Getting a little help building an audio amplifier - diyAudio
Go Back   Home > Forums > Live Sound > Instruments and Amps

Instruments and Amps Everything that makes music, Especially including instrument amps.

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 24th April 2013, 01:40 AM   #1
Noobert is offline Noobert  United States
diyAudio Member
 
Join Date: Apr 2013
Default Getting a little help building an audio amplifier

I am attempting to build this amplifier in LT spice: Basic Audio Amplifier

I am having some trouble with my LT spice build. Would it be possible for someone to remote desktop with me and take a look? Here is the file if you want to take a look on your own: https://dl.dropboxusercontent.com/u/...our%20appp.asc

Any help would be appreciated. Thanks.
  Reply With Quote
Old 24th April 2013, 06:09 AM   #2
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
I'm more inclined to help somebody who includes a little profile info about himself and his background . . . but since you provided a link and attached the circuit file I'll give it a shot. (At least until I have to actually THINK about the problem - thinking makes my brain hurt.)

Computer programs like LTSpice are rather simple things. They tend to do EXACTLY what you tell them to do . . . which MAY (or may not) be what you want them to do. Your attached circuit file simulates nicely, and its simulated behavior agrees with my intuition for the topology and values you have entered. (I have not done any calculations to check against simulated results.)

Your big error is the capacitor values you specified. The original SPICE program expected capacitances to be specified in FARADS and LTSpice has adhered to this standard. Most practical capacitors have values in the MICRO-farad, or PICO-farad range. Consequently LTSpice sees your C1 as a 2,000 microfarad capacitor; C2 is 200 uFd. While probably not very realistic, these values are tolerable. The 200 uFd output coupling capacitor with the 8 ohm load should be flat to a few hundred Hertz if I remember correctly; this may not be your design goal but you can see it in an .ac analysis and easily correct it.

What is causing the simulation results to be different from your expectations is the compensation capacitor (C3) value. The web page for your circuit suggests that 500 PICO-farads is a suitable value. Your circuit file calls for 2000 MICRO-farads - a value FOUR MILLION times larger than shown on the web page!

LTSpice allows you to use letter abbreviations for many standard engineering power-of-ten notations. In this case, use the lower-case "u" in capacitor values to represent "micro-farads", and lower-case "p" for "pico-farads". (I think those letter abbreviations are accepted by default, but you might have to poke around in the "Control Panel" menu and check a box to activate that feature.) Other letter suffixes it recognizes include upper-case "K" for "kilo-", upper-case "G" for "gig-", and I think it accepts lower-case "n" for "nano-". BE CAREFUL with "M"!! That is used for "milli-", e.g. "10M" could be the value for a 10 milli-ohm current-sensing resistor. If you want to specify a 10 MEG-ohm resistor, you need to spell out "10MEG".

Once you have corrected that problem . . . the LED's you use in the bias networks are setting the idle currents way too high! I'll let you do a little background investigation to get a better understanding of why it works this way.

(You can use LTSpice to do some of this investigation. Look at the DC operating point voltages for the nodes associated with the bias networks, then compare them to the operating point voltages when you use the diode types specified on the web page where you found the circuit.)

The output transistors you chose (2N2222/2N2907) are really NOT suitable for driving an 8 ohm load. I'm not sure how the simulator will behave since you're asking it to operate these devices well outside their design envelope. (I don't know if the devices called for on your circuit's web page are available in a basic LTSpice installation or not. I've added quite a few devices to my "standard.bjt" file, so just because a device is listed on my installation doesn't mean it's available to you. You should learn how to paste device models right on your schematic diagram and call them out using the "Component Attributes" dialog but for the first few hours you play with LTSpice it's easier to use the built-in models.

While you're playing with this file . . . add some labels to a few of the nodes so you can easily refer to them by name rather than cryptic (and changeable) node numbers. Also consider changing a few of the component designators to more meaningful names.

See atch screen capture.

Dale
Attached Images
File Type: png Capture.PNG (77.2 KB, 150 views)
  Reply With Quote
Old 25th April 2013, 03:44 AM   #3
Noobert is offline Noobert  United States
diyAudio Member
 
Join Date: Apr 2013
Quote:
Originally Posted by dchisholm View Post
I'm more inclined to help somebody who includes a little profile info about himself and his background . . . but since you provided a link and attached the circuit file I'll give it a shot. (At least until I have to actually THINK about the problem - thinking makes my brain hurt.)

