Errors with NxP's BJT Models

H

Hammy

Guest
I keep getting these errors for NXP's dual BJT's. I'm using Capture
10.5, with PSPICE 10.5. I get similar errors with their PMD3001D
model.

This is the error I get with their PBSS4160DPN spice model

*Analysis directives:
..TRAN 0 100us 0 1u
..PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
..INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source PUSHPULL
R_R6 N09277 N00165 1k
R_R3 0 N09870 50
V_V2 N00833 0
+SIN 0 5 1000k 0 0 0
D_D1 N07581 N09467 D1N4148
V_V1 N00165 0 6
D_D2 N09277 N07581 D1N4148
R_R4 N07581 N00833 50
R_R5 N00229 N09467 1k
X_U2 N09870 N09277 N00229 N09870 N09467 N00165 PBSS4160DPN
V_V3 0 N00229 6

**** RESUMING ttutu.cir ****
..END


**** EXPANSION OF SUBCIRCUIT X_U2 ****
X_U2.Q1 N00165 N09277 N09870 X_U2.PBSS4160DS
X_U2.D1 N09277 N00165 X_U2.DIODE1
X_U2.Q2 N00229 N09467 N09870 X_U2.PBSS5160DS
X_U2.D2 N00229 N09467 X_U2.DIODE2
..MODEL X_U2.PBSS4160DS NPN IS 1.831E-013 NF 0.9823 ISE 3.486E-015 NE
+ 1.336 BF 490 IKF 0.15 VAF 10 NR 0.9825 ISC 1E-018 NC 1.821 BR 50
+ IKR 1.5 VAR 18 RB 19 IRB 0.00043 RBM 1.7 RE 0.025 RC 0.125 XTB 0 EG
+ 1.11 XTI 3 CJE 1.115E-010 VJE 0.57 MJE 0.308 TF 4.8E-010 XTF 8 VTF
+ 1.5 ITF 1.3 PTF 0 CJC 1.893E-011 VJC 0.6185 MJC 0.4452 XCJC 1 TR
+ 4.3E-008 CJS 0 VJS 0.75 MJS 0.333 FC 0.9
..MODEL X_U2.DIODE1 D IS 8E-015 N 0.98 BV 1000 IBV 0.001 RS 850 CJO 0
+ VJ 1 M 0.7 FC 0 TT 0 EG 1.11 XTI 3 IS 1.695E-013 NF
---------------------------------------------------$
ERROR -- 'NF' is not a model parameter name
??????


I get similar errors when using their PMD3001D model. Is this not a
Psice model or is it for another simulator?

The PMD3001D model is here ;
http://www.nxp.com/models/spicespar/PMD3001D.html

A C/P of the PBSS4160DPN spice model is below.

*
..SUBCKT PBSS4160DPN 1 2 3 4 5 6
*
Q1 6 2 1 PBSS4160DS
D1 2 6 DIODE1
Q2 3 5 4 PBSS5160DS
D2 3 5 DIODE2
*
* The diode does not reflect a
* physical device but improves
* only modeling in the reverse
* mode of operation.
*
..MODEL PBSS4160DS NPN
+ IS = 1.831E-013
+ NF = 0.9823
+ ISE = 3.486E-015
+ NE = 1.336
+ BF = 490
+ IKF = 0.15
+ VAF = 10
+ NR = 0.9825
+ ISC = 1E-018
+ NC = 1.821
+ BR = 50
+ IKR = 1.5
+ VAR = 18
+ RB = 19
+ IRB = 0.00043
+ RBM = 1.7
+ RE = 0.025
+ RC = 0.125
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 1.115E-010
+ VJE = 0.57
+ MJE = 0.308
+ TF = 4.8E-010
+ XTF = 8
+ VTF = 1.5
+ ITF = 1.3
+ PTF = 0
+ CJC = 1.893E-011
+ VJC = 0.6185
+ MJC = 0.4452
+ XCJC = 1
+ TR = 4.3E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.9
*
..MODEL DIODE1 D
+ IS = 8E-015
+ N = 0.98
+ BV = 1000
+ IBV = 0.001
+ RS = 850
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
*
*.MODEL PBSS5160DS PNP
+ IS = 1.695E-013
+ NF = 0.9919
+ ISE = 1.5E-014
+ NE = 1.348
+ BF = 370
+ IKF = 0.4
+ VAF = 40
+ NR = 0.9912
+ ISC = 1.541E-013
+ NC = 1.821
+ BR = 30
+ IKR = 0.4
+ VAR = 18
+ RB = 12
+ IRB = 0.001
+ RBM = 1.12
+ RE = 0.06
+ RC = 0.105
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 9.466E-011
+ VJE = 0.8044
+ MJE = 0.3919
+ TF = 9E-010
+ XTF = 20
+ VTF = 1.1
+ ITF = 1.35
+ PTF = 0
+ CJC = 3.162E-011
+ VJC = 0.7543
+ MJC = 0.4479
+ XCJC = 1
+ TR = 3.2E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.8
*
..MODEL DIODE2 D
+ IS = 1.651E-014
+ N = 1.079
+ BV = 1000
+ IBV = 0.001
+ RS = 1000
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
..ENDS
 
