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@[EMAIL PROTECTED]
> schrieb im Newsbeitrag
news:6f3524e63a13a2c80fae5c40b25a1e85@[EMAIL PROTECTED]
> 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
>
|