Computer programs like LTSpice are rather simple things. They tend to do EXACTLY what you tell them to do . . . which MAY (or may not) be what you want them to do. Your attached circuit file simulates nicely, and its simulated behavior agrees with my intuition for the topology and values you have entered. (I have not done any calculations to check against simulated results.)

Your big error is the capacitor values you specified. The original SPICE program expected capacitances to be specified in FARADS and LTSpice has adhered to this standard. Most practical capacitors have values in the MICRO-farad, or PICO-farad range. Consequently LTSpice sees your C1 as a 2,000 microfarad capacitor; C2 is 200 uFd. While probably not very realistic, these values are tolerable. The 200 uFd output coupling capacitor with the 8 ohm load should be flat to a few hundred Hertz if I remember correctly; this may not be your design goal but you can see it in an .ac analysis and easily correct it.

What is causing the simulation results to be different from your expectations is the compensation capacitor (C3) value. The web page for your circuit suggests that 500 PICO-farads is a suitable value. Your circuit file calls for 2000 MICRO-farads - a value FOUR MILLION times larger than shown on the web page!

LTSpice allows you to use letter abbreviations for many standard engineering power-of-ten notations. In this case, use the lower-case "u" in capacitor values to represent "micro-farads", and lower-case "p" for "pico-farads". (I think those letter abbreviations are accepted by default, but you might have to poke around in the "Control Panel" menu and check a box to activate that feature.) Other letter suffixes it recognizes include upper-case "K" for "kilo-", upper-case "G" for "gig-", and I think it accepts lower-case "n" for "nano-". BE CAREFUL with "M"!! That is used for "milli-", e.g. "10M" could be the value for a 10 milli-ohm current-sensing resistor. If you want to specify a 10 MEG-ohm resistor, you need to spell out "10MEG".

Once you have corrected that problem . . . the LED's you use in the bias networks are setting the idle currents way too high! I'll let you do a little background investigation to get a better understanding of why it works this way.

(You can use LTSpice to do some of this investigation. Look at the DC operating point voltages for the nodes associated with the bias networks, then compare them to the operating point voltages when you use the diode types specified on the web page where you found the circuit.)

The output transistors you chose (2N2222/2N2907) are really NOT suitable for driving an 8 ohm load. I'm not sure how the simulator will behave since you're asking it to operate these devices well outside their design envelope. (I don't know if the devices called for on your circuit's web page are available in a basic LTSpice installation or not. I've added quite a few devices to my "standard.bjt" file, so just because a device is listed on my installation doesn't mean it's available to you. You should learn how to paste device models right on your schematic diagram and call them out using the "Component Attributes" dialog but for the first few hours you play with LTSpice it's easier to use the built-in models.

While you're playing with this file . . . add some labels to a few of the nodes so you can easily refer to them by name rather than cryptic (and changeable) node numbers. Also consider changing a few of the component designators to more meaningful names.

See atch screen capture.

Dale
Thanks so much for your help. I made the changes you suggested. I changed the caps, the diodes (to those of the original circuit), voltage rails to 13.8v, added the models for the power transistors and the circuit seems to be amplifying properly.

Here is what I have thus far: https://dl-web.dropbox.com/get/Worki...2TwhdIolBQsASQ
(I don't know if you have tip41c and tip42c in your library, but I figured there might be a chance)

I will be working on adding labels and learning exactly what each part/stage does tomorrow. Thanks again!
  Reply With Quote
Old 25th April 2013, 08:42 PM   #4
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Quote:
Originally Posted by Noobert View Post
Thanks so much for your help. I made the changes you suggested. I changed the caps, the diodes (to those of the original circuit), voltage rails to 13.8v, added the models for the power transistors and the circuit seems to be amplifying properly.

Here is what I have thus far: https://dl-web.dropbox.com/get/Worki...2TwhdIolBQsASQ
(I don't know if you have tip41c and tip42c in your library, but I figured there might be a chance)

I will be working on adding labels and learning exactly what each part/stage does tomorrow. Thanks again!
Your link gives an "Access not authorized" error.

You can often find simulation models by seeding a search engine with, e.g., "TIP41C SPICE". Another source is the "LTSpice" Yahoo group at http://tech.groups.yahoo.com/group/LTspice/ Please respect the members' time by searching the Files and old messages before posting "Can somebody send me a model for . . . ".