"Hammy" <spam@spam.com> schrieb im Newsbeitrag
news:lnvbs5d280j5k6e3nqskaf3jo7j11346ph@4ax.com...
I keep getting these errors for NXP's dual BJT's. I'm using Capture
10.5, with PSPICE 10.5. I get similar errors with their PMD3001D
model.

This is the error I get with their PBSS4160DPN spice model

*Analysis directives:
.TRAN 0 100us 0 1u
.PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source PUSHPULL
R_R6 N09277 N00165 1k
R_R3 0 N09870 50
V_V2 N00833 0
+SIN 0 5 1000k 0 0 0
D_D1 N07581 N09467 D1N4148
V_V1 N00165 0 6
D_D2 N09277 N07581 D1N4148
R_R4 N07581 N00833 50
R_R5 N00229 N09467 1k
X_U2 N09870 N09277 N00229 N09870 N09467 N00165 PBSS4160DPN
V_V3 0 N00229 6

**** RESUMING ttutu.cir ****
.END


**** EXPANSION OF SUBCIRCUIT X_U2 ****
X_U2.Q1 N00165 N09277 N09870 X_U2.PBSS4160DS
X_U2.D1 N09277 N00165 X_U2.DIODE1
X_U2.Q2 N00229 N09467 N09870 X_U2.PBSS5160DS
X_U2.D2 N00229 N09467 X_U2.DIODE2
.MODEL X_U2.PBSS4160DS NPN IS 1.831E-013 NF 0.9823 ISE 3.486E-015 NE
+ 1.336 BF 490 IKF 0.15 VAF 10 NR 0.9825 ISC 1E-018 NC 1.821 BR 50
+ IKR 1.5 VAR 18 RB 19 IRB 0.00043 RBM 1.7 RE 0.025 RC 0.125 XTB 0 EG
+ 1.11 XTI 3 CJE 1.115E-010 VJE 0.57 MJE 0.308 TF 4.8E-010 XTF 8 VTF
+ 1.5 ITF 1.3 PTF 0 CJC 1.893E-011 VJC 0.6185 MJC 0.4452 XCJC 1 TR
+ 4.3E-008 CJS 0 VJS 0.75 MJS 0.333 FC 0.9
.MODEL X_U2.DIODE1 D IS 8E-015 N 0.98 BV 1000 IBV 0.001 RS 850 CJO 0
+ VJ 1 M 0.7 FC 0 TT 0 EG 1.11 XTI 3 IS 1.695E-013 NF
---------------------------------------------------$
ERROR -- 'NF' is not a model parameter name
??????
Click to expand...


I get similar errors when using their PMD3001D model. Is this not a
Psice model or is it for another simulator?

