error in LTSpice III...Can't find definition of model.....

E

Elk

Guest
Hello,

I am trying to simulate BUZ272 in LTSpice, here is my buz272.mod file

*******
*p-MOSFET*100V 15A 0.3mOhm*Add_in_Line
.SUBCKT BUZ-272 1 2 3
LS 5 2 7N
LD 86 3 5N
RG 4 95 9.6
RS 5 76 56M
D272 86 76 DREV
.MODEL DREV D CJO=1.7N RS=20M TT=180N IS=300P BV=100
M272 102 95 76 76 MBUZ
.MODEL MBUZ PMOS VTO=-3.149 KP=1.761
M2 11 102 8 8 MSW
.MODEL MSW PMOS VTO=-0.001 KP=.5
M3 102 11 8 8 MSW
COX 11 8 700P
DGD 102 8 DCGD
.MODEL DCGD D CJO=692P M=0.659 VJ=1.029
CGS 76 95 2N
VGC 11 95 -10
* BESCHREIBT EINE IMPLANTIERTE LADUNG (VERSCHIEBT DIE EINSATZSPANNUNG)
MHELP 86 102 102 102 MVRD
.MODEL MVRD PMOS VTO=13 KP=0.8
LG 4 1 7N
.ENDS

And this is my buz272.asy, modified from on of the existing pmos models:
Version 4
SymbolType CELL
LINE Normal 48 48 48 96
LINE Normal 16 80 48 80
LINE Normal 16 48 24 48
LINE Normal 48 48 24 44
LINE Normal 48 48 24 52
LINE Normal 24 44 24 52
LINE Normal 16 8 16 24
LINE Normal 16 40 16 56
LINE Normal 16 72 16 88
LINE Normal 0 80 8 80
LINE Normal 8 16 8 80
LINE Normal 48 16 16 16
LINE Normal 48 0 48 16
WINDOW 0 56 32 Left 0
WINDOW 3 56 72 Left 0
SYMATTR Value BUZ-272
SYMATTR Prefix MP
SYMATTR SpiceModel C:\Programme\SwCADIII\lib\sym\buz272.mod
SYMATTR Description P-Channel MOSFET transistor
PIN 0 80 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 1
PIN 48 96 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 2
PIN 48 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 3


When I use this component in LTSpice, I get the error "Can't find
definition of model "c:\programme\swcadiii\lib\sym\buz272.mod"

Does anybody know what's wrong?

--
Message posted using http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad/
More information at http://www.talkaboutelectronicequipment.com/faq.html
 
On Tue, 01 Jul 2008 09:25:13 -0500, "Elk" <forum_user@gmx.net> wrote:

Hello,

I am trying to simulate BUZ272 in LTSpice, here is my buz272.mod file

*******
*p-MOSFET*100V 15A 0.3mOhm*Add_in_Line
SUBCKT BUZ-272 1 2 3
..SUBCKT BUZ-272 1 2 3
LS 5 2 7N
LD 86 3 5N
RG 4 95 9.6
RS 5 76 56M
D272 86 76 DREV
MODEL DREV D CJO=1.7N RS=20M TT=180N IS=300P BV=100
M272 102 95 76 76 MBUZ
MODEL MBUZ PMOS VTO=-3.149 KP=1.761
M2 11 102 8 8 MSW
MODEL MSW PMOS VTO=-0.001 KP=.5
M3 102 11 8 8 MSW
COX 11 8 700P
DGD 102 8 DCGD
MODEL DCGD D CJO=692P M=0.659 VJ=1.029
CGS 76 95 2N
VGC 11 95 -10
* BESCHREIBT EINE IMPLANTIERTE LADUNG (VERSCHIEBT DIE EINSATZSPANNUNG)
MHELP 86 102 102 102 MVRD
MODEL MVRD PMOS VTO=13 KP=0.8
LG 4 1 7N
ENDS
..ENDS

[snip]
Click to expand...

