaps limit it by a conditional (behavorial) clamp to > |±1..2*Vt| .
Good luck! erikl

 

[macg84]

cadence tools for mosfet

Hello erikl, thank you for your valuable advice.
I have to design a transferred impedance filter, in other words a passive mixer(you can see the attached file) and so i have some problem for Vds=0. If i want to change the paramter of the mosfet, where can i go in cadence? I don't find the section with the differnt paramenter. How reported in the paper of Peter Bendix i could change the value of n from 1 to 2 in nmos in the velocity saturation to skip this problem. According to you is it right and can i do this?
Now i'm using the nmos4 and pmos4 model, but if i right understand all this model have the same problem in Vds=0.

Thank you

 

[erikl]

modify analoglib cdf cadence

Hello erikl, ... i have some problem for Vds=0. If i want to change the paramter of the mosfet, where can i go in cadence? I don't find the section with the differnt paramenter.

Oh dear, I already told you in my answer from Sun, 22 Mar 2009 18:23 : It's in the Virtuoso Analog Design Environment User Guide, Product Version 5.1.41
$CDS_INST_DIR/doc/anasimhelp/chap3.html
Chapter: Model Files in the Virtuoso Analog Design Environment

Also, the Virtuoso Advanced Analysis Tools User Guide.pdf may be helpful, even if it describes corner, statistical & Monte Carlo simulations.

$CDS_INST_DIR/doc/dirsimmodel/chap1.html, Chapter: External Models
is also a good info source for how to change external parameters of model files.

How reported in the paper of Peter Bendix i could change the value of n from 1 to 2 in nmos in the velocity saturation to skip this problem. According to you is it right and can i do this?

Yes & No. Yes it is right, and no, you can't do this: This n value (the exponent in the velocity saturation equation) is an internal parameter of the original MOSFET model(s), and you have no access to those - as I already told you before. If you'd change the external n=N parameter (SPICE is case-insensitive), you'd change the emission coefficient of Is (the saturation current) - which would create quite a different effect. BTW: BSIM3v3 now uses 206 (!) parameters!

Now i'm using the nmos4 and pmos4 model, but if i right understand all this model have the same problem in Vds=0.

I guess: yes. AFAIK they rely on the mos2 model.
In the $CDS_INST_DIR/tools/dfII/samples/artist/models/spectre/ directory there is an rfModels.scs file which contains special RF MOSFET models based on the mos3 model. I don't know it, but you might give it a try.

 

[macg84]

cadence nmos model include

I have another question (sorry sorry), i would make the gummel symmetry test to nmos4, so i make the test bantch in the figure (gummeltest) and by dc analysis i sweep V5 between -0.3 to 0.3. My current result is attached in the figure caratteristiccurrent. To get (d^2I/dv^2) I have to use in calculator the special function deriv in other words: derive(deriv(IS("/MN0/D"))) but in this way i not get a correct results.

What's the error??

Thank you Thank you

 

[erikl]

cadence cdf mos ad

... i would make the gummel symmetry test to nmos4, so i make the test bantch in the figure (gummeltest) and by dc analysis i sweep V5 between -0.3 to 0.3. My current result is attached in the figure caratteristiccurrent. To get (d^2I/dv^2) I have to use in calculator the special function deriv in other words: derive(deriv(IS("/MN0/D"))) but in this way i not get a correct results.

What's the error??

I think your schematic - its power suppy - is not correct: The drain voltage is 500mV below vdd, and your source voltage is 500mV above vdd. And I don't see V5, so I don't know which node you are sweeping. You would want to sweep the gate voltage, but there you have a vdc with a fixed voltage.
Moreover I think IS is not the current you want, it looks like the saturation current of the nmos (1.7fA).

Now my question: Did you ever run a successful simulation before? It looks to me you're quite new to this procedure. I'd suggest to attend a simulation course; there's a lot of examples in the Cadence docs (and samples) and on Internet.

