SemiSouth Spice models?

[buzzforb]

Just wandering if anyone has SPice models for any of the Semisouth fets. I would like to try using them in Pass SOX and BOSOZ. Evrything I have read about them (by Pass) says they are superior. So while i wait on parts for my first amp build(Aleph J), I would like to play with these gold plated JFets with no money down.

 

[Melon Head]

They are still being developed by semisouth.

 

[EUVL]

Have you asked ?

Patrick


PS See Table 1 of :
http://www.semisouth.com/applicatio...ratures_Greater_than_300C_HiTEC04_Merrett.pdf

.

 

[knutn]

PSpice Model

I have made my own, using curve fitting:

.MODEL SJEP120 NMOS
+ LEVEL=3
+ L=2.0000E-6
+ W=150
+ KP=1.0014E-6
+ RS=10.000E-3
+ RD=27.968E-3
+ VTO=.94454
+ RDS=6.0000E6
+ TOX=2.0000E-6
+ CGSO=66.667E-18
+ CGDO=544.10E-15
+ CBD=1.1197E-9
+ MJ=.68177
+ RG=10.000E-3
+ IS=1.0000E-18
+ N=5
+ RB=1.0000E-9
+ GAMMA=0
+ KAPPA=0
*$

 

[EUVL]

Thanks a lot.

Patrick

 

[Melon Head]

Have you asked ?

Patrick


PS See Table 1 of :
http://www.semisouth.com/applicatio...ratures_Greater_than_300C_HiTEC04_Merrett.pdf

.

Yes. They told me they are still working on the spice models. They will be getting back to me when they are finished.
I have seen that pdf, but I am waiting on them to send me their official spice model.

Great work knutn. I will have a look at it.

 

[buzzforb]

Have you asked ?

Patrick


PS See Table 1 of :
http://www.semisouth.com/applicatio...ratures_Greater_than_300C_HiTEC04_Merrett.pdf

.

I had also seen the table in the Semisouth datasheet, but it was incomplete in comparison to other models i had used and i am not informed enough to proceed otherwise. Thanks knutn for the model. Now i can just simulate destroying it. Interesting that the dollar sign came up in your measurements.

 

[buzzforb]

I have made my own, using curve fitting:

.MODEL SJEP120 NMOS
+ LEVEL=3
+ L=2.0000E-6
+ W=150
+ KP=1.0014E-6
+ RS=10.000E-3
+ RD=27.968E-3
+ VTO=.94454
+ RDS=6.0000E6
+ TOX=2.0000E-6
+ CGSO=66.667E-18
+ CGDO=544.10E-15
+ CBD=1.1197E-9
+ MJ=.68177
+ RG=10.000E-3
+ IS=1.0000E-18
+ N=5
+ RB=1.0000E-9
+ GAMMA=0
+ KAPPA=0
*$

This modeled just as I expected. Thanks for knutn! I mean thanks Knutn!

 

[lhquam]

I have made my own, using curve fitting:

.MODEL SJEP120 NMOS
+ LEVEL=3
+ L=2.0000E-6
+ W=150
+ KP=1.0014E-6
+ RS=10.000E-3
+ RD=27.968E-3
+ VTO=.94454
+ RDS=6.0000E6
+ TOX=2.0000E-6
+ CGSO=66.667E-18
+ CGDO=544.10E-15
+ CBD=1.1197E-9
+ MJ=.68177
+ RG=10.000E-3
+ IS=1.0000E-18
+ N=5
+ RB=1.0000E-9
+ GAMMA=0
+ KAPPA=0
*$

Those values for CGSO and CGDO are not believable. Does anyone have better values for these parameters? They are essential for predicting AC behavior and harmonic distortion components.

 

[knutn]

Those values for CGSO and CGDO are not believable. Does anyone have better values for these parameters? They are essential for predicting AC behavior and harmonic distortion components.

No, you are right; I did not model these capacitances. If you take a look at the data sheet, you will see that Semisouth is specifying Ciss=670 pF, Coss=103 pF and Crss=97 pF at VDD=100V. My first try for the Spice model would be to set CGSO=Ciss=700E-12 and CGDO=Crss=100E-12 (Keep the bulk-drain capacitance CBD=1.1197E-9). Please, be aware that especially CGD increases when the drain-gate voltage decreases. I am afraid you will have to try to run Spice and change the values to comply with the data sheet values. Anyone who has any values from Semisouth?

 

[davygrvy]

Over on the LTspice yahoo group, analogspiceman just made a very accurate model of the SJEP120R100 for us to enjoy.

 

[davygrvy]

The negative thermal (-1.5mV/C) Vto is killing me.

I'm thinking a PTC set at 120C or 130C in the current source of my bootstrap bias feed might do it.

 

[Bademeischda]

hey guys!

I made a model of the depletion SiC-JFET (SJDP120R085)...or at least I tried to. I took the model and the LTspice files of analogspiceman and changed them. The only thing that doesn't want to work properly is the Gate Current (Fig.6) [and I cheated a bit in Fig.10 Typical Capacitance: I think the "0.01uA" from "im(I(Vg))/(2*Pi*0.01uA)" should be "10uA" if I interpret the .plt file of analogspiceman correctly].
Do you have any idea what I'm doing wrong?

 

[kees52]

Can I use this also for multisim tryout so I can test it.

thanks.