Spice: how to set IDSS etc? - 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 5th August 2005, 08:37 PM   #1
expert in tautology
diyAudio Member
 
bear's Avatar
 
Join Date: Apr 2002
Location: New York State USA
Default Spice: how to set IDSS etc?

Being slow to the dance, I just downloaded Linear Tech's SwcadIII and have been playing about with it...

Among the many things that are not mentioned or clear with or without the help file is how does one go about "setting" the IDSS for a JFET, or similarly Vgs for a Mosfet.

I see a great number of parameters for a given JFET, but none seems to directly correspond to IDSS (for example) - or else they're calling it something else.

Yes, I understand about chosing specific devices from the available devices, and/or the possibility of adding in devices (from someplace or another...), but for simplicity at this point I'd just as soon massage these two parameters for existing models for the sake of just making given circuits work according to what a pen and paper design says that they ought to.

Any input, or citations for sites that can provide this sort of info, would be appreciated.

_-_-bear
__________________
_-_-bear
http://www.bearlabs.com -- Btw, I don't actually know anything, FYI -- [...2SJ74 Toshiba bogus asian parts - beware! ]
  Reply With Quote
Old 5th August 2005, 08:47 PM   #2
Mr Evil is offline Mr Evil  United Kingdom
diyAudio Member
 
Join Date: Aug 2004
Location: Behind you
For JFETs you want to change vt0, which is the turn-off gate-source voltage. Also of use is beta, which is the transconductance. Both of those will change Idss.
__________________
https://mrevil.asvachin.eu/
  Reply With Quote
Old 6th August 2005, 01:59 PM   #3
expert in tautology
diyAudio Member
 
bear's Avatar
 
Join Date: Apr 2002
Location: New York State USA
Ok, now all we need is a formula that relates the Beta & Vto to IDSS! Or a citation where I can find this info myself...

This is an example of two of the "standard" JFET models:

.model 2N3819 NJF(Beta=1.304m Betatce=-.5 Rd=1 Rs=1 Lambda=2.25m Vto=-3 Vtotc=-2.5m Is=33.57f Isr=322.4f N=1 Nr=2 Xti=3 Alpha=311

.model 2N4338 NJF(Beta=781u Betatce=-.5 Rd=1 Rs=1 Lambda=1.167m Vto=-.6606 Vtotc=-2.5m Is=114.5f Isr=1.091p N=1 Nr=2 Xti=3 Alpha=506.8u Vk=251.7 Cgd=2.8p M=.2271 Pb=.5 Fc=.5 Cgs=2.916p Kf=2.918E-18 Af=1 mfg=Fairchild)

_-_-bear
__________________
_-_-bear
http://www.bearlabs.com -- Btw, I don't actually know anything, FYI -- [...2SJ74 Toshiba bogus asian parts - beware! ]
  Reply With Quote
Old 6th August 2005, 03:40 PM   #4
andy_c is offline andy_c  United States
Banned
 
Join Date: Apr 2003
Hi bear,

From Massobrio and Antognetti, here is the equation in SPICE form for the JFET drain current in the saturated region (not analogous to BJT saturation):

ID=beta*(VGS-VTO)2*(1+lambda*VDS)

from which you can calculate IDSS.
  Reply With Quote
Old 6th August 2005, 04:28 PM   #5
diyAudio Member
 
Join Date: Mar 2003
Location: Willmar, Minnesota
Hi,
If you're using LTspice you should also join the LTspice forum on yahoogroups.com [very active and helpful!!!] Look through the archives your question has probably been answered at least a dozen times.

Good Luck!
-=Randy
  Reply With Quote
Old 6th August 2005, 06:50 PM   #6
expert in tautology
diyAudio Member
 
bear's Avatar
 
Join Date: Apr 2002
Location: New York State USA
Gosh, I really don't like Yahoo's groups... but I will join anyhow.

Here's a really odd FFT result from LT's spice... the source is simply the internal virtual AC generator with a 100k load! I'm baffled as to why it should show any harmonics whatsover??

One is a 2000Hz source, the other is a 2200 Hz. source, the 1kHz source looks far worse!

_-_-bear
Attached Images
File Type: jpg ltswcad-fft1.jpg (88.4 KB, 153 views)
__________________
_-_-bear
http://www.bearlabs.com -- Btw, I don't actually know anything, FYI -- [...2SJ74 Toshiba bogus asian parts - beware! ]
  Reply With Quote
Old 8th August 2005, 02:15 AM   #7
SkyChu is offline SkyChu  Taiwan
diyAudio Member
 
Join Date: May 2002
Location: Taiwan
Have you turned off compression ( Tools>Control Panel>Compression ) ?
__________________
Sky Chu
  Reply With Quote
Old 8th August 2005, 03:01 AM   #8
heater is offline heater  Finland
diyAudio Member
 
Join Date: Jul 2004
Location: Helsinki
I have been fighting with the FFT problem as well recently. Seemed every schematic had different harmonics on it's sine wave generators and is very sensitive to stop time and maximum time step (in the edit simulation command dialog box).

Now turning off compression, using a stop time of 100ms and a time step of 0.5uS I can get a plain generator with those spikes down 140db.

Trouble is this puts up the time it takes for simulation to complete which on my old 266MHz machine can be considerable.

Cheers for the tip.
__________________
For me the past is not over yet.
  Reply With Quote
Old 8th August 2005, 03:26 AM   #9
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
LtSpice default compression of analysis data is inconvenient, remembering to disable it in the control panel menu every time you restart the program isn't reliable (for me anyway)

I add (or copy to actually) a spice directive line to all of my schematics:

.param plotwinsize=0
  Reply With Quote
Old 8th August 2005, 04:09 AM   #10
Tom2 is offline Tom2  United States
diyAudio Member
 
Join Date: Jun 2004
Location: Central CA
Quote:
jcx said
I add (or copy to actually) a spice directive line to all of my schematics:
.param plotwinsize=0
jcx,

I think it should be

.options plotwinsize=0


Also the .raw and .fft files associated with the schematic can be large. Usually after playing around with the schematic, I delete them to free up hard drive space and I leave the original .asc file.

tom
  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
High Idss jFETs AndrewT Parts 24 30th October 2008 03:50 PM
FS: Idss matched K170 bbp Swap Meet 1 26th August 2007 08:25 PM
Free Spice Or Cheap Spice Simulator-Where To Start? kelticwizard Everything Else 29 15th February 2007 02:38 AM
Ono - 2SK170, Which Idss? transducer Pass Labs 11 25th March 2003 11:29 PM
P-spice THD JensRasmussen Solid State 10 18th October 2002 06:18 AM


New To Site? Need Help?

All times are GMT. The time now is 01:35 PM.


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