Pspice Mosfet Headaches

Hammy · Jun 7, 2007

I've been trying to use Fairchild's RFP30N06LE (logic level n-channel
Mosfet) Pspice model.

The datasheet with the model is here:

http://www.fairchildsemi.com/ds/RF/RFP30N06LE.pdf

The model fails to converge in a simple switching a resistive load
test cct, let alone the cct I want to use it in. I have tried all
typical approaches to resolve this such as relaxing the tolerances,
GMIN stepping, increasing ITL4 and skipping DC bias point. I've also
tried other mosfet models based on this same subcircuit and none of
them converge like the RF1S23N06LE and RF1S30N06LE. Placing the
FDN359AN in the exact same cct the cct converges, so I know there is
nothing wrong with the test cct.

I'm hoping someone knowledgeable in FET modeling could take a look at
the model and provide some insight. The model text is below as well.

Thank you.

PSPICE Electrical Model

SUBCKT RFP30N06LE 2 1 3; rev 6/2/93

CA 12 8 1 3.34e-9
CB 15 14 3.44e-9
CIN 6 8 0 1.343e-9

DBODY 7 5 DBDMOD
DBREAK 5 11 DBKMOD
DESD1 91 9 DESD1MOD
DESD2 91 7 DESD2MOD
DPLCAP 10 5 DPLCAPMOD

EBREAK 11 7 17 18 75.39
EDS 14 8 5 8 1
EGS 13 8 6 8 1
ESG 6 10 6 8 1
EVTO 20 6 18 8 1

IT 8 17 1

LDRAIN 2 5 1e-9
LGATE 1 9 7.22e-9
LSOURCE 3 7 6.31e-9

MOS1 16 6 8 8 MOSMOD M = 0.99
MOS2 16 21 8 8 MOSMOD M = 0.01

RBREAK 17 18 RBKMOD 1
RDRAIN 50 16 RDSMOD 11.86e-3
RGATE 9 20 2.52
RIN 6 8 1e9
RSCL1 5 51 RSLVCMOD 1e-6
RSCL2 5 50 1e3
RSOURCE 8 7 RDSMOD 26.6e-3
RVTO 18 19 RVTOMOD 1

S1A 6 12 13 8 S1AMOD
S1B 13 12 13 8 S1BMOD
S2A 6 15 14 13 S2AMOD
S2B 13 15 14 13 S2BMOD

VBAT 8 19 DC 1
VTO 21 6 0.5

ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))

..MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3 TRS2 =
6.08e-6 CJO = 1.05e-9 TT = 3.84e-8)
..MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
..MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5 TRS1 = 0
TRS2 = 0)
..MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4 TBV2 = -3.0e-6 RS = 0
TRS1 = 0 TRS2 = 0)
..MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)
..MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30 N = 10 TOX = 1 L
= 1u W = 1u)
..MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
..MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
..MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
..MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
..MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
..MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
..MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
..MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
..ENDS

Jim Thompson · Jun 7, 2007

That's not a model, that's an abortion, with all those
voltage-controlled switches. Does the FDN359AN have switches in its
subcircuit?

On Thu, 07 Jun 2007 11:50:17 GMT, Hammy <spamme@hotmail.com> wrote:

I've been trying to use Fairchild's RFP30N06LE (logic level n-channel
Mosfet) Pspice model.

The datasheet with the model is here:

http://www.fairchildsemi.com/ds/RF/RFP30N06LE.pdf

The model fails to converge in a simple switching a resistive load
test cct, let alone the cct I want to use it in. I have tried all
typical approaches to resolve this such as relaxing the tolerances,
GMIN stepping, increasing ITL4 and skipping DC bias point. I've also
tried other mosfet models based on this same subcircuit and none of
them converge like the RF1S23N06LE and RF1S30N06LE. Placing the
FDN359AN in the exact same cct the cct converges, so I know there is
nothing wrong with the test cct.

I'm hoping someone knowledgeable in FET modeling could take a look at
the model and provide some insight. The model text is below as well.

Thank you.

