Getting a little help building an audio amplifier

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
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
 

Attachments

  • Capture.PNG
    Capture.PNG
    77.2 KB · Views: 227
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/Working Circuit.asc?w=AAAqkPFuIzwhi2UMTRBF4VIn_Tgx4o5n2TwhdIolBQsASQ
(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!
 
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/Working Circuit.asc?w=AAAqkPFuIzwhi2UMTRBF4VIn_Tgx4o5n2TwhdIolBQsASQ
(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/Electronics_365/Praktika/Using your own models in LTScpice.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:
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/Electronics_365/Praktika/Using your own models in LTScpice.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/48974sqdrojro7o/Working Circuit138e.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/Collateral/1N4007.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.
 
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.
 
Last edited:
Administrator
Joined 2007
Paid Member
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 ?
 
Agree and add: real parts have tolerances.
Even if each one looks small ... they add up.
One feedback resistor 5% higher, another other 5% lower ... now you have 10,5% gain diference.
And **measuring** itself has tolerance :eek:
Some typical cheap multimeters have 5% tolerance , or a number that *sounds* smaller until you realize what it really means: "guaranteed accuracy 1% (or 2%) of full scale range" which means: if you are in a 200V scale , error may be up to 200V * 0.02=4V :eek: which if you are measuring, say, 180V is not much (it still is *almost* 2%) but if you are measuring, say, 26V , those 4V are *a lot*.
And why would anybody measure 26V on a 200V scale?
Simple, it overflows the next lower scale (20V).

Digital meters give a false sense of security if you don't consider these facts.
Simulators are far worse, the happily tell you that an amp has "158.457W RMS"
Indeed?
They must be taken for what they really are: excellent tools to save time, try ideas, but the final word comes from what you've built and sits in your bench.
 
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 . . .
I agree. The mid-band gain in this circuit should track very closely between simulation and measurements. If you are constructing with 5% tolerance resistors I wouldn't expect more than about 5% difference.

Can you share details of the procedure you are using to measure the gain?

As a quick first step to troubleshooting I would measure the values of the two gain-setting resistors with a multimeter. If that looks OK, I'd look at the DC operating point voltages (no signal applied) on each of the transistor connections, and compare to the simulated values. Since transistor characteristics vary widely even within a given type number you may find differences as high as 20% or so, but certainly anything greater than that would make me look for a construction error or a defective component.

Dale
 
You've got an output capacitor to the speaker so you don't need a fuse there. Of course one puts a fuse in the AC input to the transformer or switching power supply in case the diodes short out there. One can also put fuses between the output filter capacitor of the power supply and the rails, where the voltage source is shown in the schematic diagram. These fuses are outside the feedback loop so the amp should compensate for any errors they cause by being non-linear. The rail fuses could also protect any other output transistors if one of them overheats and fails.
 
You've got an output capacitor to the speaker so you don't need a fuse there. Of course one puts a fuse in the AC input to the transformer or switching power supply in case the diodes short out there. One can also put fuses between the output filter capacitor of the power supply and the rails, where the voltage source is shown in the schematic diagram. These fuses are outside the feedback loop so the amp should compensate for any errors they cause by being non-linear. The rail fuses could also protect any other output transistors if one of them overheats and fails.
Thanks for the replies. I will be adding those fuses today.

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 ?
Yes I believe I am measuring at midband. I checked again and I am getting a gain of 9.6 peak to peak today. I don't know what I was looking at yesterday .

Now I am working adding a potentiometer for volume control, and possibly tone and balance control. I have the volume control working okay with a logarithmic potentiometer, but it isn't perfect. The potentiometer should be wired into the input correct? Any suggestions on picking the proper potentiometer for my circuit?

For tone and balance it would just be 2 more potentiometers correct? How would you wire/set up the potentiometer for tone control? For balance?

Thanks.

Final build:
https://www.dropbox.com/s/vnmajwl1vdbrjd5/Working Circuit138ebuilt1.asc
 
For a simple integrated sample amp to copy look at the schematic of the Armstrong 625 on this thread http://www.diyaudio.com/forums/soli...rmstrong-625-gone-wrong-please-help-me-5.html post 48. It has the tone controls, high level and magnetic phono level inputs, just about anything you want or you can leave anything out. Biggest thing I see wrong with this amp is that if the output transistor bias control potentiometer breaks, the idle current runs away. If I build one I might put a clamp diode across the bias control pot. 40636 transistor was a specially selected 2n3055 for high voltage: sort of an early manufacturer's only 2n3772.
 
Okay thanks for all of your help guys.
Also, how does one go about designing something like this on their own? How did they know how to bias each bjt? When you bias one it certainly must change the values of other things in the circuit. Any background info on designing something like this would be appreciated :)
 
Administrator
Joined 2007
Paid Member
Okay thanks for all of your help guys.
Also, how does one go about designing something like this on their own? How did they know how to bias each bjt? When you bias one it certainly must change the values of other things in the circuit. Any background info on designing something like this would be appreciated :)

Designing successful circuits from scratch only comes when you have a thorough grounding and understanding of the theory and practice. For many that means having chosen electronics as a career.

Learning is a progressive thing though and you don't need to be at that level to take a design and modify or tweak it :)
 
Since the 2n3055 was invented people have been biasing TO3 transistors about 20 ma each pair. See the Armstrong 621 amp circuit above from the early 70's. They say to increase bias current until the turn on edges disappear from the oscilloscope trace on sine waves, but I don't have a sine wave generator or a scope. Djoffe designed a 20 ma closed loop bias circuit for my dynakit ST120, "deformed son of the Leak Stereo 70", and it sounds better with that much. Doesn't overheat, either. I can measure bias current with a voltmeter.
I fool around with old capacitor coupled circuits like this because if you make a stupid mistake it doesn't burn up your $600 pair of speakers. The speaker coupling cap stops the rail current before it hurts anything expensive. The latest design of an amp with speaker capacitor is the Sakis Geezer amp http://www.diyaudio.com/forums/solid-state/229120-g-amp.html
If you want to understand the terms around here, last week google found for me the build instruction document for the "honey badger" amp with an explanation of each transistor and what it does. The "honey badger" is a sticky thread at the top of "solid state" forum, sold as a kit by diyaudiostore, and is supposed to be your starter amp. Other than trashing your speakers if you make a mistake, I suppose it is a good choice. I've been wondering 2 1/2 years what a "long tailed pair" and "Vbe multiplier" are, and how a "CCS" or current source works. Not to mention the mysterious "VAS stage". The build instructions for the "honey badger" spells out those acronyms and points out which transistor is which, finally. Honey badger has got way more connections than I want to assemble point to point, but using $.08 transistors to stabilize current to signal amp stages makes economic sense, instead of using a $5 transistor and $8 heat sink to regulate the power supply like the Dynakit ST120 does.
If you're really a newbie, a good textbook I found surplus at Goodwill from the local community college was "Electronic Devices, the Electron Flow version" by Thomas L. Floyd. Great explanations of power supplies and how to use a meter, some basic amplifier circuits. It is a way better book than what I started on, "Electronics for Scientists (& dogs)", 1968 version, and "GE transistor manual 7th edition".
 
Last edited:
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.