The PMD3001D model is here ;
http://www.nxp.com/models/spicespar/PMD3001D.html

A C/P of the PBSS4160DPN spice model is below.

*
.SUBCKT PBSS4160DPN 1 2 3 4 5 6
*
Q1 6 2 1 PBSS4160DS
D1 2 6 DIODE1
Q2 3 5 4 PBSS5160DS
D2 3 5 DIODE2
*
* The diode does not reflect a
* physical device but improves
* only modeling in the reverse
* mode of operation.
*
.MODEL PBSS4160DS NPN
+ IS = 1.831E-013
+ NF = 0.9823
+ ISE = 3.486E-015
+ NE = 1.336
+ BF = 490
+ IKF = 0.15
+ VAF = 10
+ NR = 0.9825
+ ISC = 1E-018
+ NC = 1.821
+ BR = 50
+ IKR = 1.5
+ VAR = 18
+ RB = 19
+ IRB = 0.00043
+ RBM = 1.7
+ RE = 0.025
+ RC = 0.125
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 1.115E-010
+ VJE = 0.57
+ MJE = 0.308
+ TF = 4.8E-010
+ XTF = 8
+ VTF = 1.5
+ ITF = 1.3
+ PTF = 0
+ CJC = 1.893E-011
+ VJC = 0.6185
+ MJC = 0.4452
+ XCJC = 1
+ TR = 4.3E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.9
*
.MODEL DIODE1 D
+ IS = 8E-015
+ N = 0.98
+ BV = 1000
+ IBV = 0.001
+ RS = 850
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
*
*.MODEL PBSS5160DS PNP
+ IS = 1.695E-013
+ NF = 0.9919
+ ISE = 1.5E-014
+ NE = 1.348
+ BF = 370
+ IKF = 0.4
+ VAF = 40
+ NR = 0.9912
+ ISC = 1.541E-013
+ NC = 1.821
+ BR = 30
+ IKR = 0.4
+ VAR = 18
+ RB = 12
+ IRB = 0.001
+ RBM = 1.12
+ RE = 0.06
+ RC = 0.105
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 9.466E-011
+ VJE = 0.8044
+ MJE = 0.3919
+ TF = 9E-010
+ XTF = 20
+ VTF = 1.1
+ ITF = 1.35
+ PTF = 0
+ CJC = 3.162E-011
+ VJC = 0.7543
+ MJC = 0.4479
+ XCJC = 1
+ TR = 3.2E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.8
*
.MODEL DIODE2 D
+ IS = 1.651E-014
+ N = 1.079
+ BV = 1000
+ IBV = 0.001
+ RS = 1000
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
.ENDS
Click to expand...


..SUBCKT PMD3001D 1 2 3 4 5 6
*
R1 2 3 0
R2 5 6 0
Q1 6 1 4 TR1
Q2 3 1 4 TR2
*
..MODEL TR1 NPN
+ IS = 1.967E-13
+ NF = 0.9876
+ ISE = 1.999E-13
+ NE = 2.5
+ BF = 480
+ IKF = 1
+ VAF = 85
+ NR = 0.9878
+ ISC = 1E-18
+ NC = 2.563
+ BR = 65
+ IKR = 5.5
+ VAR = 12
+ RB = 80
+ IRB = 3E-05
+ RBM = 0.6
+ RE = 0.053
+ RC = 0.073
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 1.158E-10
+ VJE = 0.5499
+ MJE = 0.3105
+ TF = 4.5E-10
+ XTF = 9
+ VTF = 3
+ ITF = 0.8
+ PTF = 0
+ CJC = 2.146E-11
+ VJC = 0.739
+ MJC = 0.4495
+ XCJC = 1
+ TR = 1.5E-08
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.5
*
..MODEL TR2 PNP
+ IS = 2.526E-013
+ NF = 0.9959
+ ISE = 1.056E-013
+ NE = 1.763
+ BF = 480
+ IKF = 0.49
+ VAF = 40
+ NR = 0.994
+ ISC = 5.238E-014
+ NC = 1.128
+ BR = 75
+ IKR = 0.3
+ VAR = 10
+ RB = 21
+ IRB = 0.00019
+ RBM = 0.2
+ RE = 0.085
+ RC = 0.095
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 9.2E-011
+ VJE = 0.8407
+ MJE = 0.4065
+ TF = 5.6E-010
+ XTF = 10
+ VTF = 1
+ ITF = 0.4
+ PTF = 0
+ CJC = 3.212E-011
+ VJC = 0.5149
+ MJC = 0.3901
+ XCJC = 1
+ TR = 6E-009
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.78
..ENDS
*