PSPICE Electrical Model

SUBCKT RFP30N06LE 2 1 3; rev 6/2/93

CA 12 8 1 3.34e-9
CB 15 14 3.44e-9
CIN 6 8 0 1.343e-9

[snip]
.MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
.MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
.MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
.MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
.MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
.MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
.MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
.MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
.ENDS

480)460-2350 | |
| E-mail Address at Website Fax

Hammy · Jun 7, 2007

On Thu, 07 Jun 2007 07:14:30 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@My-Web-Site.com> wrote:

That's not a model, that's an abortion, with all those
voltage-controlled switches. Does the FDN359AN have switches in its
subcircuit?

...Jim Thompson

Hi Jim:

Thanks for your response. Regarding your question I don't see any
VCS's in the FDN359AN. This is a more recent model made in 2002
according to the text.
This is the FDN359AN

..SUBCKT FDN359AN 20 10 30 50
*20=DRAIN 10=GATE 30=SOURCE 50=VTEMP
Rg 10 11x 1
Rdu 12x 1 1u
M1 2 1 4x 4x DMOS L=1u W=1u
..MODEL DMOS NMOS(VTO=1.9 KP=2.25E+1
+THETA=.1 VMAX=0.8E5 LEVEL=3)
Cgs 1 5x 420p
Rd 20 4 1.5E-2
Dds 5x 4 DDS
..MODEL DDS D(M=3.55E-1 VJ=6.33E-1 CJO=226p)
Dbody 5x 20 DBODY
..MODEL DBODY D(IS=4.96E-12 N=1.127089 RS=.001349 TT=12.63n)
Ra 4 2 1.5E-2
Rs 5x 5 0.5m
Ls 5 30 0.5n
M2 1 8 6 6 INTER
E2 8 6 4 1 2
..MODEL INTER NMOS(VTO=0 KP=10 LEVEL=1)
Cgdmax 7 4 260p
Rcgd 7 4 10meg
Dgd 6 4 DGD
Rdgd 6 4 10meg
..MODEL DGD D(M=7.3E-2 VJ=3.11E-1 CJO=260p)
M3 7 9 1 1 INTER
E3 9 1 4 1 -2
*ZX SECTION
EOUT 4x 6x poly(2) (1x,0) (3x,0) 0 0 0 0 1
FCOPY 0 3x VSENSE 1
RIN 1x 0 1G
VSENSE 6x 5x 0
RREF 3x 0 10m
*TEMP SECTION
ED 101 0 VALUE {V(50,100)}
VAMB 100 0 25
EKP 1x 0 101 0 .0195
*VTO TEMP SECTION
EVTO 102 0 101 0 .002
EVT 12x 11x 102 0 1
*DIODE THEMO BREAKDOWN SECTION
EBL VB1 VB2 101 0 .08
VBLK VB2 0 30
D 20 DB1 DBLK
..MODEL DBLK D(IS=1E-14 CJO=.1p RS=.1)
EDB DB1 0 VB1 0 1
..ENDS FDN359AN
*FDN359AN (Rev.A1) 5/15/02 **ST

This was my original choice for what I'm building, and then I got 20
RFP30N06LE for a good price (free) .The RFP30N06LE is overkill for
what I'm doing but easier to work with in a T0-220 packages, versus
the microscopic SOT-23 of the FDN359AN.

I'm sure I can find other uses for RFP30N06LE which is why I'm
interested in the model.

Helmut Sennewald · Jun 7, 2007

"Hammy" <spamme@hotmail.com> schrieb im Newsbeitrag
news

trf63lefn47gfbof2sthtrr8meu7vjtmb@4ax.com...

I've been trying to use Fairchild's RFP30N06LE (logic level n-channel
Mosfet) Pspice model.

The datasheet with the model is here:

http://www.fairchildsemi.com/ds/RF/RFP30N06LE.pdf

The model fails to converge in a simple switching a resistive load
test cct, let alone the cct I want to use it in. I have tried all
typical approaches to resolve this such as relaxing the tolerances,
GMIN stepping, increasing ITL4 and skipping DC bias point. I've also
tried other mosfet models based on this same subcircuit and none of
them converge like the RF1S23N06LE and RF1S30N06LE. Placing the
FDN359AN in the exact same cct the cct converges, so I know there is
nothing wrong with the test cct.

