BUZ90x SPICE models - diyAudio
Go Back   Home > Forums > Amplifiers > Solid State

Solid State Talk all about solid state amplification.

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 22nd June 2006, 09:34 AM   #1
diyAudio Member
 
teodorom's Avatar
 
Join Date: Apr 2004
Location: Milano
Default BUZ90x SPICE models

Hi,
does anybody have the (P)SPICE models for the power mosfets BUZ900/901 and BUZ905/906 ?
Thanks
__________________
Teodoro
  Reply With Quote
Old 22nd June 2006, 10:25 AM   #2
diyAudio Member
 
Join Date: Sep 2002
Location: Sweden
According to Charles Hanssen in an earlier thread both Magnatec and Exicon use exactly the same Semelab chips in their lateral MOSFETs, so the Exicon models should work fine.
http://www.diyaudio.com/forums/showt...238#post171238
  Reply With Quote
Old 22nd June 2006, 11:33 AM   #3
cs is offline cs  United Kingdom
diyAudio Member
 
Join Date: Jun 2005
Location: .
Here they are.
(I got the models directly from Magnatec).

.SUBCKT BUZ901D 1 2 3
* MODEL FORMAT: SPICE Level 1
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source

M1 9 7 8 8 MM L=0.001 W=0.001
* Default values used in M:
* The capacitances are added externally
* Other default values are:
* RS=0 RD=0 LD=0 CBD=0 CBS=0 CGBO=0
.MODEL MM NMOS LEVEL=1 IS=1e-32
+VTO=0.362 LAMBDA=0.06 KP=3.097
RS 8 3 0.178
D1 8 9 MD
.MODEL MD D IS=1.0e-32 N=50 BV=250
+CJO=1.77e-9 VJ=0.1 M=0.28
RDS 8 9 1e+06
RD 9 1 0.265
RG 2 7 42
* Gate Source capacitance Cgs0
CAP1 7 8 900e-12
*************************
* Gate Drain capacitance Cdg0
CAP 7 4 18.7e-12
*************************
* Gate Drain Capacitance Cdgj0
* Modelled as a diode
D2 4 9 MDD
.MODEL MDD D IS=1e-32 N=50
+CJO=75e-12 VJ=0.1 M=0.768
*************************
.ENDS BUZ901D

.SUBCKT BUZ901P 1 2 3

* MODEL FORMAT: SPICE Level 1
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source

M1 9 7 8 8 MM L=0.001 W=0.001
* Default values used in M:
* The capacitances are added externally
* Other default values are:
* RS=0 RD=0 LD=0 CBD=0 CBS=0 CGBO=0
.MODEL MM NMOS LEVEL=1 IS=1e-32
+VTO=0.473 LAMBDA=0.092 KP=1.585
RS 8 3 0.41
D1 8 9 MD
.MODEL MD D IS=1.0e-32 N=50 BV=250
+CJO=1.0e-9 VJ=0.7 M=0.5
RDS 8 9 1e+06
RD 9 1 0.58
RG 2 7 80
* Gate Source capacitance Cgs0
CAP1 7 8 400e-12
*************************
* Gate Drain capacitance Cdg0
CAP 7 4 10.5e-12
*************************
* Gate Drain Capacitance Cdgj0
* Modelled as a diode
D2 4 9 MDD
.MODEL MDD D IS=1e-32 N=50
+CJO=94.8e-12 VJ=0.3 M=1
*************************
.ENDS BUZ901P

.SUBCKT BUZ906d 1 2 3

* MODEL FORMAT: SPICE Level 1
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source

M1 9 7 8 8 MM L=0.001 W=0.001
* Default values used in M:
* The capacitances are added externally
* Other default values are:
* RS=0 RD=0 LD=0 CBD=0 CBS=0 CGBO=0
.MODEL MM PMOS LEVEL=1 IS=1e-32
+VTO=-0.273 LAMBDA=0.5 KP=0.548
RS 8 3 0.171
D1 9 8 MD
.MODEL MD D IS=1.0e-32 N=50 BV=250
+CJO=1e-9 VJ=0.7 M=0.5
RDS 8 9 1e+06
RD 9 1 0.259
RG 2 7 45
* Gate Source capacitance Cgs0
CAP1 7 8 1.08e-9
*************************
* Gate Drain capacitance Cdg0
CAP 7 4 36e-12
*************************
* Gate Drain Capacitance Cdgj0
* Modelled as double diode
D2 9 10 MDD
D3 4 10 MDD
.MODEL MDD D IS=1e-32 N=50
+CJO=762e-12 VJ=0.1 M=1
*************************
.ENDS BUZ906d