The quality and effectiveness of simulation models is a major topic by itself. The ones published by device manufacturers are usually OK for representing basic behavior in run-of-the-mill applications. You may also find some pretty crude models thrown together by individuals . . . . and in some situations a crude model is all you really need to investigate the behavior of a circuit. Occasionally you will find models that have been carefully crafted or modified by individuals to better represent some aspect of the physical component's behavior, or its behavior in certain situations. Bob Cordell's SPICE models are examples.

Here's what I found for the TIP4xx family:
.MODEL TIP41C NPN (IS=7.55826e-11 BF=260.542 NF=1.11221 VAF=100 IKF=0.526814 ISE=1e-08 NE=2.18072 BR=26.0542 NR=1.5 VAR=1000 IKR=3.54059 ISC=1e-08 NC=1.63849 RB=4.56157 IRB=0.1 RBM=0.1 RE=0.0162111 RC=0.0810556 XTB=0.1 XTI=1 EG=1.206 CJE=1.93296e-10 VJE=0.4 MJE=0.259503 TF=1e-08 XTF=4.06972 VTF=7.1157 ITF=0.001 CJC=1.09657e-10 VJC=0.730921 MJC=0.23 XCJC=0.803085 FC=0.8 CJS=0 VJS=0.75 MJS=0.5 TR=9.01013e-08 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP42C PNP (IS=5.65618e-10 BF=120.073 NF=1.24004 VAF=90.6071 IKF=1.46498 ISE=6.98929e-14 NE=4 BR=2.83268 NR=1.30331 VAR=27.1221 IKR=10 ISC=6.98934e-14 NC=3.78125 RB=4.71382 IRB=0.234602 RBM=0.12691 RE=0.000666374 RC=0.0927424 XTB=3.21145 XTI=1 EG=1.05 CJE=1.93221e-10 VJE=0.4 MJE=0.259369 TF=9.99163e-09 XTF=4.41941 VTF=6.53488 ITF=0.001 CJC=1.0962e-10 VJC=0.731968 MJC=0.23 XCJC=0.799902 FC=0.799995 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP41C NPN ( IS=290.83E-15 BF=113.55 VAF=100 IKF=1.9905 ISE=1.3946E-12 NE=1.4763 BR=.1001 VAR=100 IKR=10.010E-3 ISC=320.65E-12 NC=1.8994 NK=.58929 RB=.71129 CJE=348.44E-12 VJE=.78228 MJE=.42865 CJC=184.26E-12 VJC=.47897 MJC=.40458 TF=36.381E-9 XTF=100.32 VTF=21.563 ITF=28.791 TR=10.000E-9 Vceo=100 ICrating=6 mfg=Central_Semi)

.MODEL TIP42C PNP (Is=66.19f Xti=3 Eg=1.11 Vaf=100 Bf=137.6 Ise=862.2f Ne=1.481 Ikf=1.642 Nk=.5695 Xtb=2 Br=5.88 Isc=273.5f Nc=1.24 Ikr=3.555 Rc=79.39m Cjc=870.4p Mjc=.6481 Vjc=.75 Fc=.5 Cje=390.1p Mje=.4343 Vje=.75 Tr=235.4n Tf=23.21n Itf=71.33 Xtf=5.982 Vtf=10 Rb=.1 Vceo=100 ICrating=6 mfg=Texas_Inst)

You will probably want to check out "How to Import a Transistor Model in LTSpice" at http://courses.ee.sun.ac.za/Electron...20LTScpice.pdf (The associated course syllabus page at http://courses.ee.sun.ac.za/Electronics_365/ includes links to additional TIP4xx models.)

If you are studying this circuit as a way to learn about amplifiers (which is not a bad idea!), consider doing the following exercise, based on your observations from the circuit you first entered into LTSpice:
  • Learn to do a frequency response plot using the " .AC " analysis. Measure the upper and lower cutoff frequencies for your circuit.
  • Change some capacitor values, one at a time. The compensation capacitor might be a good place to start, since it's value was originally your most significant error. Increase, or decrease, its value by a factor of, say, 3 or 4. Then try a factor of 20 or 50. Or even 1000. What happens? Do you see why your original value gave the results you observed?
  • Do the same experiment with the input and output coupling capacitors. How do they affect overall performance?
Dale

Last edited by dchisholm; 25th April 2013 at 09:04 PM.
  Reply With Quote
Old 26th April 2013, 02:44 PM   #5
Noobert is offline Noobert  United States
diyAudio Member
 
Join Date: Apr 2013
Quote:
Originally Posted by dchisholm View Post
Your link gives an "Access not authorized" error.

