Evaluation results: MJL3281A/MJL1302A SPICE Models - diyAudio
Go Back   Home > Forums > Amplifiers > Solid State

Solid State Talk all about solid state amplification.

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 19th September 2003, 04:41 AM   #1
andy_c is offline andy_c  United States
Banned
 
Join Date: Apr 2003
Default Evaluation results: MJL3281A/MJL1302A SPICE Models

Well, I finally got done with a preliminary evaluation of several SPICE models for the MJL3281A and MJL1302A to compare their simulated performance, mainly of ft vs collector current, with the data sheet values. This all started a while back when I was looking at the simulated performance of a power amplifier with a capacitive load of 2 uF in parallel with 8 Ohms using these devices for the output stage. I was trying to see if I could get the thing stable for this load with no output inductor. It turned out that the simulated open-loop output inductance of the amp was so large that a major resonance occurred at about 100 kHz, preventing stability from being achieved with any reasonable unity loop gain frequency with the capacitive load. In a previous thread involving Fred and myself (which I can't seem to locate at the moment), it became apparent that the models he was using with his simulator and the models I was using, provided by On Semiconductor, were quite different. We got very different results for the output inductance using the same test circuit.

This subject came up again in the thread about the amp in the Randy Slone book. But seeing that Randy Slone thread title keep coming up again and again made me feel like giving Randy a break - and the discussion of models really didn't have anything to do with the original thread topic anyway. So I thought I'd post the results of my evaluation in a new thread specifically about the SPICE models for these devices. My main purpose is to end up with a modified model whose simulated output inductance will be as close as possible to that of the real devices, assuming the real devices match up with the data sheet. Actually, I'd like as many of the parameters to match up as closely as possible with reality, but I'm starting with ft vs frequency. The desire to compare simulated and data sheet ft values came from the following site: http://www.reed-electronics.com/ednm...2596/09df3.htm. There they have an expression for the output inductance of an emitter follower as follows:

Lout = R / (2 * pi * ft)

where R is the internal plus external base resistance. This clearly shows the need for accurate ft in the model to get accurate output inductance. I'll also look at the internal base resistance, but that will be the topic of another post to this thread. I have three models for each of the NPN and PNP devices: the On Semiconductor models, the PSpice models for the Toshiba 2SC3281 and 2SA1302, and the models Fred posted in the thread I referred to earlier. I'm not sure if Fred's models were for the Toshiba or On Semiconductor devices though.

The simulation test circuits for ft are similar to those shown in http://www.diyaudio.com/forums/showt...089#post235089, except that I put the DC supply in the base instead of the emitter (to keep a constant Vce) and set the collector supply to 10Vdc to match the value used in the ft vs Ic plots in the data sheets. I temporarily placed a current source in the emitter to set the currents to the desired values, then determined Vbe. Then I used these Vbe values to set the currents when doing the actual ft simulation. The result is a spreadsheet with two plots and the raw data. So without further ado, here is a plot for ft vs collector current for the MJL3281A.
Attached Images
File Type: gif mjl3281a.gif (52.4 KB, 1800 views)
  Reply With Quote
Old 19th September 2003, 04:56 AM   #2
Banned
 
Join Date: Feb 2002
Location: As far from the NOSsers as possible
Default This may be straying a bit.....

But some of you guys think that the ON versions are better than the Toshiba ones.

According to a buddy who was in that department when it was Motorola:

The very first ones that they sold were Toshibas that they bought, without any inking, and the "batwing" logo was put on by Motorola. Reason was that they could not get theirs right.

The ON parts are a second source. Second source implies that it is as close as possible, if not indeed identical, in every way that can be. Otherwise, new parts would have to go through an evaluation process at darn near any company that used lots of them. And that is not what a second source is supposed to be.

Jocko
  Reply With Quote
Old 19th September 2003, 04:56 AM   #3
andy_c is offline andy_c  United States
Banned
 
Join Date: Apr 2003
Default More data

...and below is a plot for ft vs Ic of the MJL1302A. Clearly, the models for the MJL3281A are all pretty far off from reality, though the new On Semiconductor model for the MJL1302A looks at least reasonable. For small-signal analysis, the ft value for Ic of 100 mA is probably the most important. For the MJL3281A at 100 mA, the On Semiconductor model is more than a factor of six low for ft. So this says if the model can be tweaked to get this right, my previous estimates of power amp performance with a capacitive load will have been shown to be very pessimistic. This weekend I'm going to play around with the parameters of the On Semiconductor models in an attempt to get the plots to match up with the data sheets as closely as possible. I'll keep y'all posted on what happens. I'm going to try to fix the DC parameters first, then go for ft vs current. I'll also have a look at the internal base resistance if time allows.
Attached Images
File Type: gif mjl1302a.gif (41.1 KB, 1712 views)
  Reply With Quote
Old 19th September 2003, 04:59 AM   #4
andy_c is offline andy_c  United States
Banned
 