I'm hoping someone knowledgeable in FET modeling could take a look at
the model and provide some insight. The model text is below as well.

Thank you.

Hello Hammy,

I have tried to run the subcircuit and got error messages.

How have you solved the the two erros in the subcircuit
regarding the three pins of the capacitors?

CA 12 8 1 3.34e-9
CA 12 8 3.34e-9

CIN 6 8 0 1.343e-9
CIN 6 8 1.343e-9

One more change.

SUBCKT RFP30N06LE 2 1 3; rev 6/2/93
..SUBCKT RFP30N06LE 2 1 3

I have tested the "repaired" model with LTspice and PSPICE demo 10.5.
My test circuit has worked in both simulators.

Where is your netlist?
---------------------

Best regards,
Helmut

PSPICE Electrical Model

SUBCKT RFP30N06LE 2 1 3; rev 6/2/93

CA 12 8 1 3.34e-9
CB 15 14 3.44e-9
CIN 6 8 0 1.343e-9

DBODY 7 5 DBDMOD
DBREAK 5 11 DBKMOD
DESD1 91 9 DESD1MOD
DESD2 91 7 DESD2MOD
DPLCAP 10 5 DPLCAPMOD

EBREAK 11 7 17 18 75.39
EDS 14 8 5 8 1
EGS 13 8 6 8 1
ESG 6 10 6 8 1
EVTO 20 6 18 8 1

IT 8 17 1

LDRAIN 2 5 1e-9
LGATE 1 9 7.22e-9
LSOURCE 3 7 6.31e-9

MOS1 16 6 8 8 MOSMOD M = 0.99
MOS2 16 21 8 8 MOSMOD M = 0.01

RBREAK 17 18 RBKMOD 1
RDRAIN 50 16 RDSMOD 11.86e-3
RGATE 9 20 2.52
RIN 6 8 1e9
RSCL1 5 51 RSLVCMOD 1e-6
RSCL2 5 50 1e3
RSOURCE 8 7 RDSMOD 26.6e-3
RVTO 18 19 RVTOMOD 1

S1A 6 12 13 8 S1AMOD
S1B 13 12 13 8 S1BMOD
S2A 6 15 14 13 S2AMOD
S2B 13 15 14 13 S2BMOD

VBAT 8 19 DC 1
VTO 21 6 0.5

ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))

.MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3 TRS2 =
6.08e-6 CJO = 1.05e-9 TT = 3.84e-8)
.MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
.MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5 TRS1 = 0
TRS2 = 0)
.MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4 TBV2 = -3.0e-6 RS = 0
TRS1 = 0 TRS2 = 0)
.MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)
.MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30 N = 10 TOX = 1 L
= 1u W = 1u)
.MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
.MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
.MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
.MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
.MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
.MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
.MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
.MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
.ENDS

Hammy · Jun 7, 2007

On Thu, 7 Jun 2007 17:40:10 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:

"Hammy" <spamme@hotmail.com> schrieb im Newsbeitrag
newstrf63lefn47gfbof2sthtrr8meu7vjtmb@4ax.com...

Hello Hammy,

I have tried to run the subcircuit and got error messages.

How have you solved the the two erros in the subcircuit
regarding the three pins of the capacitors?

CA 12 8 1 3.34e-9
CA 12 8 3.34e-9

CIN 6 8 0 1.343e-9
CIN 6 8 1.343e-9

One more change.
SUBCKT RFP30N06LE 2 1 3; rev 6/2/93
.SUBCKT RFP30N06LE 2 1 3

I have tested the "repaired" model with LTspice and PSPICE demo 10.5.
My test circuit has worked in both simulators.

Where is your netlist?
---------------------

Best regards,
Helmut

Hi Helmut:

Thanks for your assistance. I did the corrections you suggested (I'm
using OrCAD demo 10.5 to), but I still get convergence problems. I
also get several errors in my output file.

This is my test circuit netlist.