You can often find simulation models by seeding a search engine with, e.g., "TIP41C SPICE". Another source is the "LTSpice" Yahoo group at LTspice : LTspice/SwitcherCAD III Please respect the members' time by searching the Files and old messages before posting "Can somebody send me a model for . . . ".

The quality and effectiveness of simulation models is a major topic by itself. The ones published by device manufacturers are usually OK for representing basic behavior in run-of-the-mill applications. You may also find some pretty crude models thrown together by individuals . . . . and in some situations a crude model is all you really need to investigate the behavior of a circuit. Occasionally you will find models that have been carefully crafted or modified by individuals to better represent some aspect of the physical component's behavior, or its behavior in certain situations. Bob Cordell's SPICE models are examples.

Here's what I found for the TIP4xx family:
.MODEL TIP41C NPN (IS=7.55826e-11 BF=260.542 NF=1.11221 VAF=100 IKF=0.526814 ISE=1e-08 NE=2.18072 BR=26.0542 NR=1.5 VAR=1000 IKR=3.54059 ISC=1e-08 NC=1.63849 RB=4.56157 IRB=0.1 RBM=0.1 RE=0.0162111 RC=0.0810556 XTB=0.1 XTI=1 EG=1.206 CJE=1.93296e-10 VJE=0.4 MJE=0.259503 TF=1e-08 XTF=4.06972 VTF=7.1157 ITF=0.001 CJC=1.09657e-10 VJC=0.730921 MJC=0.23 XCJC=0.803085 FC=0.8 CJS=0 VJS=0.75 MJS=0.5 TR=9.01013e-08 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP42C PNP (IS=5.65618e-10 BF=120.073 NF=1.24004 VAF=90.6071 IKF=1.46498 ISE=6.98929e-14 NE=4 BR=2.83268 NR=1.30331 VAR=27.1221 IKR=10 ISC=6.98934e-14 NC=3.78125 RB=4.71382 IRB=0.234602 RBM=0.12691 RE=0.000666374 RC=0.0927424 XTB=3.21145 XTI=1 EG=1.05 CJE=1.93221e-10 VJE=0.4 MJE=0.259369 TF=9.99163e-09 XTF=4.41941 VTF=6.53488 ITF=0.001 CJC=1.0962e-10 VJC=0.731968 MJC=0.23 XCJC=0.799902 FC=0.799995 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP41C NPN ( IS=290.83E-15 BF=113.55 VAF=100 IKF=1.9905 ISE=1.3946E-12 NE=1.4763 BR=.1001 VAR=100 IKR=10.010E-3 ISC=320.65E-12 NC=1.8994 NK=.58929 RB=.71129 CJE=348.44E-12 VJE=.78228 MJE=.42865 CJC=184.26E-12 VJC=.47897 MJC=.40458 TF=36.381E-9 XTF=100.32 VTF=21.563 ITF=28.791 TR=10.000E-9 Vceo=100 ICrating=6 mfg=Central_Semi)

.MODEL TIP42C PNP (Is=66.19f Xti=3 Eg=1.11 Vaf=100 Bf=137.6 Ise=862.2f Ne=1.481 Ikf=1.642 Nk=.5695 Xtb=2 Br=5.88 Isc=273.5f Nc=1.24 Ikr=3.555 Rc=79.39m Cjc=870.4p Mjc=.6481 Vjc=.75 Fc=.5 Cje=390.1p Mje=.4343 Vje=.75 Tr=235.4n Tf=23.21n Itf=71.33 Xtf=5.982 Vtf=10 Rb=.1 Vceo=100 ICrating=6 mfg=Texas_Inst)

You will probably want to check out "How to Import a Transistor Model in LTSpice" at http://courses.ee.sun.ac.za/Electron...20LTScpice.pdf (The associated course syllabus page at Elektronika 365 - 2012 includes links to additional TIP4xx models.)

If you are studying this circuit as a way to learn about amplifiers (which is not a bad idea!), consider doing the following exercise, based on your observations from the circuit you first entered into LTSpice:
  • Learn to do a frequency response plot using the " .AC " analysis. Measure the upper and lower cutoff frequencies for your circuit.
  • Change some capacitor values, one at a time. The compensation capacitor might be a good place to start, since it's value was originally your most significant error. Increase, or decrease, its value by a factor of, say, 3 or 4. Then try a factor of 20 or 50. Or even 1000. What happens? Do you see why your original value gave the results you observed?
  • Do the same experiment with the input and output coupling capacitors. How do they affect overall performance?
Dale
Thanks for your response.