Join Date: Apr 2003
Jocko,

Just to clarify, the curves marked as "data sheet" are from the On Semiconductor data sheet. All the other curves are simulated data. I didn't include the Toshiba data sheet info.
  Reply With Quote
Old 19th September 2003, 07:08 AM   #5
diyAudio Member
 
jan.didden's Avatar
 
Join Date: May 2002
Location: Great City of Turnhout, Belgium
Blog Entries: 7
Well, I don't know why all this ON-bashing, but to me the ON- models are way closer to the data sheet then any of the other ones. Since the data sheets are generated by actually characterizing the "average" device that is my reference.

The Pspice models clearly are a joke. Any decent text on semiconductor physics will show at least the general shape as shown by the ON-models.

Jan Didden
  Reply With Quote
Old 19th September 2003, 08:33 AM   #6
Banned
 
Join Date: Feb 2002
Location: As far from the NOSsers as possible
Our resident simulation "expert" (Phred) has told me countless times that the PSpice models are dreck. If what is here is typical, perhaps he is right.

Yes, the ON model looks like what one would expect, even if the data sheet said elsewise.

As for ON in general, I suspect that they are as good now as the Toshibas. I just find it hard to believe that they are "way better", as some claim.

Jocko
  Reply With Quote
Old 19th September 2003, 08:46 AM   #7
Account Disabled
 
Join Date: May 2002
Default Re: More data

Quote:
Originally posted by andy_c
Well, I finally got done with a preliminary evaluation of several SPICE models for the MJL3281A and MJL1302A to compare their simulated performance, mainly of ft vs collector current, with the data sheet values. This all started a while back when I was looking at the simulated performance of a power amplifier with a capacitive load of 2 uF in parallel with 8 Ohms using these devices for the output stage. I was trying to see if I could get the thing stable for this load with no output inductor. It turned out that the simulated open-loop output inductance of the amp was so large that a major resonance occurred at about 100 kHz, preventing stability from being achieved with any reasonable unity loop gain frequency with the capacitive load. In a previous thread involving Fred and myself (which I can't seem to locate at the moment), it became apparent that the models he was using with his simulator and the models I was using, provided by On Semiconductor, were quite different. We got very different results for the output inductance using the same test circuit.

This subject came up again in the thread about the amp in the Randy Slone book. But seeing that Randy Slone thread title keep coming up again and again made me feel like giving Randy a break - and the discussion of models really didn't have anything to do with the original thread topic anyway. So I thought I'd post the results of my evaluation in a new thread specifically about the SPICE models for these devices. My main purpose is to end up with a modified model whose simulated output inductance will be as close as possible to that of the real devices, assuming the real devices match up with the data sheet. Actually, I'd like as many of the parameters to match up as closely as possible with reality, but I'm starting with ft vs frequency. The desire to compare simulated and data sheet ft values came from the following site: http://www.reed-electronics.com/ednm...2596/09df3.htm. There they have an expression for the output inductance of an emitter follower as follows:

Lout = R / (2 * pi * ft)

where R is the internal plus external base resistance. This clearly shows the need for accurate ft in the model to get accurate output inductance. I'll also look at the internal base resistance, but that will be the topic of another post to this thread. I have three models for each of the NPN and PNP devices: the On Semiconductor models, the PSpice models for the Toshiba 2SC3281 and 2SA1302, and the models Fred posted in the thread I referred to earlier. I'm not sure if Fred's models were for the Toshiba or On Semiconductor devices though.

The simulation test circuits for ft are similar to those shown in http://www.diyaudio.com/forums/showt...089#post235089, except that I put the DC supply in the base instead of the emitter (to keep a constant Vce) and set the collector supply to 10Vdc to match the value used in the ft vs Ic plots in the data sheets. I temporarily placed a current source in the emitter to set the currents to the desired values, then determined Vbe. Then I used these Vbe values to set the currents when doing the actual ft simulation. The result is a spreadsheet with two plots and the raw data. So without further ado, here is a plot for ft vs collector current for the MJL3281A.