* source FRFTR
R_R8 N81164 N81004 2
V_V4 N81004 0 44
X_U1 N81164 N80914 0 RFP30N06LE/HA
R_R12 0 N80914 22k
V_V5 N81706 0
+PULSE 0 5 0 20n 20n 3.82u 26u
R_R14 N81706 N80914 22

This is my output file section with errors.

ERROR -- End of expression not seen
..MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5 TRS1 = 0
TRS2 = 0)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4 TBV2 = -3.0e-6 RS = 0
TRS1 = 0 TRS2 = 0)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30 N = 10 TOX = 1 L=
1u W = 1u)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
-----------------------------------------------------------------------------------------------------$
ERROR -- End of expression not seen
..ENDS

Hammy · Jun 7, 2007

On Thu, 07 Jun 2007 16:43:08 GMT, Hammy <spamme@hotmail.com> wrote:

X_U1 N81164 N80914 0 RFP30N06LE/HA

Hi Helmut:

A correction to my netlist, for this line:

X_U1 N81164 N80914 0 RFP30N06LE/HA

Should be just:

X_U1 N81164 N80914 0 RFP30N06LE

Thanks for any assistance.

Helmut Sennewald · Jun 7, 2007

"Hammy" <spamme@hotmail.com> schrieb im Newsbeitrag
news:s7dg63l2ab4plj160hdu3bnjoo9k3ir874@4ax.com...

On Thu, 7 Jun 2007 17:40:10 +0200, "Helmut Sennewald"
helmutsennewald@t-online.de> wrote:

"Hammy" <spamme@hotmail.com> schrieb im Newsbeitrag
newstrf63lefn47gfbof2sthtrr8meu7vjtmb@4ax.com...

Hello Hammy,

I have tried to run the subcircuit and got error messages.

How have you solved the the two erros in the subcircuit
regarding the three pins of the capacitors?

CA 12 8 1 3.34e-9
CA 12 8 3.34e-9

CIN 6 8 0 1.343e-9
CIN 6 8 1.343e-9

One more change.
SUBCKT RFP30N06LE 2 1 3; rev 6/2/93
.SUBCKT RFP30N06LE 2 1 3

I have tested the "repaired" model with LTspice and PSPICE demo 10.5.
My test circuit has worked in both simulators.

Where is your netlist?
---------------------

Best regards,
Helmut

Hi Helmut:

Thanks for your assistance. I did the corrections you suggested (I'm
using OrCAD demo 10.5 to), but I still get convergence problems. I
also get several errors in my output file.

This is my test circuit netlist.

* source FRFTR
R_R8 N81164 N81004 2
V_V4 N81004 0 44
X_U1 N81164 N80914 0 RFP30N06LE/HA
R_R12 0 N80914 22k
V_V5 N81706 0
+PULSE 0 5 0 20n 20n 3.82u 26u
R_R14 N81706 N80914 22

Hello Hammy,

And here is the working example.
You have overlooked the broken lines. The SPICE syntax
requires a "+" character in the first column for multiline SPICE-lines.

May I mention that I got with two mouse clicks the average power
dissipation of the MOSFET with LTspice. It's 4.86Watt in your example.
..
Best regards,
Helmut

Netlist "RFP30N06E_test2.cir"

* RFP30N06LE_test2.asc
XM1 DRAIN GATE 0 RFP30N06LE
V1 VG 0 PULSE 0 5 0 20n 20n 3.82u 26u
V2 V44 0 44
RL V44 DRAIN 2
RG GATE 0 22k
RS VG GATE 22
..include RFP30N06LE.lib
* .dc V1 0 4 10m
..tran 0 100u 0 1u
..probe
..end

Library file "RFP30N06LE.lib"
Hopefully the lines are short enough for your news reader.