Note the required "dot" before SUBCKT and ENDS

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona 85048 Skype: Contacts Only | |
| Voice:(480)460-2350 Fax: Available upon request | Brass Rat |
| E-mail Icon at http://www.analog-innovations.com | 1962 |
| |
| Vote Barack... Help Make America an Obama-nation |
| |
| Due to excessive spam, googlegroups, UAR & AIOE are blocked! |
 
Hello Elk,

The Prefix in the symbol should be X, because it's a subcircuit model.

SYMATTR Prefix MP
-->
SYMATTR Prefix X


Normally you should set the X in the symbol editor of course.

I have sent you an example with a specific symbol for the BUZ272.
If your email-address doesn't work, please send me a valid email-address.

Either keep the model file in the directory of the schematic or
in the LTspice folder ...\Swcadiii\lib\sub\
You could also make a universal symbol for all subcircuit-Mosfets
with the pin-order G, S, D.


There is a large user group for LTspice.

http://tech.groups.yahoo.com/group/LTspice/

Best regards,
Helmut


"Elk" <forum_user@gmx.net> schrieb im Newsbeitrag
news:6f3524e63a13a2c80fae5c40b25a1e85@localhost.talkaboutelectronicequipment.com...
Hello,

I am trying to simulate BUZ272 in LTSpice, here is my buz272.mod file

*******
*p-MOSFET*100V 15A 0.3mOhm*Add_in_Line
.SUBCKT BUZ-272 1 2 3
LS 5 2 7N
LD 86 3 5N
RG 4 95 9.6
RS 5 76 56M
D272 86 76 DREV
.MODEL DREV D CJO=1.7N RS=20M TT=180N IS=300P BV=100
M272 102 95 76 76 MBUZ
.MODEL MBUZ PMOS VTO=-3.149 KP=1.761
M2 11 102 8 8 MSW
.MODEL MSW PMOS VTO=-0.001 KP=.5
M3 102 11 8 8 MSW
COX 11 8 700P
DGD 102 8 DCGD
.MODEL DCGD D CJO=692P M=0.659 VJ=1.029
CGS 76 95 2N
VGC 11 95 -10
* BESCHREIBT EINE IMPLANTIERTE LADUNG (VERSCHIEBT DIE EINSATZSPANNUNG)
MHELP 86 102 102 102 MVRD
.MODEL MVRD PMOS VTO=13 KP=0.8
LG 4 1 7N
.ENDS

And this is my buz272.asy, modified from on of the existing pmos models:
Version 4
SymbolType CELL
LINE Normal 48 48 48 96
LINE Normal 16 80 48 80
LINE Normal 16 48 24 48
LINE Normal 48 48 24 44
LINE Normal 48 48 24 52
LINE Normal 24 44 24 52
LINE Normal 16 8 16 24
LINE Normal 16 40 16 56
LINE Normal 16 72 16 88
LINE Normal 0 80 8 80
LINE Normal 8 16 8 80
LINE Normal 48 16 16 16
LINE Normal 48 0 48 16
WINDOW 0 56 32 Left 0
WINDOW 3 56 72 Left 0
SYMATTR Value BUZ-272
SYMATTR Prefix MP
SYMATTR SpiceModel C:\Programme\SwCADIII\lib\sym\buz272.mod
SYMATTR Description P-Channel MOSFET transistor
PIN 0 80 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 1
PIN 48 96 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 2
PIN 48 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 3


When I use this component in LTSpice, I get the error "Can't find
definition of model "c:\programme\swcadiii\lib\sym\buz272.mod"

Does anybody know what's wrong?

--
Message posted using
http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad/
More information at http://www.talkaboutelectronicequipment.com/faq.html
Click to expand...
 
Hello,

thank you very much. I got the email. It works fine know!

Thank You!

Best regards,
Sven

--
Message posted using http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad/
More information at http://www.talkaboutelectronicequipment.com/faq.html
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top