LTSpice simulation error using downloaded BF998 model from NXP

[silverba...@gmail.com]

Hi, if anyone can help me solve this really annoying problem I'd be grateful. I have a downloaded BF998 model from NXP, I then got LTSpice to autogenerate a symbol and added it to my circuit, but when I try to simulate a really simple dc sweep I get "Can't find definition of model 'C'" errors.

This is the model from NXP

* BF998 SPICE MODEL OCTOBER 1993 PHILIPS SEMICONDUCTORS
* ENVELOPE SOT143 (R)
* 1.: SOURCE; 2.: DRAIN; 3.: GATE 2; 4.: GATE 1;
.SUBCKT BF998 1 2 3 4
L10 1 10 L=0.12N
L20 2 20 L=0.12N
L30 3 30 L=0.12N
L40 4 40 L=0.12N
L11 10 11 L=1.20N
L21 20 21 L=1.20N
L31 30 31 L=1.20N
L41 40 41 L=1.20N
C13 10 30 C=0.085P
C14 10 40 C=0.085P
C23 20 30 C=0.085P
C24 20 40 C=0.005P
D11 42 11 ZENER
D12 42 41 ZENER
D21 32 11 ZENER
D22 32 31 ZENER
RS 10 12 R=100
MOS1 61 41 11 12 GATE1 L=1.1E-6 W=1150E-6
MOS2 21 31 61 12 GATE2 L=2.0E-6 W=1150E-6
.MODEL ZENER D BV=10 CJO=1.2E-12 RS=10
.MODEL GATE1
+ NMOS LEVEL=3 UO=600 VTO=-0.250 NFS=300E9 TOX=42E-9
+ NSUB=3E15 VMAX=140E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+ ETA=0.06 KAPPA=2 LD=0.1E-6
+ CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12
.MODEL GATE2
+ NMOS LEVEL=3 UO=600 VTO=-0.250 NFS=300E9 TOX=42E-9
+ NSUB=3E15 VMAX=100E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+ ETA=0.06 KAPPA=2 LD=0.1E-6
+ CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12
.ENDS BF998

and this is my symbol that LTSpice made

Version 4
SymbolType BLOCK
RECTANGLE Normal -32 -40 32 40
WINDOW 0 0 -40 Bottom 2
WINDOW 3 0 40 Top 2
SYMATTR Prefix X
SYMATTR Value BF998
SYMATTR ModelFile C:\Users\Rob\Documents\LTSpice\LNA\spice_BF998.prm
PIN 32 -16 LEFT 8
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN 32 16 LEFT 8
PINATTR PinName 2
PINATTR SpiceOrder 2
PIN -32 -16 RIGHT 8
PINATTR PinName 3
PINATTR SpiceOrder 3
PIN -32 16 RIGHT 8
PINATTR PinName 4
PINATTR SpiceOrder 4

and finally my simple little circuit

Version 4
SHEET 1 880 680
WIRE 224 -64 -80 -64
WIRE -80 -32 -80 -64
WIRE -80 96 -80 48
WIRE 112 144 -208 144
WIRE 224 144 224 -64
WIRE 224 144 176 144
WIRE -208 176 -208 144
WIRE 112 176 -32 176
WIRE 224 176 176 176
WIRE -208 304 -208 256
WIRE -32 304 -32 176
WIRE -32 432 -32 384
WIRE 224 464 224 176
FLAG -208 304 0
FLAG -32 432 0
FLAG 224 464 0
FLAG -80 96 0
SYMBOL voltage -208 160 R0
WINDOW 39 24 124 Left 2
SYMATTR SpiceLine Rser=0
SYMATTR InstName VG2
SYMATTR Value 4
SYMBOL voltage -32 288 R0
SYMATTR InstName VG1
SYMBOL voltage -80 -48 R0
WINDOW 39 24 124 Left 2
SYMATTR SpiceLine Rser=0
SYMATTR InstName VDS
SYMATTR Value 5
SYMBOL AutoGenerated\\BF998 144 160 R0
SYMATTR InstName U1
TEXT 8 344 Left 2 !.dc VG1 -1 1 0.1

[m...@iae.nl]

L=0.12n should simply be "0.12n".
Vg1 is missing a dc value.
What's that .prm file?
The .asy file should link to the bf998.sub.

Works for me.

-marcel

-- bf998.sub ---------------------------------------------------

* BF998 SPICE MODEL OCTOBER 1993 PHILIPS SEMICONDUCTORS
* ENVELOPE SOT143 (R)
* 1.: SOURCE; 2.: DRAIN; 3.: GATE 2; 4.: GATE 1;
.SUBCKT BF998 1 2 3 4

L10 1 10 0.12N
L20 2 20 0.12N
L30 3 30 0.12N
L40 4 40 0.12N
L11 10 11 1.20N
L21 20 21 1.20N
L31 30 31 1.20N
L41 40 41 1.20N
C13 10 30 0.085P
C14 10 40 0.085P
C23 20 30 0.085P
C24 20 40 0.005P

D11 42 11 ZENER
D12 42 41 ZENER
D21 32 11 ZENER
D22 32 31 ZENER

RS 10 12 100

MOS1 61 41 11 12 GATE1 L=1.1E-6 W=1150E-6
MOS2 21 31 61 12 GATE2 L=2.0E-6 W=1150E-6
.MODEL ZENER D BV=10 CJO=1.2E-12 RS=10
.MODEL GATE1
+ NMOS LEVEL=3 UO=600 VTO=-0.250 NFS=300E9 TOX=42E-9
+ NSUB=3E15 VMAX=140E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+ ETA=0.06 KAPPA=2 LD=0.1E-6
+ CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12
.MODEL GATE2
+ NMOS LEVEL=3 UO=600 VTO=-0.250 NFS=300E9 TOX=42E-9
+ NSUB=3E15 VMAX=100E3 RS=2.0 RD=2.0 XJ=200E-9 THETA=0.11
+ ETA=0.06 KAPPA=2 LD=0.1E-6
+ CGSO=0.3E-9 CGDO=0.3E-9 CBD=0.5E-12 CBS=0.5E-12
.ENDS BF998

-- test.net --------------
* C:\spice\mhx\bf998\test.asc
VG2 N002 0 4 Rser=0
VG1 N003 0 0.1
VDS N001 0 5 Rser=0
XU1 N001 0 N002 N003 BF998
.dc VG1 -1 1 0.1
.lib BF998.sub
.backanno
.end

[Jones Joy Panicker]

Found this useful after six years. Thanks!