In praise of: Cordell SPICE models of BJTs - diyAudio
Go Back   Home > Forums > Design & Build > Software Tools
Home Forums Rules Articles diyAudio Store Gallery Wiki Blogs Register Donations FAQ Calendar Search Today's Posts Mark Forums Read

Software Tools SPICE, PCB CAD, speaker design and measurement software, calculators

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 11th September 2011, 11:55 PM   #1
diyAudio Member
 
Join Date: May 2011
Location: Silicon Valley
Default In praise of: Cordell SPICE models of BJTs

I've been tinkering with LTspice simulations of high current drivers, which eventually led me to downloading and trying out Bob Cordell's free SPICE models at http://www.cordellaudio.com/book/spice_models.shtml

I've been simulating the "sustained beta" complementary pair MJE1302 / MJE3281 using Cordell models, and thus far I'm quite pleased. The model results (from my LTspice simulations) are shown in color below. The measured results (from ON Semiconductor datasheets) are shown in black and white.




I'm pleased for a couple of reasons:
  • The modeled NPN and PNP are not perfectly complementary, which strikes me as a nice dose of "Murphy's Law WILL bite you in the ***" for the potentially unrealistic world of simulation. NPN is just plain faster at all collector currents. You don't get perfect cancellation of base currents between the push and the pull. Deal with it.
  • The shape of the modelled curves is about right; peak fT around 2 amps, falling off both above and below. It's not some ridiculous flatline nonsense with constant fT at all collector currents
So far, I'm a very satisfied non-paying customer; thank you, Bob Cordell!
Attached Images
File Type: png measured.png (147.5 KB, 243 views)
File Type: png simulated.png (31.0 KB, 234 views)

Last edited by Mark Johnson; 12th September 2011 at 12:00 AM. Reason: mention that models are free
  Reply With Quote
Old 12th September 2011, 12:35 AM   #2
diyAudio Member
 
jackinnj's Avatar
 
Join Date: Apr 2002
Location: Llanddewi Brefi, NJ
We should tempt Mr. Cordell to unleash some of the other LTSpice models he has for MOSFETs. As our French brothers say, (loosely) "Le livre vaut le voyage".
  Reply With Quote
Old 26th September 2011, 11:26 AM   #3
diyAudio Member
 
Join Date: Apr 2011
Location: Pretoria
How did you plot those fT curves? Must be a big bucks commercial software product- I haven't seen that in LTspice.
  Reply With Quote
Old 26th September 2011, 02:42 PM   #4
diyAudio Member
 
Join Date: May 2011
Location: Silicon Valley
It's from LTspice. I used .MEAS along with .STEP, then copied the .MEASUREd results from the "Error Log" window into a file that I fed to Microsoft Excel for plotting. Surely you recognize the Calibri font, and other visual signatures of the plots, which positively scream Here Is Yet One More Excel Chart.

Inspecting the horizontal axis and horizontal spacing of the data points on the chart (30 equally spaced points per decade of collector current), you can quickly deduce that I must have measured fT using the DECade option of the .STEP statement. And you'd be right.

It's a fun little homework problem to design and debug a simulation "circuit" (or call it a "test fixture" if you prefer), which enables you to .MEASURE the fT of a transistor at a given collector current and VCE bias condition. Once you've got that, then merely .STEP the collector current and Bob's your uncle.

Last edited by Mark Johnson; 26th September 2011 at 03:10 PM. Reason: repair a paragraphing error
  Reply With Quote
Old 3rd October 2015, 11:17 AM   #5
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
I find that the model for 2n5401c returns an hFE that is massively higher than the 2n5551c
I am getting a sim result in amplifiers showing around 120 to 130 for the 5551 which is close to what I have in my stock of devices.

But the 5401 is reporting around 250 to 270 which is around double the hFE any in my stock.

What part/s of the model control hFE and can these be changed to better match real device hFE of 100 to 150?
Can these two be made more similar and still preserve the essential differences between NPN and PNP?