* Fairchild
* PSPICE Electrical Model
*; rev 6/2/93
* PSPICE Electrical Model
..SUBCKT RFP30N06LE 2 1 3
*CA 12 8 1 3.34e-9
CA 12 8 3.34e-9
CB 15 14 3.44e-9
*CIN 6 8 0 1.343e-9
CIN 6 8 1.343e-9
DBODY 7 5 DBDMOD
DBREAK 5 11 DBKMOD
DESD1 91 9 DESD1MOD
DESD2 91 7 DESD2MOD
DPLCAP 10 5 DPLCAPMOD
EBREAK 11 7 17 18 75.39
EDS 14 8 5 8 1
EGS 13 8 6 8 1
ESG 6 10 6 8 1
EVTO 20 6 18 8 1
IT 8 17 1
LDRAIN 2 5 1e-9
LGATE 1 9 7.22e-9
LSOURCE 3 7 6.31e-9
MOS1 16 6 8 8 MOSMOD M = 0.99
MOS2 16 21 8 8 MOSMOD M = 0.01
RBREAK 17 18 RBKMOD 1
RDRAIN 50 16 RDSMOD 11.86e-3
RGATE 9 20 2.52
RIN 6 8 1e9
RSCL1 5 51 RSLVCMOD 1e-6
RSCL2 5 50 1e3
RSOURCE 8 7 RDSMOD 26.6e-3
RVTO 18 19 RVTOMOD 1
S1A 6 12 13 8 S1AMOD
S1B 13 12 13 8 S1BMOD
S2A 6 15 14 13 S2AMOD
S2B 13 15 14 13 S2BMOD
VBAT 8 19 DC 1
VTO 21 6 0.5
ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))}
..MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3
+ TRS2 = 6.08e-6 CJO = 1.05e-9 TT = 3.84e-8)
..MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
..MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5
+ TRS1 = 0 TRS2 = 0)
..MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4
+ TBV2 = -3.0e-6 RS = 0 TRS1 = 0 TRS2 = 0)
..MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)
..MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30
+ N = 10 TOX = 1 L = 1u W = 1u)
..MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
..MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
..MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
..MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
..MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
..MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
..MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
..MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
..ENDS
* NOTE: For further discussion of the PSPICE model,
* consult A New PSPICE Sub-Circuit for the Power MOSFET
* Featuring Global Temperature Options;
* IEEE Power Electronics Specialist Conference Records 1991.

Hammy · Jun 7, 2007

On Thu, 7 Jun 2007 19:43:25 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:

"Hammy" <spamme@hotmail.com> schrieb im Newsbeitrag
news:s7dg63l2ab4plj160hdu3bnjoo9k3ir874@4ax.com...
On Thu, 7 Jun 2007 17:40:10 +0200, "Helmut Sennewald"
helmutsennewald@t-online.de> wrote:

Hello Hammy,

And here is the working example.
You have overlooked the broken lines. The SPICE syntax
requires a "+" character in the first column for multiline SPICE-lines.

May I mention that I got with two mouse clicks the average power
dissipation of the MOSFET with LTspice. It's 4.86Watt in your example.
.
Best regards,
Helmut

Netlist "RFP30N06E_test2.cir"

* RFP30N06LE_test2.asc
XM1 DRAIN GATE 0 RFP30N06LE
V1 VG 0 PULSE 0 5 0 20n 20n 3.82u 26u
V2 V44 0 44
RL V44 DRAIN 2
RG GATE 0 22k
RS VG GATE 22
.include RFP30N06LE.lib
* .dc V1 0 4 10m
.tran 0 100u 0 1u
.probe
.end

Library file "RFP30N06LE.lib"
Hopefully the lines are short enough for your news reader.

