
Home  Forums  Rules  Articles  diyAudio Store  Gallery  Wiki  Blogs  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 
18th December 2005, 07:28 PM  #1 
diyAudio Member
Join Date: Dec 2005
Location: Palermo

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. 
18th December 2005, 08:17 PM  #2 
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Here is my try.
It sort of works. Tom 
19th December 2005, 10:10 AM  #3 
diyAudio Member
Join Date: Dec 2005
Location: Palermo

Good
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 zerovoltage 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 zerovoltage capacitances. .MODEL LU1014D NJF (VTO=1.8 BETA=29000M LAMBDA=0.18 RD=0.0065 CGD=363P CGS=784P VTOTC=2.6M) Thanks 
20th December 2005, 11:08 AM  #4 
diyAudio Member
Join Date: Jun 2004
Location: Central CA

Giusedia,
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. Tom 
20th December 2005, 05:02 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. 
9th March 2006, 09:29 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:
http://mixedsignal.eleg.uark.edu/sic...OMPEL_JFET.pdf 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" /Andy 
9th March 2006, 11:04 PM  #7 
diyAudio Member

Hi,
using an existing standard JFET model does not work because all this models are based on a quadratic equation in the form: Id = Ids(1Ugs/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): http://www.normankoren.com/Audio/ BTW: I wanted to do this, but I have no LU1014 
10th March 2006, 03:14 AM  #8 
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. Tom 
10th March 2006, 07:15 AM  #9 
diyAudio Member
Join Date: Oct 2004

Hi,
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(VgsVp)}] ·tanh(áVds) ·e ^ëVds Tom2: the mesfet model you are using is this something already implemented in LTC or is this your own "tweaked" model? /Andy 
10th March 2006, 09:02 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 SpiceOpus has some limited parameter extraction capabilities. Anyone with similar programs around? Myself I'm going to try something with something I have handy. Bye 
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? 