Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

Importing a Supetex SPICE model - Issues

Solved!
Go to solution

Hi,

 

I have a .MOD file from Supertex for one of their MOSFETs. I've attempted to import the component in to multisum using the 'Component wizard' of multisim but i always get the error....

 

------ Checking SPICE netlist for Design1 - 04 June 2013, 15:53:44 ------ 
SPICE Netlist Error in schematic RefDes 'u2', element 'mosmod': Unsupported model type 'nmos'
SPICE Netlist Error in schematic RefDes 'u2', element 'm1': Unsupported SPICE device type 'MOS7'
======= SPICE Netlist check completed, 2 error(s), 0 warning(s) =======

 

 

Why does multisim not like this model? And how can i alter it to fix the issues?

 

 

 

 The model that was provided to is:

 

 

.SUBCKT TN6420 1 2 3 
M1 11 2 3 3 
+ MOSMOD 
+ L = 3E-06
+ W = 0.058 
+ AD = 9E-12 
+ PD = 1.2E-05 
+ AS = 9E-12 
+ PS = 1.2E-05 
JFET 1 3 11 JMOD 1
* AREA = 1 
Dbody 3 1 Diode 1
* A = 1 
Rdummy 1 11 1E+06 
.MODEL JMOD NJF
+ vto = -10 
+ beta = 0.03864
+ is = 1E-15 
+ rd = 3.281 
+ lambda = 0 
.MODEL Diode D
+ is = 1E-15 
+ n = 1 
+ rs = 1 
+ bv = 250 
+ ibv = 0.001 
+ tt = 1E-06 
+ cjo = 8E-11 
+ vj = 0.6 
+ m = 0.5 
.model MOSMOD NMOS 
+ level = 7 
+ version = 3.2 
+ paramchk = 1 
+ mobmod = 3 
+ capmod = 3 
+ noimod = 1 
+ delta = 0.01 
+ tnom = 27 
+ tox = 7.5E-08
+ toxm = 7.5E-08 
+ nch = 7.739E+16 
+ xj = 5E-06 
+ vth0 = 1.1
+ k1 = 0 
+ k2 = 0 
+ k3 = -11.69 
+ k3b = -22.99 
+ w0 = 0.0001 
+ nlx = 0 
+ dvt0 = 2.2 
+ dvt1 = 0.53 
+ dvt2 = -0.05058 
+ dvt0w = 0 
+ dvt1w = 5.3E+06 
+ dvt2w = -0.032 
+ eta0 = 0 
+ etab = 1581 
+ dsub = 0.56 
+ u0 = 261.1
+ ua = 1E-10 
+ ub = 1E-20 
+ uc = -1E-09 
+ vsat = 1.778E+04 
+ a0 = 0 
+ ags = -1 
+ b0 = 0 
+ b1 = 0 
+ keta = -0.136 
+ a1 = 0 
+ a2 = 3.414 
+ rdsw = 3.273E+04 
+ prwb = 0.3214 
+ prwg = -10 
+ wr = 1 
+ wint = 0 
+ wl = 0 
+ wln = 1 
+ ww = 0 
+ wwn = 1 
+ wwl = 0 
+ dwg = 0 
+ dwb = 0 
+ lint = 0 
+ ll = 0 
+ lln = 1 
+ lw = 0 
+ lwn = 1 
+ lwl = 0 
+ voff = -0.0157 
+ nfactor = 0.7 
+ cit = 0 
+ cdsc = 0 
+ cdscb = 0 
+ cdscd = 0 
+ pclm = 0.1 
+ pdiblc1 = 0 
+ pdiblc2 = 1E-06 
+ pdiblcb = 1 
+ drout = 0 
+ pscbe1 = 3.548E+08 
+ pscbe2 = 1E-09 
+ pvag = 1E-06 
+ alpha0 = 0 
+ alpha1 = 0.04694 
+ beta0 = 210.8 
+ js = 5E-10 
+ jsw = 0 
+ nj = 1 
+ ijth = 0.1 
+ cj = 0 
+ mj = 0.2387 
+ pb = 0.3 
+ cjsw = 0 
+ mjsw = 0.33 
+ pbsw = 0.3 
+ cjswg = 0 
+ mjswg = 0.33 
+ pbswg = 1 
+ cgbo = 0 
+ cgdo = 0 
+ cgso = 0 
+ cgsl = 4.5E-09
+ cgdl = 2.8E-09 
+ ckappa = 0.6 
+ cf = 0 
+ noff = 1 
+ voffcv = 0 
+ acde = 1 
+ moin = 15 
+ dlc = 0 
+ dwc = -3.584E-08 
+ llc = 0 
+ lwc = 0 
+ lwlc = 0 
+ wlc = 0 
+ wwc = 0 
+ wwlc = 0 
+ clc = 1E-07 
+ cle = 0.6 
+ elm = 2 
+ xpart = 0.6 
+ kt1 = -0.11 
+ kt1l = 0 
+ kt2 = 0.022 
+ ute = -1.5 
+ ua1 = 4.31E-09 
+ ub1 = -7.61E-18 
+ uc1 = -5.6E-11 
+ at = 3.3E+04 
+ prt = 0 
+ xti = 3 
+ tpb = 0 
+ tpbsw = 0 
+ tpbswg = 0 
+ tcj = 0 
+ tcjsw = 0 
+ tcjswg = 0 
+ af = 1.5 
+ ef = 1.5 
+ kf = 1E-17 
+ em = 4.1E+07 
+ noia = 2E+29 
+ noib = 5E+04 
+ noic = -1.4E-12 
.ENDS