* Fairchild
* PSPICE Electrical Model
*; rev 6/2/93
* PSPICE Electrical Model
.SUBCKT RFP30N06LE 2 1 3
*CA 12 8 1 3.34e-9
CA 12 8 3.34e-9
CB 15 14 3.44e-9
*CIN 6 8 0 1.343e-9
CIN 6 8 1.343e-9
DBODY 7 5 DBDMOD
DBREAK 5 11 DBKMOD
DESD1 91 9 DESD1MOD
DESD2 91 7 DESD2MOD
DPLCAP 10 5 DPLCAPMOD
EBREAK 11 7 17 18 75.39
EDS 14 8 5 8 1
EGS 13 8 6 8 1
ESG 6 10 6 8 1
EVTO 20 6 18 8 1
IT 8 17 1
LDRAIN 2 5 1e-9
LGATE 1 9 7.22e-9
LSOURCE 3 7 6.31e-9
MOS1 16 6 8 8 MOSMOD M = 0.99
MOS2 16 21 8 8 MOSMOD M = 0.01
RBREAK 17 18 RBKMOD 1
RDRAIN 50 16 RDSMOD 11.86e-3
RGATE 9 20 2.52
RIN 6 8 1e9
RSCL1 5 51 RSLVCMOD 1e-6
RSCL2 5 50 1e3
RSOURCE 8 7 RDSMOD 26.6e-3
RVTO 18 19 RVTOMOD 1
S1A 6 12 13 8 S1AMOD
S1B 13 12 13 8 S1BMOD
S2A 6 15 14 13 S2AMOD
S2B 13 15 14 13 S2BMOD
VBAT 8 19 DC 1
VTO 21 6 0.5
ESCL 51 50 VALUE = {(V(5,51)/ABS(V(5,51)))*(PWR(V(5,51)*1e6/89,7))}
.MODEL DBDMOD D (IS = 3.80e-13 RS = 1.12e-2 TRS1 = 1.61e-3
+ TRS2 = 6.08e-6 CJO = 1.05e-9 TT = 3.84e-8)
.MODEL DBKMOD D (RS = 1.82e-1 TRS1 = 7.50e-3 TRS2 = -4.0e-5)
.MODEL DESD1MOD D (BV = 13.54 TBV1 = 0 TBV2 = 0 RS = 45.5
+ TRS1 = 0 TRS2 = 0)
.MODEL DESD2MOD D (BV = 11.46 TBV1 = -7.576e-4
+ TBV2 = -3.0e-6 RS = 0 TRS1 = 0 TRS2 = 0)
.MODEL DPLCAPMOD D (CJO = 0.591e-9 IS = 1e-30 N = 10)
.MODEL MOSMOD NMOS (VTO = 1.94 KP = 139.2 IS = 1e-30
+ N = 10 TOX = 1 L = 1u W = 1u)
.MODEL RBKMOD RES (TC1 = 1.07e-3 TC2 = -3.03e-7)
.MODEL RDSMOD RES (TC1 = 5.38e-3 TC2 = 1.64e-5)
.MODEL RSLVCMOD RES (TC1 = 1.75e-3 TC2 = 3.90e-6)
.MODEL RVTOMOD RES (TC1 = -2.15e-3 TC2 = -5.43e-6)
.MODEL S1AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -4.05 VOFF = -1.5)
.MODEL S1BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -1.5 VOFF = -4.05)
.MODEL S2AMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = -2.2 VOFF = 2.8)
.MODEL S2BMOD VSWITCH (RON = 1e-5 ROFF = 0.1 VON = 2.8 VOFF = -2.2)
.ENDS
* NOTE: For further discussion of the PSPICE model,
* consult A New PSPICE Sub-Circuit for the Power MOSFET
* Featuring Global Temperature Options;
* IEEE Power Electronics Specialist Conference Records 1991.

Hi Helmut:

Thank you for your patience. The problem still persists.

I tried to run your netlist and got the following error:

ERROR -- Less than 2 connections at node DRAIN

I then copied your model text with the corrections over the existing
model txt. This took care of all the syntax errors (or at least Pspice
isn't reporting them).The output file is below. The same test cct I
posted earlier.

ERROR -- Convergence problem in transient analysis at Time = 185.5E-09
Time step = 2.028E-15, minimum allowable step size =
4.000E-15

These voltages failed to converge:

V(X_U1.12) = 3.091V \ 3.189V
V(X_U1.8) = 606.39mV \ 705.10mV
V(X_U1.15) = 3.090V \ 3.189V
V(X_U1.14) = 1.744V \ 1.843V
V(X_U1.6) = 3.091V \ 3.189V
V(X_U1.7) = 42.26mV \ 140.97mV
V(X_U1.5) = 1.744V \ 1.843V
V(X_U1.11) = 75.43V \ 75.53V
V(X_U1.91) = 189.52mV \ 288.23mV
V(X_U1.9) = 3.286V \ 3.384V
V(X_U1.10) = 606.39mV \ 705.10mV
V(X_U1.17) = 1.606V \ 1.705V
V(X_U1.18) = 606.39mV \ 705.10mV
V(X_U1.13) = 3.091V \ 3.189V
V(X_U1.20) = 3.090V \ 3.189V
V(X_U1.16) = 1.495V \ 1.594V
V(X_U1.21) = 3.591V \ 3.689V
V(X_U1.50) = 1.746V \ 1.844V
V(X_U1.51) = 1.744V \ 1.843V
V(X_U1.19) = -393.61mV \ -294.90mV