Quote:
*
* 2N5401C - created March 10, 2011 copyright Cordell Audio
.MODEL 2N5401C pnp
+IS=25e-15 BF=220 VAF=196
+IKF=0.2 ISE=2e-15 NE=1.4 NF=1
+RB=60 RC=2 RE=0.1
+CJE=35e-12 MJE=0.40 VJE=0.75
+CJC=15e-12 MJC=0.55 VJC=0.75 FC=0.5
+TF=800e-12 XTF=60 VTF=0 ITF=4
+TR=1.5e-9 BR=4 IKR=0
+EG=1.1 XTB=1.5 XTI=3 NC=2
+ISC=0 mfg=CA031011
*
*
* 2N5551C - created March 10, 2011 copyright Cordell Audio
.MODEL 2N5551C npn
+IS=9e-15 BF=125 VAF=667
+IKF=0.09 ISE=1e-15 NE=1.3 NF=1
+RB=92 RC=1 RE=0.1
+CJE=45e-12 MJE=0.35 VJE=0.75
+CJC=4.9e-12 MJC=0.30 VJC=0.75 FC=0.5
+TF=565e-12 XTF=300 VTF=5 ITF=2.0
+TR=1.2e-9 BR=3 IKR=0
+EG=1.1 XTB=1.5 XTI=3 NC=2
+ISC=0 mfg=CA031011
__________________
regards Andrew T.
Sent from my desktop computer using a keyboard
  Reply With Quote
Old 3rd October 2015, 11:34 AM   #6
diyAudio Member
 
Join Date: Apr 2008
According to Q Bipolar transistor - LTwiki-Wiki for LTspice and Explanation of most significant SPICE parameters :: NXP Semiconductors

BF is the 'ideal maximum forward beta' value

IKF is the 'corner for forward hFE high-current roll-off (controls where hFE falls at high IC, forward mode of operation)'

IKR is the 'corner for reverse hFE high-current roll-off (controls where hFE falls at high IC, reverse mode of operation)'
__________________
Regards,
currentflow
  Reply With Quote
Old 3rd October 2015, 12:23 PM   #7
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
BF certainly explains what I am seeing.
But there is something else.
for 5551 I'm getting hFE (Ie/Ib) ~127 cf BF=125 : very close.
for 5401 I'm getting hFE ~265 to 270 cf BF=220: exceeds the ideal hFE by >20%

I could just reduce BF to 120 to match the 5401 to the 5551.
Should I do anything else?
__________________
regards Andrew T.
Sent from my desktop computer using a keyboard
  Reply With Quote
Old 3rd October 2015, 12:34 PM   #8
diyAudio Member
 
Join Date: Apr 2008
Perhaps the IKF parameter should be adjusted too as your original models contain very different values. I don't use LTSPice, so I'm working blind!
At least you could experiment by making the IKF values equal for the two transistors and see if that gets you closer...
__________________
Regards,
currentflow
  Reply With Quote
Old 3rd October 2015, 12:35 PM   #9
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
changing 5401 BF to 125 brings the in circuit sim hFE down to 147 to 149 for the 3devices in my simmed amp (Pavel SymaSym)

Much closer to sim values for 5551 and much closer to measured values for my devices.
__________________
regards Andrew T.
Sent from my desktop computer using a keyboard
  Reply With Quote
Old 3rd October 2015, 12:37 PM   #10
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Quote:
Originally Posted by currentflow View Post
Perhaps the IKF parameter should be adjusted too as your original models contain very different values. I don't use LTSPice, so I'm working blind!
I can try that to see if there is any effect. But my 5401 are passing Ie ~2.4mA, hardly high current.
__________________
regards Andrew T.
Sent from my desktop computer using a keyboard
  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 stinius Solid State 0 18th November 2008 09:07 PM
Looking for SPICE models of power BJTs Jorge Solid State 9 21st July 2005 01:13 PM
looking for spice models bocka Software Tools 16 23rd November 2003 02:00 PM


New To Site? Need Help?

All times are GMT. The time now is 07:04 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2016 DragonByte Technologies Ltd.
Copyright 1999-2016 diyAudio

Content Relevant URLs by vBSEO 3.3.2
Wiki