I have already added the proper spice models to my spice directory. I was not asking for someone to find the models and do it for me. I was just stating that because I didn't want people to waste their time opening it if they couldn't simulate it without the models that I have. I suppose what I should have done is just posted the text here for each model that I added and others could add it to their libraries if they chose to view my circuit. Sorry for the confusion.

I am also sorry that I posted a link that was apparently not private. (wasn't thinking )

Current Circuit: https://www.dropbox.com/s/48974sqdro...ircuit138e.asc

Necessary models:
Tip41c:
http://www.onsemi.com/pub_link/Collateral/TIP41C.LIB
tip42c:
http://www.onsemi.com/pub_link/Collateral/TIP42C.LIB
dn14007 :
http://www.onsemi.com/pub_link/Colla...N4007.REV0.LIB

The circuit posted above still give me a very clean output with a gain of 10. I have changed some of the components to those that I have on hand so I could build it. I did build it and it does work, but sounds very bad. My goal is to make it sound good .

My hope is to learn about amplifiers by studying this circuit. I appreciate the bullets you posted. I will be running through those exercises later today.

Thanks for your responses. I really appreciate your insight.
  Reply With Quote
Old 26th April 2013, 04:47 PM   #6
diyAudio Member
 
indianajo's Avatar
 
Join Date: Jan 2010
Location: Jeffersonville, Indiana USA
Thanks for labeling your sample amp "compensation cap". I've repaired a few amps and read a lot of text here. I thought caps in that position (b-e on lower driver transistor) were just to prevent the output from radio frequency oscillating. The first transistor amp I repaired didn't have one from the factory; it was installed in a 3 year later modification. Will go back and read some threads and try to figure out what else designers are doing with it.
This is a simulation free zone unless I find a pspice program that is designed to work with Pentium IV CPU's with 500 MB ram and Linux op system. No money here for continual microsoft updates and upgrades. Easier and cheaper to build amps point to point on NEMA-LE boards and see what happens.
__________________
Dynakit ST70, ST120, PAS2,Hammond H182(2 ea),H112,A100,10-82TC,Peavey CS800S,1.3K, SP2-XT's, T-300 HF Proj's, Steinway console, Herald RA88a mixer, Wurlitzer 4500, 4300

Last edited by indianajo; 26th April 2013 at 04:50 PM.
  Reply With Quote
Old 28th April 2013, 02:30 AM   #7
Noobert is offline Noobert  United States
diyAudio Member
 
Join Date: Apr 2013
Hello all, I finally got it working on my breadboard. It plays music, looks good on my scope (no noise/cutoff).

The only concern I have is that it has a gain of 8 and in simulation it had a gain of 10. What could have caused this? Thanks for your help.
  Reply With Quote
Old 28th April 2013, 05:39 AM   #8
JMFahey is offline JMFahey  Argentina
diyAudio Member
 
JMFahey's Avatar
 
Join Date: Mar 2009
Location: Buenos Aires - Argentina
Welcome to the real World
  Reply With Quote
Old 28th April 2013, 01:44 PM   #9
Noobert is offline Noobert  United States
diyAudio Member
 
Join Date: Apr 2013
Quote:
Originally Posted by JMFahey View Post
Welcome to the real World
:P. So I guess it's safe to assume, gain in a simulation isn't always the same as what is built in a real world circuit. Thanks.
  Reply With Quote
Old 28th April 2013, 01:54 PM   #10
Mooly is offline Mooly  United Kingdom
diyAudio Moderator
 
Mooly's Avatar
 
Join Date: Sep 2007
I would look a little harder at your built amplifier and compare the circuit and the passive component values to those used in the simulation.

The gain should be identical (to within minute limits) of sim vs actual build for a simple design like this . There will be a real reason why the two differ. It could be a component value error or even something like a wiring error where the feedback signal is getting "modulated" or modified due to "real world" wiring having resistance. Are you measuring the gain at "mid band" frequency where the capacitors reactive component is negligable ?
__________________
-------------------------------------------------------
A simulation free zone. Design it, build it, test it.
  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
building an amplifier nayrdivad Construction Tips 3 16th November 2010 11:51 AM
Building A new amplifier steevo Solid State 0 10th November 2008 06:02 PM
Building a new Amplifier Frank Berry Everything Else 2 29th September 2008 11:18 AM
Building a sub amplifier AudioAddicted Solid State 0 6th November 2006 09:32 AM
Building an amplifier mbates14 Solid State 7 5th September 2002 02:14 AM


New To Site? Need Help?

All times are GMT. The time now is 11:52 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