These devices failed to converge:
X_U1.ESCL

ERROR -- Discontinuing simulation due to convergence problem

Last node voltages tried were:

NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE

(N80914) 3.2938 (N81004) 44.0000 (N81706) 5.0000 (X_U1.5)
1.7439

(X_U1.6) 3.0905 (X_U1.7) .0423 (X_U1.8) .6064 (X_U1.9)
3.2855

(N810301) 1.7616 (X_U1.10) .6064
(X_U1.11) 75.4320 (X_U1.12) 3.0905
(X_U1.13) 3.0905 (X_U1.14) 1.7439
(X_U1.15) 3.0904 (X_U1.16) 1.4948
(X_U1.17) 1.6064 (X_U1.18) .6064
(X_U1.19) -.3936 (X_U1.20) 3.0904
(X_U1.21) 3.5905 (X_U1.50) 1.7455
(X_U1.51) 1.7439 (X_U1.91) .1895

**** Interrupt ****

As you may have guessed I'm not exactly an expert on spice.

Could this be the problem "X_U1.ESCL" What exactly does ESCL stand for
on the model schematic the symbol looks like a DC source?

I like LTSpice too but it doesn't have a layout tool.

Helmut Sennewald · Jun 7, 2007

Hello Hammy,

I have sent my files to your email address. Please try it.

Just open the .cir file with PSPICE-AD and press RUN(-&gt

.

Have you changed the default convergence settings?

I recommend you send me your files for a check.
You can tell me a lot about your netlist and library file,
but I only believe that when I can verify this with your files.

Best regards,
Helmut

I like LTSpice too but it doesn't have a layout tool.

If you don't simulate the whole board, you have to change
the schematic anyway for PSPICE.
So it's not so far from drawing it again in another tool.

Hammy · Jun 7, 2007

On Thu, 7 Jun 2007 22:43:52 +0200, "Helmut Sennewald"
<helmutsennewald@t-online.de> wrote:

Hello Hammy,

I have sent my files to your email address. Please try it.

Just open the .cir file with PSPICE-AD and press RUN(-&gt.

Have you changed the default convergence settings?

I recommend you send me your files for a check.
You can tell me a lot about your netlist and library file,
but I only believe that when I can verify this with your files.

Best regards,
Helmut

I like LTSpice too but it doesn't have a layout tool.

If you don't simulate the whole board, you have to change
the schematic anyway for PSPICE.
So it's not so far from drawing it again in another tool.

Hi Helmut:

Thanks much for your help it's working!!

I set all simulation settings to there default,and it worked.

You will probably get your email back the email addy with my name is
bogus. Sorry but I'm new to newsgroup posting,and didnt want to get
more "spam". My email address is max0412@hotmail.com .

Again thanks alot you saved me a lot of time,hopefully I can return
the favour in the future.

Kevin Aylward · Jun 9, 2007

Helmut Sennewald wrote:

May I mention that I got with two mouse clicks the average power
dissipation of the MOSFET with LTspice. It's 4.86Watt in your example.
.

May I mention that with no mouse clicks I get the average power of any
device in SuperSpice

--
Kevin Aylward
kaEXTRACT@anasoft.co.uk
www.anasoft.co.uk

Pspice Mosfet Headaches

Hammy

Guest

Jim Thompson

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Kevin Aylward

Guest

Welcome to EDABoard.com

Sponsor

Online statistics

Forum statistics

Pspice Mosfet Headaches

Hammy

Guest

Jim Thompson

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Helmut Sennewald

Guest

Hammy

Guest

Kevin Aylward

Guest

Log in

Welcome to EDABoard.com

Sponsor