LD1014 SPiCE models - Page 2 - diyAudio
Go Back   Home > Forums > Amplifiers > Pass Labs

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
Reply
 
Thread Tools Search this Thread
Old 10th March 2006, 08:46 PM   #11
kekso22 is offline kekso22  Germany
diyAudio Member
 
kekso22's Avatar
 
Join Date: Feb 2005
Location: Bavaria
Send a message via AIM to kekso22 Send a message via MSN to kekso22 Send a message via Yahoo to kekso22
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
  Reply With Quote
Old 10th March 2006, 09:28 PM   #12
kekso22 is offline kekso22  Germany
diyAudio Member
 
kekso22's Avatar
 
Join Date: Feb 2005
Location: Bavaria
Send a message via AIM to kekso22 Send a message via MSN to kekso22 Send a message via Yahoo to kekso22
Hi,

a very good description of all the MESFET models can be found in:
http://www.ct.tkk.fi/publications/dt-antti/thesis.pdf

_____________________
let's work now
  Reply With Quote
Old 10th March 2006, 10:50 PM   #13
kekso22 is offline kekso22  Germany
diyAudio Member
 
kekso22's Avatar
 
Join Date: Feb 2005
Location: Bavaria
Send a message via AIM to kekso22 Send a message via MSN to kekso22 Send a message via Yahoo to kekso22
My first results:

I took some values from the LU1014 datasheet and placed this in Tablecurve3D with the model from "Materka-Kacprzak". From the result I made my first LTC-Spice 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))*(1-V(2,3)/
+ (c+d*V(1,3)))**(g+h*V(2,3))*TANH((e*V(1,3))/
+ (a*(1-f*V(2,3))))}
.ENDS LU1014

Ids curves are from Vgs 0v to -2V
Attached Images
File Type: jpg ltc_1014.jpg (80.6 KB, 430 views)
  Reply With Quote
Old 11th March 2006, 09:05 AM   #14
Tom2 is offline Tom2  United States
diyAudio Member
 
Join Date: Jun 2004
Location: Central CA
Quote:
builderandy said:
Tom2: the mesfet model you are using is this something already implemented in LTC or is this your own "tweaked" model?
It's a simplified model I made for LTspice.
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
Attached Images
File Type: png tom3.png (15.1 KB, 430 views)
  Reply With Quote
Old 11th March 2006, 08:51 PM   #15
Tom2 is offline Tom2  United States
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
  Reply With Quote
Old 11th March 2006, 11:04 PM   #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
Attached Images
File Type: jpg idvsvgs.jpg (77.8 KB, 372 views)
  Reply With Quote
Old 12th March 2006, 03:24 AM   #17
Tom2 is offline Tom2  United States
diyAudio Member
 
Join Date: Jun 2004
Location: Central CA
Quote:
builderrandy said:
Do you see the same in your simulations.
This output is
Id vs Vgs with constant Vds.
Vds = 2,4,6,8,10 volts from right to left.

Tom
Attached Images
File Type: png vgsvsidvdsconstant.png (8.3 KB, 342 views)
  Reply With Quote
Old 12th March 2006, 03:40 AM   #18
Tom2 is offline Tom2  United States
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
Attached Files
File Type: zip tom3fetmodel.zip (2.4 KB, 78 views)
  Reply With Quote
Old 12th March 2006, 05:37 PM   #19
kekso22 is offline kekso22  Germany
diyAudio Member
 
kekso22's Avatar
 
Join Date: Feb 2005
Location: Bavaria
Send a message via AIM to kekso22 Send a message via MSN to kekso22 Send a message via Yahoo to kekso22
Quote:
Originally posted by builderandy
Nice work kekso22, could you comment on the above observations, how is your model working?
Hi Andy,

The "Materka-Kacprzak" 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
  Reply With Quote
Old 12th March 2006, 06:04 PM   #20
kekso22 is offline kekso22  Germany
diyAudio Member
 
kekso22's Avatar
 
Join Date: Feb 2005
Location: Bavaria
Send a message via AIM to kekso22 Send a message via MSN to kekso22 Send a message via Yahoo to kekso22
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 "Materka-Kacprzak" 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:
Attached Files
File Type: zip lu1014.zip (1.8 KB, 80 views)
  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
new spice models available Joel Tubes / Valves 32 10th July 2013 05:30 PM
spice models for led fscarpa58 Parts 18 10th August 2009 10:16 PM
Spice Models Bonsai Solid State 5 24th September 2003 09:44 AM
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 04:05 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