Quote:
Originally posted by andy_c
...and below is a plot for ft vs Ic of the MJL1302A. Clearly, the models for the MJL3281A are all pretty far off from reality, though the new On Semiconductor model for the MJL1302A looks at least reasonable. For small-signal analysis, the ft value for Ic of 100 mA is probably the most important. For the MJL3281A at 100 mA, the On Semiconductor model is more than a factor of six low for ft. So this says if the model can be tweaked to get this right, my previous estimates of power amp performance with a capacitive load will have been shown to be very pessimistic. This weekend I'm going to play around with the parameters of the On Semiconductor models in an attempt to get the plots to match up with the data sheets as closely as possible. I'll keep y'all posted on what happens. I'm going to try to fix the DC parameters first, then go for ft vs current. I'll also have a look at the internal base resistance if time allows.


Great work Andy....cheers
  Reply With Quote
Old 19th September 2003, 10:50 AM   #8
jcarr is offline jcarr  United States
diyAudio Member
 
Join Date: Jul 2002
Location: Tokyo, Japan
Jan:

>The Pspice models clearly are a joke.<

IME, many of them are. Spice is useful, but unless you are sure that your models are trustworthy (which is when?), better take the results with a large pinch of salt.

I have built circuits that appeared fine in the simulator, but proved pretty much impossible to get working in the real world

But I have also made circuits that performed far better than what the simulator predicted.

Jocko:

>Phred has told me countless times that the PSpice models are dreck. If what is here is typical, perhaps he is right.<

My experience suggests the same, time and time again.

But note that at least ft-Ic and capacitance-voltage curves can be found in many data sheets, so it is possible for hard workers like Andy C to plot the "simulated" curves against reality and locate the differences.

So what do you do when you are interested in Early voltages and other parameters that are _not_ stated in the data sheet?

Anyone know of an affordable but decent curve-tracer kit?

Nice post, Andy!

regards, jonathan carr
__________________
http://www.lyraconnoisseur.com/, http://www.lyraaudio.com
  Reply With Quote
Old 19th September 2003, 11:05 AM   #9
diyAudio Member
 
jan.didden's Avatar
 
Join Date: May 2002
Location: Great City of Turnhout, Belgium
Blog Entries: 7
Quote:
Originally posted by jcarr
Jan:

>The Pspice models clearly are a joke.<

IME, many of them are. Spice is useful, but unless you are sure that your models are trustworthy (which is when?), better take the results with a large pinch of salt.

I have built circuits that appeared fine in the simulator, but proved pretty much impossible to get working in the real world

But I have also made circuits that performed far better than what the simulator predicted.
[snip]
nice post, Andy!

regards, jonathan carr
Jonathan,

I used to use a spreadsheet-based model maker from an early IsSpice version called, surprisingly, ModelMaker. Basically you put in as many parameters as you can find on the data sheet, guess on the once you are not sure about, and the program generates the model file. I need to see if I still have it.

But over the years I have gone back from trying to simulate everything until the last volt, amp or Hz. Nowadays I use the simulator more as a "proof of concept" tool and then built a prototype. I find that faster: you need a few iterations in the PCB layout anyway and this way you can combine that with electrical tweaking. (The big boys call it "concurrent engineering", I call it common sense).

Thanks to Andy, we are again reminded that the map is not the world!

Enjoy the weekend,

Jan Didden
  Reply With Quote
Old 19th September 2003, 11:34 AM   #10
jcarr is offline jcarr  United States
diyAudio Member
 
Join Date: Jul 2002
Location: Tokyo, Japan
Jan:

I've been looking at MultiSim 7, not the least because it has an optional model maker function. Looking at the device models included with a lot of EDA packages has led me to believe that a home-brewed model couldn't possibly be any worse.

Your description of ModelMaker from IsSpice suggests that it is a stand-alone program (or interfaces with another spreadsheet program like Excel?). Is there any place to download a copy, or purchase?

>Over the years I have gone back from trying to simulate everything until the last volt, amp or Hz. Nowadays I use the simulator more as a "proof of concept" tool and then built a prototype.<

Similar situation here. Getting bitten a lot at first is a good way to learn quickly.

>Thanks to Andy, we are again reminded that the map is not the world!<

Very true. And those were only the semiconductors. The board layout is also an issue for stability and performance, and at times the passive components can cause problems as well.

regards, jonathan carr
__________________
http://www.lyraconnoisseur.com/, http://www.lyraaudio.com
  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
Spice models stinius Solid State 0 18th November 2008 10:07 PM
Spice models Grahamm Tubes / Valves 7 19th December 2006 02:36 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?

All times are GMT. The time now is 03:19 AM.


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