LD1014 SPiCE models - diyAudio
Go Back   Home > Forums > Amplifiers > Pass Labs
Home Forums Rules Articles diyAudio Store Gallery Wiki Blogs Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

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
Old 18th December 2005, 06:28 PM   #1
diyAudio Member
Join Date: Dec 2005
Location: Palermo
Default LD1014 SPiCE models

I'm searching for a S.P.I.C.E model for the lovoltech LD1014 (even if any of the Lovoltech JFET will do just fine).
I saw a previous post but the guy received uncorrelated answers.
What's all this secret about those models?
I've come out with one that fits IV curves nicely, but there's some work to do on the transient response.
Please, if you have any infos, I 'd really like to have a look to it.
  Reply With Quote
Old 18th December 2005, 07:17 PM   #2
Tom2 is offline Tom2  United States
diyAudio Member
Join Date: Jun 2004
Location: Central CA
Here is my try.
It sort of works.

Attached Images
File Type: gif jfetpower1.gif (8.9 KB, 997 views)
  Reply With Quote
Old 19th December 2005, 09:10 AM   #3
diyAudio Member
Join Date: Dec 2005
Location: Palermo
Are you using LTC?
Why did you indipendently modelled those gate, drain, capacitances with external capacitors?
There are two drawbacks to this approch, but I may be wrong.
First, they are partly voltage controlled capacitors. You can include then in the model, and SPICE will take care of those himself.

Second I believe we both made the same error: LTC (if you are using it of course)uses in the fet model zero-voltage Capatacitance values , while those in the Lovoltech datasheet are not.
I have to see better this.
Here there's my model. I suppose beta and lambda are less accurate than yours. Capacitances again, may be wrong as they are not zero-voltage capacitances.

.MODEL LU1014D NJF (VTO=-1.8 BETA=29000M LAMBDA=0.18 RD=0.0065 CGD=363P CGS=784P VTOTC=-2.6M)
  Reply With Quote
Old 20th December 2005, 10:08 AM   #4
Tom2 is offline Tom2  United States
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Yes I am using LTspice.

It seems the value of lambda I used is high.
I simulate a fet curve tracer with LTspice and try to
fit the model to the curves in figure 8 of the LU1014D
data sheet. I try different values of vto, lamda and beta
to get the curves, then I try the fet model in zen v8 circuit and see
what the currents and gain are. I am really just guessing and tweaking
the fet values. Here is some new fet parameters that might work.
(Vto=-1.8, beta=2 lambda=.7) and change R5 to 22k

The junction capacitances were read off the data sheet. The values are
the 10V vds (-5v vgs) values. Yes you are correct the large signal
fet model does change the cap values with voltage. I put them in there
since the fet is used as a cascode and the junction
voltage changes seem small. Also the default spice
capacitances are zero. I looked up the Shichman and Hodges
model on the web and putting the caps in the circuit seemed ok
to me. I could be wrong.

I think the fet spice models are inadequite to model the power fets.
For example in figure 8 of the data sheet, the vgs=-1v curve has
some curvature to it. I don't think the fet model in the pinch off
region can show curvature(or is it the linear region?).
Using lambda fakes it, since it is similar to an Early voltage.

I am looking through some books I have to find a more basic device
model for fets. It might yield better Id vs Vds (Vgs constant) curves.

  Reply With Quote
Old 20th December 2005, 04:02 PM   #5
diyAudio Member
Join Date: Dec 2005
Location: Palermo
I agree with you, and I also feel the models are inadeguate to model that strange upwards curve we need.
I see that Lovoltech provides S.P.I.C.E models, so we are to wonder if:
-They fake that upwards curve in the way/in a similar way you are doing.
-They provide a macrocircuit that has that curve, thus bypassing the need for a suitable fet model.
-They just don't care, as their product is intended for switching applications and they don't care a lot about the shape of the IV characteristics.
About the capacitances, I also believe the changes would be little, I didn't think we were cascoding.
Why don't you put a current source instead of the resistor?
It surely helped me with supply requirements, but wreaked havoc with the noise.
I can't wait to get a grip on the real jfet and make some real mesurements.
  Reply With Quote
Old 9th March 2006, 08:29 PM   #6
diyAudio Member
Join Date: Oct 2004
Hi, I've tried to model the LU1014D power JFET for a couple of evenings now and I haven't come up with something useful. So I did a search on google and found this:


Reading the abstract made me glad but as always, the more you read.....

To use the model described in the paper above I need a lot of information from Lovoltech since the input parameters for the model is on process level. And even if I get the parameters I'm not sure that it would be possible to use the model in a Spice simulator.

So, if anyone in this forum have a lot of experience in modelling, please take a look at the paper and tell me if it could be useful.

Does it exist a working Spice model for the LU1014D power JFET that I could get hold off?

Copied from Lovoltech application note:
"Spice models and high level circuit simulation models can be provided to customers for circuit and system simulation"

  Reply With Quote
Old 9th March 2006, 10:04 PM   #7
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
using an existing standard JFET model does not work because all this models are based on a quadratic equation in the form:
Id = Ids(1-Ugs/Up)^2
with such an equation it is not possible to model the exponential triode like curve we want to have.

Finding a model should go the following way:
- take a LU1014 and measure it (Lovoltech data is not good enough)
- find a general 3d equation like
Ids=a + b*Vds +c*Vgs + d*Vds*Vgs + e*Vds^2 ....
or something else
- put this in MATLAB and make an variation of the constants a,b...
- put the result in SPICE and thats it

a nice site for this is (for tubes):

BTW: I wanted to do this, but I have no LU1014
  Reply With Quote
Old 10th March 2006, 02:14 AM   #8
Tom2 is offline Tom2  United States
diyAudio Member
Join Date: Jun 2004
Location: Central CA
Try using Mesfet models.

Here is my try using a TOM3 mesfet model.
The curves are Vgs=0v, -.5v and -1v.

Attached Images
File Type: png curvetrace.png (7.2 KB, 634 views)
  Reply With Quote
Old 10th March 2006, 06:15 AM   #9
diyAudio Member
Join Date: Oct 2004

kekso22: your idea is good but I have the same problem as you, nothing to measure on. The proposal in the article is to go with the equation below, describing the drain current:

Ijfet= io∑[1+tanh{P1(Vgs-Vp)}] ∑tanh(ŠVds) ∑e ^ŽVds

Tom2: the mesfet model you are using is this something already implemented in LTC or is this your own "tweaked" model?

  Reply With Quote
Old 10th March 2006, 08:02 AM   #10
diyAudio Member
Join Date: Dec 2005
Location: Palermo
I've been thinking about this, and I believe that our best bet is to run those datasheets into a parameter model extractor such as MODPEX or similar.
That would give us probably an usable model with no hassle.
Actually I'm not sure It would model properly the region of interest.

Unfortunately I was no able to find such a program, and especially nor a free one, even if I recall that Spice-Opus has some limited parameter extraction capabilities.
Anyone with similar programs around?
Myself I'm going to try something with something I have handy.
  Reply With Quote


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 Software Tools 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 01:14 AM.

vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2017 DragonByte Technologies Ltd.
Copyright ©1999-2017 diyAudio

Content Relevant URLs by vBSEO 3.3.2