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

Thread view:

Enable EMail Alerts

Start New Thread

Thread rating:

Elk - 01 Jul 2008 15:25 GMT

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 fin
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.htm

Reply to this Message

Jim Thompson - 01 Jul 2008 16:29 GMT

>Hello,
>
[quoted text clipped - 3 lines]
>*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
[quoted text clipped - 17 lines]
>LG 4 1 7N
>ENDS

.ENDS <<<<

[snip]

Note the required "dot" before SUBCKT and ENDS

...Jim Thompson

Reply to this Message

Elk - 01 Jul 2008 18:15 GMT

The dots are there. I tried to create the *.mod and *.asy new. But it i
the same error.

-
Message posted using http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad
More information at http://www.talkaboutelectronicequipment.com/faq.htm

Reply to this Message

Helmut Sennewald - 01 Jul 2008 20:56 GMT

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

> Hello,
>
[quoted text clipped - 66 lines]
> http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad/
> More information at http://www.talkaboutelectronicequipment.com/faq.html

Reply to this Message

Elk - 02 Jul 2008 16:35 GMT

Hello,

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

Thank You!

Best regards,
Sve

-
Message posted using http://www.talkaboutelectronicequipment.com/group/sci.electronics.cad
More information at http://www.talkaboutelectronicequipment.com/faq.htm

Reply to this Message

Electronics Forum / CAD / July 2008

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