06-05-2013 10:30 AM - edited 06-05-2013 10:30 AM
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
Solved! Go to Solution.
06-10-2013 06:29 AM
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.
06-11-2013 08:18 AM
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.
06-12-2013 09:12 AM - edited 06-12-2013 09:20 AM
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:
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.
06-12-2013 09:45 AM
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?
06-12-2013 09:47 AM
I did not.
06-12-2013 09:48 AM
Okay thank you.
02-07-2021 06:10 PM