
Home  Forums  Rules  Articles  diyAudio Store  Gallery  Wiki  Blogs  Register  Donations  FAQ  Calendar  Search  Today's Posts  Mark Forums Read  Search 
Software Tools SPICE, PCB CAD, speaker design and measurement software, calculators 

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 
10th January 2008, 07:09 PM  #481 
diyAudio Member
Join Date: Jul 2007
Location: Central Berlin, Germany

LTspice resolution to double precision
Thanks to the yahoo LTspice group, I now found the option needed to get double precision resolution (I knew they would have build that into the s/w):
.option numdgt=15 Now the internal sine source harmonics are down to about 1e13. One then needs a very small time step though (10k...100k points per period), causing sim time and output data amounts to skyrocket... Not that one would need that for any real world circuits, but sometimes it is useful. One might also need to adjust other options to really get that resolution.  Klaus 
5th February 2008, 11:22 PM  #482 
Account disabled at member's request
Join Date: Aug 2005
Location: Toronto

Japanese JFET models
These are some good models that I have used lately for the popular Toshiba JFETs. 2SK389 and 2SJ109 are simply dual 2SK170 and 2SJ74.
K170 and J74 models are set to an Idss of about 12mA while K246 and J103 are set to an Idss of about 6mA. For other Idss values, adjust the model BETA parameter. In a first approximation, BETA=Idss*Vto^2 where Vto is the threshold voltage, already defined in each model. .model J2sk170 NJF(Beta=59.86m Rs=4.151 Rd=4.151 Betatce=.5 Lambda=1.923m + Vto=.5024 Vtotc=2.5m Cgd=20p M=.3805 Pb=.4746 Fc=.5 + Cgs=25.48p Isr=84.77p Nr=2 Is=8.477p N=1 Xti=3 Alpha=10u Vk=100 + Kf=111.3E18 Af=1) .model J2sk246 NJF(Beta=1.07m Rs=56.76 Rd=56.76 Betatce=.5 Lambda=2.8m + Vto=2.638 Vtotc=2.5m Cgd=10.38p M=.4373 Pb=.3905 Fc=.5 + Cgs=6.043p Isr=112.8p Nr=2 Is=11.28p N=1 Xti=3 Alpha=10u Vk=100 + Kf=1E18 Af=1) .model J2sj74 PJF(Beta=92.12m Rs=7.748 Rd=7.748 Betatce=.5 Lambda=4.464m + Vto=.5428 Vtotc=2.5m Cgd=85.67p M=.3246 Pb=.3905 Fc=.5 + Cgs=78.27p Isr=129.8p Nr=2 Is=12.98p N=1 Xti=3 Alpha=10u Vk=100 + Kf=26.64E18 Af=1) .model J2sj103 PJF(Beta=2.197m Rs=76.76 Rd=76.76 Betatce=.5 Lambda=735.3u + Vto=2.037 Vtotc=2.5m Cgd=18.95p M=.5045 Pb=.3905 Fc=.5 + Cgs=17.02p Isr=38.48f Nr=2 Is=3.848f N=1 Xti=3 Alpha=10u Vk=100 + Kf=1E18 Af=1) 
6th February 2008, 01:14 AM  #483 
diyAudio Member
Join Date: Oct 2004

Hi Syn08,
AFAIK, VTO is proportional to Idss. Thus, if you want to have a specific Idss value for your JFETs, you need to scale VTO aswell as BETA. Sigurd 
6th February 2008, 01:21 AM  #484  
diyAudio Member
Join Date: Jan 2006
Location: New Jersey

Re: Japanese JFET models
Quote:
__________________
"We are all agreed that your theory is crazy. The question which divides us is whether it is crazy enough to have a chance of being correct. " Niels Bohr 

6th February 2008, 01:40 AM  #485  
Account disabled at member's request
Join Date: Aug 2005
Location: Toronto

Quote:
Id=Beta*(VgVto)^2 and Id=Idss*(1(Vg/Vto)^2) You do the math... 

6th February 2008, 07:50 AM  #486  
diyAudio Member
Join Date: Oct 2004

I did the math, and using your formulas:
Idss*(1(Vg/Vto)^2) = Beta*(VgVto)^2 => Idss = Beta*(VgVto)^2 / (1(Vg/Vto)^2) and  at Vg = 0  that Idss = Beta * Vto^2 Looking in the datasheet, I read that Idss is dependant on Vto. I copied the relavant part and attached it. Tell me, where am I wrong. Sigurd Quote:


6th February 2008, 10:38 AM  #487  
Account disabled at member's request
Join Date: Aug 2005
Location: Toronto

Quote:
You could also easily check the validity of the above formula using your favorite simulator. Connect the gate to the source and the drain to a DC source. Do a DC sweep analysis (0...5V) and watch the drain current saturate. The Id saturation value is Idss. Then modify Beta and see how Idss follows the above formula (Vto is defined in the model). 

