If you have Cadence' analogLib, use its nmos & pmos models - and copy & modify them, if necessary.macg84 said:... how can find this model in cadence and how can i change this model??? ... Thanh you for your attention
Yes, they use the mos2 spectre model.macg84 said: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?
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).macg84 said:How can i change the model of this mosfet??
You cannot get rid of the gm 2nd derivative's discontinuity at Vds=0, because it's physically inherentmacg84 said:I want to do an ideal switch, to skip the problem of the model bsim3 and 4 in Vds=0.
Thank you
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).macg84 said: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
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 5.1.41macg84 said: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.
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!macg84 said: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?
I guess: yes. AFAIK they rely on the mos2 model.macg84 said: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 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.macg84 said:... 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??
Your new circuit has been removed, so I can't see your voltage sources V6 and V7.macg84 said: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?
I don't think so, because you don't seem to be content with your result ;-)macg84 said: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?
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.macg84 said: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?? ...
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?