LTSpice - some help with model needed

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Jump to Latest
C

Cybergent

Member
Joined 2004
I´m just trying a simulation of a switcher application.

There I want to use the IRF3805 - TO220.

http://www.irf.com/product-info/datasheets/data/irf3805.pdf

I checked on the IRF site for a model, but only found a very complicated thing, that has not very much in common with the NMOS Models already used in LTSpice.



This is the listing from IRF:

irf3805sl.spi

Code: 
.SUBCKT irf3805sl 1 2 3
* SPICE3 MODEL WITH THERMAL RC NETWORK 
**************************************
*      Model Generated by MODPEX     *
*Copyright(c) Symmetry Design Systems*
*         All Rights Reserved        *
*    UNPUBLISHED LICENSED SOFTWARE   *
*   Contains Proprietary Information *
*      Which is The Property of      *
*     SYMMETRY OR ITS LICENSORS      *
*Commercial Use or Resale Restricted *
*   by Symmetry License Agreement    *
**************************************
* Model generated on Dec 20, 04
* MODEL FORMAT: SPICE3
* Symmetry POWER MOS Model (Version 1.0)
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source
M1 9 7 8 8 MM L=100u W=100u
.MODEL MM NMOS LEVEL=1 IS=1e-32
+VTO=4.40718 LAMBDA=0 KP=113.534
+CGSO=7.35603e-05 CGDO=1.00004e-11
RS 8 3 0.00051393
D1 3 1 MD
.MODEL MD D IS=9.5779e-12 RS=0.00152807 N=0.957587 BV=55
+IBV=0.00025 EG=1.2 XTI=4 TT=1e-07
+CJO=4.25081e-09 VJ=0.5 M=0.483198 FC=0.1
RDS 3 1 1e+07
RD 9 1 0.00054364
RG 2 7 3.7209
D2 4 5 MD1
* Default values used in MD1:
*   RS=0 EG=1.11 XTI=3.0 TT=0
*   BV=infinite IBV=1mA
.MODEL MD1 D IS=1e-32 N=50
+CJO=2.76986e-09 VJ=0.5 M=0.381028 FC=1e-08
D3 0 5 MD2
* Default values used in MD2:
*   EG=1.11 XTI=3.0 TT=0 CJO=0
*   BV=infinite IBV=1mA
.MODEL MD2 D IS=1e-10 N=0.4 RS=3e-06
RL 5 10 1
FI2 7 9 VFI2 -1
VFI2 4 0 0
EV16 10 0 9 7 1
CAP 11 10 9.50196e-09
FI1 7 9 VFI1 -1
VFI1 11 6 0
RCAP 6 10 1
D4 0 6 MD3
* Default values used in MD3:
*   EG=1.11 XTI=3.0 TT=0 CJO=0
*   RS=0 BV=infinite IBV=1mA
.MODEL MD3 D IS=1e-10 N=0.4
.ENDS irf3805sl

*SPICE 2-Layer Thermal Model Subcircuit
.SUBCKT irf3805slt 2 0

R_RTHERM1         2 1  0.23878
C_CTHERM1         2 0  0.004255
R_RTHERM2         1 0  0.21056
C_CTHERM2         1 0  0.060865

.ENDS irf3805slt



I tried to extract those informations, that looked reasonable to me and made this model according to the structures I found in LTSpice:



Code: 
.model IRF3805 VDMOS(Rg=3.7 Rd=0.5m Rs=0.5m Vto=4.4 Kp=75 Rb=0.5m L=100u W=100u Cgs=8n Qg=200n mfg=International_Rectifier Vds=55 Ron=3.3m)



Basically this works like a MOSFET, but the switching timing is completely wrong.


The IRF3805 is supposed to behave like this:

Ton delay: 150ns
Trise: 20ns
Toff delay: 93ns
Tfall: 87ns


In the simulatuion it just switches within a few ns. No delay visible. Vth also seems not to be correct.

Sorry, I´m quite new to this simulation stuff and I´m just beginning to scratch the surface with this.

So I have absolutely no idea, what I need to change, to get this thing going. Everything I tried myself did not help.

So please anyone help. Thanks! :)
 
C

Christer

Member
Joined 2002
It is a subcircuit model, not a plan NMOS model. That is quite common, but you can't just add it to the model file. Save the file in the directory lib/sub as file irf3805.sub Then you need a symbol file for it, which is essentially the same as the generic file nmos.asy but with additional info about which model file to use. You can use the attached file for 2sk1058 and do the obvious changes. Put this file in lib/sym or even better create a lib/sym/transistors to put it in.

To sum up, you need two files

lib/sub/irf3805.sub - the one from IR
lib/sym/transistors/irf3805.sub - hack my file below


File 2sk1058.asy:
-------------------------

Version 3
SymbolType CELL
LINE Normal 12 12 12 24
LINE Normal 4 20 12 20
LINE Normal 10 12 12 12
LINE Normal 4 12 10 11
LINE Normal 4 12 10 13
LINE Normal 10 11 10 13
LINE Normal 4 2 4 6
LINE Normal 4 10 4 14
LINE Normal 4 18 4 22
LINE Normal 0 20 2 20
LINE Normal 2 4 2 20
LINE Normal 12 4 4 4
LINE Normal 12 0 12 4
WINDOW 0 14 8 Left 0
WINDOW 3 14 18 Left 0
SYMATTR Prefix X
SYMATTR SpiceModel 2sk1058.mod
SYMATTR Value 2SK1058
SYMATTR Value2 2SK1058
SYMATTR Description N-Channel MOSFET transistor
PIN 0 20 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 12 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 12 24 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3
 
C

Cybergent

Member
Joined 2004
Christer said:
To sum up, you need two files

lib/sub/irf3805.sub - the one from IR
lib/sym/transistors/irf3805.sub - hack my file below
Click to expand...

The second file needs to be named:
lib/sym/transistors/irf3805.asy

But then I got it working. Many thanks.

The simulation behavior ist still not quite like the real thing on the workbench, but it is much closer now.
Looks like the IRF model is not absolutely perfect. Hopefully I can get it adjusted.
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Top Bottom