.SUBCKT BUZ906P 1 2 3
* MODEL FORMAT: SPICE Level 1
* External Node Designations
* Node 1 -> Drain
* Node 2 -> Gate
* Node 3 -> Source

M1 9 7 8 8 MM L=0.001 W=0.001
* Default values used in M:
* The capacitances are added externally
* Other default values are:
* RS=0 RD=0 LD=0 CBD=0 CBS=0 CGBO=0
.MODEL MM PMOS LEVEL=1 IS=1e-32
+VTO=-0.426 LAMBDA=0.073 KP=0.673
RS 8 3 0.342
D1 9 8 MD
.MODEL MD D IS=1.0e-32 N=50 BV=250
+CJO=1.45e-9 VJ=0.446 M=0.377
RDS 8 9 1e+06
RD 9 1 0.523
RG 2 7 45.2
* Gate Source capacitance Cgs0
CAP1 7 8 696e-12
*************************
* Gate Drain capacitance Cdg0
CAP 7 4 15.2e-12
*************************
* Gate Drain Capacitance Cdgj0
* Modelled as a diode
D2 9 4 MDD
.MODEL MDD D IS=1e-32 N=50
+CJO=27.6e-12 VJ=0.817 M=0.871
*************************
.ENDS BUZ906P




  Reply With Quote
Old 22nd June 2006, 01:29 PM   #4
diyAudio Member
 
teodorom's Avatar
 
Join Date: Apr 2004
Location: Milano
Default Thank You !

... however I'm getting crazy in trying to make it work in Cadence ORCad PSPICE. I'm not really an expert of (P)SPICE.
Could you please give me some little help ?
Thank you
__________________
Teodoro
  Reply With Quote
Old 22nd June 2006, 01:34 PM   #5
diyAudio Member
 
Join Date: Sep 2002
Location: Sweden
I don't know that particular version of Spice, but please not that the models are subcircuit models, not standard MOSFET models. I don't know what implications that has in your version of Spice, but if you search the forum there shoudl at least be info on how to use them in LTSpice, which may or may not help you.
  Reply With Quote
Old 22nd June 2006, 03:48 PM   #6
diyAudio Member
 
Ouroboros's Avatar
 
Join Date: Dec 2003
Location: Nottingham UK
Those particular subcircuits are the ones I used with TINA and they compiled and ran perfectly. Be warned that there can be a very large device-to-device variation on BUZ90x devices (see the variation in threshold voltage shown on the data sheet) and these subcircuits don't accurately model this.
  Reply With Quote
Old 22nd June 2006, 04:27 PM   #7
diyAudio Member
 
Join Date: Sep 2002
Location: Sweden
Quote:
Originally posted by Ouroboros
Those particular subcircuits are the ones I used with TINA and they compiled and ran perfectly. Be warned that there can be a very large device-to-device variation on BUZ90x devices (see the variation in threshold voltage shown on the data sheet) and these subcircuits don't accurately model this.
No Spice models can handle device-to-device variations as far as I know. One simply has to use several model of the same device.

More precisely, when using subcircuits, it may be possible to vary some, but not most, parameters if using DC sweep analysis. But that is anyway only useful for Q points and similar.
  Reply With Quote
Old 26th June 2006, 10:35 AM   #8
diyAudio Member
 
teodorom's Avatar
 
Join Date: Apr 2004
Location: Milano
Default Success !

I succeeded in using the models you provided in PSPICE.
Thanks to all !
__________________
Teodoro
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
spice models for led fscarpa58 Parts 18 10th August 2009 10:16 PM
Spice models stinius Solid State 0 18th November 2008 09:07 PM
spice models Zoran Solid State 11 17th September 2005 02:03 PM
Spice Models Bonsai Solid State 4 13th September 2003 04:59 PM
Spice models JoeBob Solid State 18 25th April 2002 02:34 PM


New To Site? Need Help?

All times are GMT. The time now is 09:16 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2