 

[macg84]

changing model file in cadence

Hello erikl,
your words are right I have to study more. I wrong the circuit and i attached the new circuit to do gummel symmetry test. I sweep v11 e v9 between -1 an 1 by dc sweep, is it right?
To verify the simmetry i have to compute the second order derivative. So i 'm using calculator with this expession: deriv(deriv(IS("/V8/MINUS"))) is equal to do (d^2Ids/dVx^2) (X= sweepVx and y=Ids in dc sweep)...but i don't get the correct shape, i don't understand why??
can you hel me?
Excise me for trivial question

 

[erikl]

spectre change mos model

Yes I mistoke the circuit to do the gummel test. I attached the new circuit, but my the problem to make the gummel test is maybe simple but not for me . I want to sweep simultaneousuly voltage source V6 and V7, but if I use DC sweep i can choos only one between this two sorce, and also I can\'t give them the same istanze name.
How can i do to skip this problem?

Your new circuit has been removed, so I can't see your voltage sources V6 and V7.
You can only sweep 1 variable at the time, so you must run the other sweeps serially. In the Parametric Analysis tool, however, you can group variable value pairs (triples ...) into common simulation runs.

 

[macg84]

how to change mosfet

Hello erikl,
your words are right I have to study more. I wrong the circuit and i attached the new circuit to do gummel symmetry test. I sweep v11 e v9 between -1 an 1 by dc sweep, is it right?
To verify the simmetry i have to compute the second order derivative. So i 'm using calculator with this expession: deriv(deriv(IS("/V8/MINUS"))) is equal to do (d^2Ids/dVx^2) (X= sweepVx and y=Ids in dc sweep)...but i don't get the correct shape, i don't understand why??
can you hel me?
Excise me for trivial question

 

[erikl]

spectre model mosfet example

Hello erikl, ...
i attached the new circuit to do gummel symmetry test. I sweep v11 e v9 between -1 an 1 by dc sweep, is it right?

I don't think so, because you don't seem to be content with your result ;-)
Meanwhile I've simulated the Gummel symmetry test, and I got a rather satisfying result, s. the schematic and the sim. screenShot below.

To verify the simmetry i have to compute the second order derivative. So i 'm using calculator with this expession: deriv(deriv(IS("/V8/MINUS"))) is equal to do (d^2Ids/dVx^2) (X= sweepVx and y=Ids in dc sweep)...but i don't get the correct shape, i don't understand why?? ...

Try to imitate my simulation setUp (s. below). I put the vx sweep variable into both the source and drain power supplies (V0+vx) and (V0-vx), so both will be swept at the same time. The instanciated nmos4 needs a model, which in this case is a model of our foundry, which, on its part, is based on the BSIM3v2 model. The Id current is contiguous through Vds=0, and its 2nd derivative is defined and (practically) zero, s. the curves below. The steep in-/decline of Id at voltages < ~ -1V will be due to the parasitic anti-parallel diode, I guess.
If you meet difficulties to reproduce my simulation, ask specific questions!
Good luck! erikl

 

[macg84]

mosfet calculator

I do not know how to thank you, tomorrow i try ... THANK youuuuuuuuuu

 

[macg84]

spectre ideal mosfet model

Hello erik,
I obtained your same results for current and voltage, but i don't understand how you compute the second order derivative...i derived the current M0/D but i got bad results How can i do??

 

[erikl]

simple ideal mosfet

Practically I did the same as you suggested in your posting from Tue, 24 Mar 2009 13:52 : "deriv(deriv(IS("/V8/MINUS")))".

In my representation it was "deriv(deriv(clip(i("M0:d"?result"dc-dc") -1.1 2.5)))" - you could see this at my Gummel_symmetry_simulation.png. Within the calculator, I just selected the upper curve /M0/D and hit the "deriv" twice (+ Evaluation). In order not to create a pb. for the derivation of the steep decline @ voltages < -1.1V, I used the clip function.

Good luck! erikl.

 

[macg84]

parasitic diode mosfet cadence

Yes, i understand... thank you very much erikl great...