6th February 2008, 01:17 PM  #488 
diyAudio Member
Join Date: Oct 2004

Syn08,
maybe we are talking about different hings here. I am talking about how to create JFET models that approximately correlate to the JFET's datasheet. You are of course correct that if you vary Beta, Idss will change. That is as Idss = Beta * Vto^2 (at VGS = 0), but you can also vary Vto to get the same Idss value! The formula Idss = Beta * Vto^2 is only valid for UGS = 0. When UGS != 0, you will have to use the formula Idss = Beta*(VgVto)^2 / (1(Vg/Vto)^2) You say that Vto is in the model, that it correct. But how do you get that value? In SPICE you can get whatever Idss value you want just by changing Vto. No need to fiddle with Beta. But that will not give you real world JFETs. I get Vto by looking in the datasheet, in the figure I attached in my previous post, by looking at what Idss my model shall have at VGS= and and VDS = 10V, and then I get the Vto for that JFET from that figure. That Vto is then used in the model. I then adjust both Beta and Lambda so that SPICE shows me the IDss value I wanted at VGS=0 and VDS = 10V. Idss also depends on VDS. That is why the lambda parameter is there in JFET models. There also temparature dependencies in Vto and Beta but I do not use that dependencie. Sigurd 
6th February 2008, 02:21 PM  #489  
Account disabled at member's request
Join Date: Aug 2005
Location: Toronto

Quote:
For device physics reasons, the FET IdVgs dependency is, in a first approximation, parabolic. For the particular case of a JFET (it's formally almost the same for depletion MOSFETs or enhancement MOSFETs, to an X axis translation) now imagine that x=Vg and y=Id. By convention, the Vg at which Id=0 (well... almost 0) is defined as Vto. Also by convention, the drain current at Vg=0 is defined as Idss. Please note that these are definitions and they do not, by any means, depend on Vds or Vg or any other variable. This representation leads to an Id dependency to Vg as Id=Idss*(1(Vg/Vt)^2). You may chose another set of parameters, that is for example Beta and Vto. Such a representation tells more to the device physicist because Beta can be conveniently further identified (by writing the device physics equations) as a function of the device geometry and some other parameters (carriers mobilities, etc...). In this representation, Id=Beta*(VgVt)^2 Please note that in the above we discussed two ways to write the same physical dependency of Id(Vg). Id(Vg) should be the same whatever representation you may chose, therefore the two representations should be identical. The only way to make them identical is to chose Beta=Idss*Vto^2 Now, again from a device physics perspective, Id(Vg) is parabolic in at least two simplifying circumstances: a) Vds is very small and b) mobility carrier degradation is neglected. We need more that two (Idss and Vto or Beta and Vto) parameters to model these phenomena. Here comes Lambda and the other parameters in the model files I've posted, but these are by no means impacting the Idss or Beta definitions. The bottom line is that Vto and Idss (or Beta) are independent parameters that you have to extract in order to be able to model a JFET. Idss is something you could directly measure as I've mentioned in my previous post, so it is sometimes preffered by EEs. If you have Idss, then you may calculate Beta to plug into the spice JFET model. Now, for Idss and Vto you have to choose some numerical values. The regular (and simple) approach is to chose Idss and Vto as the average values between the min and max in the datasheet. Another approach is to get the datasheet curves, digitize them, and do a best fit analysis to extract Idss and Vto and perhaps the other parameters (Lambda, etc...). This can be difficult, because you have to chose in advance the model you are fitting against. Depending of the chosen model, the best fitting (usually nonlinear) process could be difficult and definitely could use some sort of computer aided help. Some simulators have the feature to let you enter the digitized curves and spit out the device model. Datasheet curves are "typical" as much as the datasheet parameters have a certain dispersion (min...max). So in fact you are always simulating a "typical" or "average" case and for anything else you need either multiple simulations or the Monte Carlo method. I hope this clears the muddy waters. 

6th February 2008, 03:41 PM  #490  
diyAudio Member
Join Date: Aug 2002
Location: Germany

Re: Japanese JFET models
Quote:
Hi, I have the same models. Your definition, however, is not reflected there, if I'm not completly off anything. For the 2SK170, it is stated BETA= 59.86m, Vto=0.5024, and you said Idss 12mA. When processing BETA=Idss*Vto^2 I get BETA=12*(0.5024^2) BETA=12*0.2524=3.028m Or, vice versa, if BETA is correct, you'd get an Idss of 237mA. Gosh! I hope I don't misinterprete the mathematical chars... The relation of the modeled values are close to BETA=Idss*(Vto*10), however... Rüdiger
__________________
"I can feel what's going on inside a piece of electronic equipment. I have a sense that I know what's going on inside the transistors." Robert Moog 

Thread Tools  Search this Thread 


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Need help with Spice simulation  overmind  Everything Else  4  23rd December 2002 05:58 PM 
New To Site?  Need Help? 