
Home  Forums  Rules  Articles  diyAudio Store  Gallery  Wiki  Blogs  Register  Donations  FAQ  Calendar  Search  Today's Posts  Mark Forums Read  Search 
Pass Labs This forum is dedicated to Pass Labs discussion. 

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 

Thread Tools  Search this Thread 
18th January 2002, 10:15 AM  #1 
diyAudio Member
Join Date: Jan 2002
Location: Belgium

2sk170 and 389 spice models
Does anyone have an official or homebrew
Spice model for the 2sk170, sj74, and sk389 FETs? Have been searching the net for ages, to no avail. Thanks, W 
18th January 2002, 10:25 AM  #2 
diyAudio Member
Join Date: Apr 2001
Location: Limoges, France

2SK389
Hi,
I've only got 3 models for 2SK389. Just make a little spice circuit to make a curve tracer, and see which one is the closest to mf's datasheet. Enjoy : .model J2sk389 NJF(Beta=51.76m Rs=8.008 Rd=8.008 Betatce=.5 Lambda=11.22m + Vto=.5275 Vtotc=2.5m Cgd=18.28p M=.3367 Pb=.3905 Fc=.5 + Cgs=20.07p Isr=112.8p Nr=2 Is=11.28p N=1 Xti=3 Alpha=10u Vk=100 + Kf=92.85E18 Af=1) *SRC=2SK389BL;QSK389BL;JFETs N;Gen. Purpose;25V 20mA .MODEL QSK389BL NJF (VTO=2.5 BETA=6M LAMBDA=1.2M RD=4.95 + RS=4.45 IS=6.32F PB=1 FC=.5 CGS=71.2P CGD=18.9P) * 25 Volt 20M Amp 35.3 ohm DepMode NChannel JFET 07281995 * 2SK389BL, TOSHIBA, 1986 D.A.T.A.BOOK, TRANSISTOR EDITION, P.227, LINE 75 *SRC=2SK389;QSK389;JFETs N;Gen. Purpose;50V 10mA .MODEL QSK389 NJF (VTO=2 BETA=20M LAMBDA=600U RD=7 + RS=6.3 IS=1.58F PB=1 FC=.5 CGS=19.5P CGD=5.5P) * 50 Volt 10M Amp 50 ohm DepMode NChannel JFET 07281995 * 2SK389, TOSHIBA, 1993 JAPANESE FET MANUAL, P.46 I would be too interested in other models, if available
__________________
François "Learning French is trivial: the word for horse is cheval, and everything else follows in the same way." 
18th January 2002, 12:54 PM  #3 
diyAudio Member
Join Date: Oct 2001
Location: Bavaria, Germany

A working model for the 2sk170 (basically one half of 2sk389) is available together with the
commercial simulation software HSPICE from Avant!. Unfortunately I cannot post it here because it is proprietary information. But if you have a chance to get your hands on a HSPICE installation you will find it in the library directory. The device is made by Toshiba. But they do not have a spice model for it on the web page. Maik 
18th January 2002, 01:31 PM  #4 
diyAudio Member
Join Date: Apr 2001
Location: Limoges, France

Oups, forgot to say that the model is actually one half of the 389, so you've got to use two of them to get the complete device.
I get the models from usenet, but if there is any copyright infringement, let me now, I'll delete the post... And... If someone has the spice model for 2SJ109, can it be shared ?
__________________
François "Learning French is trivial: the word for horse is cheval, and everything else follows in the same way." 
20th January 2002, 12:59 AM  #5 
diyAudio Member
Join Date: Jan 2002
Location: France

Here is a spice model for: 2SK170
MODEL 2sk170 NJF + VTO=5.211e001 BETA=3.683e002 LAMBDA=4.829e003 + IS=1.000e009, RD=0.000e+000 RS=0.000e+000 + CGS=5.647e011 CGD=2.562e011 + PB=4.860e+000 FC=0.5 Maybe it will help u. flyingfader
__________________
"Any instrument when dropped will roll into the least accessible corner." 
21st January 2002, 10:01 AM  #6 
diyAudio Member
Join Date: Jan 2002
Location: Belgium

Thanks a lot!
W 
2nd October 2011, 06:36 PM  #7 
diyAudio Member RIP
Join Date: May 2005
Location: Canoga Park, California

There are some models floating around out there that seem to have a very small lambda, and can be extremely misleading. The models also make a very abrupt transition from the socalled triode region to the pinchoff region, and comparison to characteristic curves on the Toshiba datasheet show marked discrepancies.
Another difficulty with parameter measurements is the signalinduced selfheating of the parts. One can deal with this using lowdutyfactor pulsed measurements, or a strategy that I'm exploring where data sets for a given temperature are acquired when the device has come to ~equilibrium, and sets are recorded keeping the sample isodissipational. This still takes time, but not as long as changing voltages/currents and waiting each time for stabilization. Brad 
2nd October 2011, 07:11 PM  #8 
The one and only

I have relied on the models posted on Bob Cordell's site.

2nd October 2011, 07:39 PM  #9 
diyAudio Member RIP
Join Date: May 2005
Location: Canoga Park, California

Thanks Nelson! I guess I've never visited Cordelland  I'll seek it out.
I did just create another model borrowing from the post above, and it still predicts a waylow output conductance (about 38uS) compared to a linear fit to the Toshiba datasheet curves for Vgs = 0 (closer to 94uS). But it gets closer at least. I have enough parts that I could even get some decent statistics. Of course they would apply to that particular run/date code. When Harman was shutting down a project (the rule there rather than the exception!) they were allowing people to take away some of the obsolete inventory, and I got a whole bunch of 2SK364BL, which is the same chip as the 170 but characterized for analog switching. Brad 
2nd October 2011, 07:50 PM  #10 
diyAudio Member RIP
Join Date: May 2005
Location: Canoga Park, California

PS: found the site, found the models, but only see now 2 parts for JFETs: both Linear Integrated Systems ones, the LS844 and the LSK389C. Had there been an SK170 before (I know the 389 sections are close but not afaik identical)?

Thread Tools  Search this Thread 


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
spice models for led  fscarpa58  Software Tools  18  10th August 2009 10:16 PM 
Spice models  stinius  Solid State  0  18th November 2008 09:07 PM 
Spice models  Grahamm  Tubes / Valves  7  19th December 2006 01:36 PM 
Spice Models  Bonsai  Solid State  5  24th September 2003 09:44 AM 
Spice models  JoeBob  Solid State  18  25th April 2002 02:34 PM 
New To Site?  Need Help? 