
Home  Forums  Rules  Articles  diyAudio Store  Blogs  Gallery  Wiki  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 
10th March 2006, 09:46 PM  #11 
diyAudio Member

Hi,
I just found an interesting program which could help us! TABLECURVE 3D @ http://www.systat.com/ It is free (30 days trial), has a lot of predefined equations and we can define our own ones. Bye 
10th March 2006, 10:28 PM  #12 
diyAudio Member

Hi,
a very good description of all the MESFET models can be found in: http://www.ct.tkk.fi/publications/dtantti/thesis.pdf _____________________ let's work now 
10th March 2006, 11:50 PM  #13 
diyAudio Member

My first results:
I took some values from the LU1014 datasheet and placed this in Tablecurve3D with the model from "MaterkaKacprzak". From the result I made my first LTCSpice model: .SUBCKT LU1014 1 2 3 ; D G S + PARAMS: a=21.7924 b=4.5599 c=10.2887 d=9.1318 e=61.579 + f=0.5726 g=16.0443 h=71.8659 G1 1 3 Value={(a+b*V(1,3))*(1V(2,3)/ + (c+d*V(1,3)))**(g+h*V(2,3))*TANH((e*V(1,3))/ + (a*(1f*V(2,3))))} .ENDS LU1014 Ids curves are from Vgs 0v to 2V 
11th March 2006, 10:05 AM  #14  
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Quote:
The model is far from perfect. It does not contain any capacitances, but they could be added. I usually change the diodes to power diodes that LTspice has. The model can have convergence problems when using it. I added the uramp functions, that helps a little. I find checking the noopiter box under the default dc solve strategy under the spice control panel helps convergence but not always. I spent alot of time playing with the parameters to get the curves. I can post the .asc and .asy files I created if you are interested. I just Googled and found the different models online. I tried some of simple models and found they did not show the triode region. I found the TOM3 model and it seemed to work. I also saw the mathematical methods and tools on the web to derive the equations. I found the Agilent web site and the spice manual of their product to be very useful. I'll post a link to it. The main insight I got running this model was the "triodeness" of these devices. Plate resistance for example, really plays into the gain of certain circuits. I've received devices from Grey and have started playing around with them in the 5mA range just to build simple circuits and measured results show the triode character is very evident. Hopefully soon I will get some simple circuits into a audio system and hear what these devices really sound like. Also I want to hear how much 1/f noise they have. Tom 

11th March 2006, 09:51 PM  #15 
diyAudio Member
Join Date: Jun 2004
Location: Central CA

I can't find the Agilent reference.
Kelso22's reference to the thesis.pdf contains the equations for the TOM3 model on page 32. Tom 
12th March 2006, 12:04 AM  #16 
diyAudio Member
Join Date: Oct 2004

Hi Tom2, copied the model and parameters you attached. The Id_vs_Vds curves are approximately the same as yours and the datablade for LU1014D, but when I simulate Id_vs_Vgs the drain current isn't zero until the "Gate threshold voltage" is reached, see attached picture. Do you see the same in your simulations.
Nice work kekso22, could you comment on the above observations, how is your model working? /Andy 
12th March 2006, 04:24 AM  #17  
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Quote:
Id vs Vgs with constant Vds. Vds = 2,4,6,8,10 volts from right to left. Tom 

12th March 2006, 04:40 AM  #18 
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Here are the working .asc and .asy files I made and use.
I have made the diodes MUR460's. LTspice has the models. Put the tom3fet2.asc and tom3fet2.asy file in the same working directory as the .asc schematic files using the tom3fet2 model. I have included a Vgs_Id.asc file and a curve trace file curvetrace.asc file. Fet parameters can be changed on the tom3fet2.asc file or on the working .asc schematic file. Remember my previous post on convergence problems that can happen using my model. Have fun. Tom 
12th March 2006, 06:37 PM  #19  
diyAudio Member

Quote:
The "MaterkaKacprzak" or the "TOM3" models are working both. It strongly depends on the constants you choose. In the meantime I also tried the TOM3 and I find it a little better. The Fitting is more precise. Emil 

12th March 2006, 07:04 PM  #20 
diyAudio Member

Hi Tom,
nice work! I have put the "TOM3" equations in TABLECURVE3D with some datapoints from the datasheet. The fitting goes very well with this model (better than with the "MaterkaKacprzak" model) and I changed your constants in the asc file. I also included capacitors, which I took from the datasheet @ Vds=2.5V and a gate resistor to stabilize some simulation. I find, that the uramp is not necessary for every equation (if the constants are correct!). Only for Vds<0 then Ids should be zero. Don't understand me wrong, yours and mine is not a model we can use, it should only show, that it can be done in such a way. I'm waiting for real data, but I have no LU1014. Maybe anybody owning a LU1014 can send us real measured data. Bye Emil PS: example with "TOM3" follows: 
Thread Tools  Search this Thread 


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
new spice models available  Joel  Tubes / Valves  32  10th July 2013 06:30 PM 
spice models for led  fscarpa58  Software Tools  18  10th August 2009 11:16 PM 
Spice Models  Bonsai  Solid State  5  24th September 2003 10:44 AM 
Spice Models  Bonsai  Solid State  4  13th September 2003 05:59 PM 
Spice models  JoeBob  Solid State  18  25th April 2002 03:34 PM 
New To Site?  Need Help? 