Hello Hammy,

The models om NXP are OK.
They don't have a parameer NF in the diode model.
The problem must be somewhere in your schematic.
Maybe your symbol is wrong. It has to be a subcircuit symbol.

Best regards,
Helmut
 
On Wed, 14 Apr 2010 22:15:46 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:


Hello Hammy,

The models om NXP are OK.
They don't have a parameer NF in the diode model.
The problem must be somewhere in your schematic.
Maybe your symbol is wrong. It has to be a subcircuit symbol.

Best regards,
Helmut
Click to expand...
Hi Helmut

Thanks for responding.

I'm using the default generic rectangle that model editor assigns to
parts. I'm following the data sheet pin out which seems to match-up
with the model text. Is there a specific subcircuit symbol? I did a
quick Google and seen no reference.

The schematic is pretty simple and works with other transistors.Its
just a push-pull buffer for an op amp. Here is a screen shot of the
schematic with the PBSS4160DPN.

http://i39.tinypic.com/2lkwahg.png


The data sheet pin out.

http://i40.tinypic.com/27yo3eu.png
 
On Wed, 14 Apr 2010 13:46:55 -0400, Hammy <spam@spam.com> wrote:

I keep getting these errors for NXP's dual BJT's. I'm using Capture
10.5, with PSPICE 10.5. I get similar errors with their PMD3001D
model.

This is the error I get with their PBSS4160DPN spice model

*Analysis directives:
.TRAN 0 100us 0 1u
.PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source PUSHPULL
R_R6 N09277 N00165 1k
R_R3 0 N09870 50
V_V2 N00833 0
+SIN 0 5 1000k 0 0 0
D_D1 N07581 N09467 D1N4148
V_V1 N00165 0 6
D_D2 N09277 N07581 D1N4148
R_R4 N07581 N00833 50
R_R5 N00229 N09467 1k
X_U2 N09870 N09277 N00229 N09870 N09467 N00165 PBSS4160DPN
V_V3 0 N00229 6

**** RESUMING ttutu.cir ****
.END


**** EXPANSION OF SUBCIRCUIT X_U2 ****
X_U2.Q1 N00165 N09277 N09870 X_U2.PBSS4160DS
X_U2.D1 N09277 N00165 X_U2.DIODE1
X_U2.Q2 N00229 N09467 N09870 X_U2.PBSS5160DS
X_U2.D2 N00229 N09467 X_U2.DIODE2
.MODEL X_U2.PBSS4160DS NPN IS 1.831E-013 NF 0.9823 ISE 3.486E-015 NE
+ 1.336 BF 490 IKF 0.15 VAF 10 NR 0.9825 ISC 1E-018 NC 1.821 BR 50
+ IKR 1.5 VAR 18 RB 19 IRB 0.00043 RBM 1.7 RE 0.025 RC 0.125 XTB 0 EG
+ 1.11 XTI 3 CJE 1.115E-010 VJE 0.57 MJE 0.308 TF 4.8E-010 XTF 8 VTF
+ 1.5 ITF 1.3 PTF 0 CJC 1.893E-011 VJC 0.6185 MJC 0.4452 XCJC 1 TR
+ 4.3E-008 CJS 0 VJS 0.75 MJS 0.333 FC 0.9
.MODEL X_U2.DIODE1 D IS 8E-015 N 0.98 BV 1000 IBV 0.001 RS 850 CJO 0
+ VJ 1 M 0.7 FC 0 TT 0 EG 1.11 XTI 3 IS 1.695E-013 NF
---------------------------------------------------$
ERROR -- 'NF' is not a model parameter name
??????