 

 

 

Thanks for any help in advance

Rob

0 Kudos
Message 1 of 8
(4,029 Views)

I fixed this issue by changing the MOSFET model to level 8. I'm not 100% sure as to whether this is the correct thing to do, as i'm unsure on whether the MOSFET is modelled the same. Some form of confirmation for this would be good if anyone actually knows what the difference is.

0 Kudos
Message 2 of 8
(3,991 Views)

Hi,

 

Increasing the model level will mean that there is extra data involved in the model for simulation. If this extra data isn't defined, it should take some defaults, so I would think this is all ok.

Ian S
Applications Engineer CLA
National Instruments UK&Ireland
Message 3 of 8
(3,970 Views)
Solution
Accepted by topic author 08Ultrasound

It looks like this subcircuit, written for a specific simulator in mind, is attempting to use the BSIM3.2 mosfet device model. We have BSIM3.3 at level=8. Just change the value of the level parameter to 8.

 

Here's a table from our help documentation:

 

Level Value
Description
1 or MOS1
Shichman-Hodges model (DEFAULT model).
2 or MOS2
More complex model than LEVEL 1 based on actual device physics.
3 or MOS3
Semi-empirical model good for simulating short channel effects.
4 or BSIM1
BSIM1.
5 or BSIM2
BSIM2.
6 or MOS6
N-th power law MOSFET model.
8 or BSIM3
BSIM3 (version 3.3.0).
10 or B4SOI
BSIMSOI4 (version 4.0).
14 or BSIM
BSIM4 (version 4.6.3).
44 or EKV
EKV (version 2.6) 

 

Attached is a test circuit with this (modified) model wrapped into a component.

 

Hope it works out for you.

 

 

Edit - I just noticed your own reply. The level parameter selects among various device models, which do not necessarily increase in complexity with increasing level value. It is simply a coincidence that you blindly increased the level value and got a working model. 

 

 

 

Max
National Instruments
Message 4 of 8
(3,956 Views)

Thank you Ian and Max for your help.

 

Max, in your altered version of the MOSFET model, did you change anything else other than the level to 8?

0 Kudos
Message 5 of 8
(3,944 Views)

I did not. 

Max
National Instruments
0 Kudos
Message 6 of 8
(3,942 Views)

Okay thank you.

0 Kudos
Message 7 of 8
(3,940 Views)

I solved this one based on this video 

 

https://youtu.be/wtDKqJMv5v0

0 Kudos
Message 8 of 8
(96 Views)