I get similar errors when using their PMD3001D model. Is this not a
Psice model or is it for another simulator?

The PMD3001D model is here ;
http://www.nxp.com/models/spicespar/PMD3001D.html

A C/P of the PBSS4160DPN spice model is below.

*
.SUBCKT PBSS4160DPN 1 2 3 4 5 6
*
Q1 6 2 1 PBSS4160DS
D1 2 6 DIODE1
Q2 3 5 4 PBSS5160DS
D2 3 5 DIODE2
*
* The diode does not reflect a
* physical device but improves
* only modeling in the reverse
* mode of operation.
*
.MODEL PBSS4160DS NPN
+ IS = 1.831E-013
+ NF = 0.9823
+ ISE = 3.486E-015
+ NE = 1.336
+ BF = 490
+ IKF = 0.15
+ VAF = 10
+ NR = 0.9825
+ ISC = 1E-018
+ NC = 1.821
+ BR = 50
+ IKR = 1.5
+ VAR = 18
+ RB = 19
+ IRB = 0.00043
+ RBM = 1.7
+ RE = 0.025
+ RC = 0.125
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 1.115E-010
+ VJE = 0.57
+ MJE = 0.308
+ TF = 4.8E-010
+ XTF = 8
+ VTF = 1.5
+ ITF = 1.3
+ PTF = 0
+ CJC = 1.893E-011
+ VJC = 0.6185
+ MJC = 0.4452
+ XCJC = 1
+ TR = 4.3E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.9
*
.MODEL DIODE1 D
+ IS = 8E-015
+ N = 0.98
+ BV = 1000
+ IBV = 0.001
+ RS = 850
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
*
*.MODEL PBSS5160DS PNP
+ IS = 1.695E-013
+ NF = 0.9919
+ ISE = 1.5E-014
+ NE = 1.348
+ BF = 370
+ IKF = 0.4
+ VAF = 40
+ NR = 0.9912
+ ISC = 1.541E-013
+ NC = 1.821
+ BR = 30
+ IKR = 0.4
+ VAR = 18
+ RB = 12
+ IRB = 0.001
+ RBM = 1.12
+ RE = 0.06
+ RC = 0.105
+ XTB = 0
+ EG = 1.11
+ XTI = 3
+ CJE = 9.466E-011
+ VJE = 0.8044
+ MJE = 0.3919
+ TF = 9E-010
+ XTF = 20
+ VTF = 1.1
+ ITF = 1.35
+ PTF = 0
+ CJC = 3.162E-011
+ VJC = 0.7543
+ MJC = 0.4479
+ XCJC = 1
+ TR = 3.2E-008
+ CJS = 0
+ VJS = 0.75
+ MJS = 0.333
+ FC = 0.8
*
.MODEL DIODE2 D
+ IS = 1.651E-014
+ N = 1.079
+ BV = 1000
+ IBV = 0.001
+ RS = 1000
+ CJO = 0
+ VJ = 1
+ M = 0.7
+ FC = 0
+ TT = 0
+ EG = 1.11
+ XTI = 3
.ENDS
Click to expand...
Hammy,
Take a look at your model library, the .lib, again. Notice on the
line for

*.MODEL PBSS5160DS PNP

that there is an '*' there. That is a comment symbol, so that line is
missing in the netlist. Remove the * and you should be back in
business!

Charlie
 
On Wed, 14 Apr 2010 16:07:45 -0700, Charlie E. <edmondson@ieee.org>
wrote:


Hammy,
Take a look at your model library, the .lib, again. Notice on the
line for

*.MODEL PBSS5160DS PNP

that there is an '*' there. That is a comment symbol, so that line is
missing in the netlist. Remove the * and you should be back in
business!

Charlie
Click to expand...
Thanks Charlie that did it!
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top