3 stage audio amplifier help

Discussion in 'Homework Help' started by beatdown31, Apr 20, 2012.

1. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
Hello. I'm currently working on a 3 stage audio amplifier for a project and need some help. The load is a 8 Ω speaker and I need to get a 1V input at a gain of 10. If I'm right, it should work as longer as all the transistors connected are in some kind of operating range. However, the PNP in the current gain stage (lower right of schematic) keeps saturating and I'm having trouble fixing it without saturating the transistor in the current source (near the PNP in the same stage). Does anyone have any suggestions? I'll attach an LT Spice file to show you.

File size:
41.8 KB
Views:
65
2. jimkeith Active Member

Oct 26, 2011
539
99
post a screen shot.jpg as I'm having problems with this zip file

3. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
Here's assorted pictures of the circuit, as well as the full circuit. In the Differential Amplifier I left the audio source to the side because I'm currently running a DC analysis of the circuit. The PNP in the Current Gain Stage is what I'm having trouble with.

File size:
35.3 KB
Views:
101
File size:
45.6 KB
Views:
111
File size:
55.2 KB
Views:
113
File size:
52.3 KB
Views:
81
4. panic mode Senior Member

Oct 10, 2011
1,318
304
hi there,

i would work from output backwards.
you know the gain is supposed to be 10, driving 8 Ohm speaker.
the input of 1V is kinda high (are you sure it is not 10mV?).

Anyway, you take the input, multiply by gain and that should be your output.
now you can start calculating supply voltage, (output Vpp plus 1-2V).
if you know you peak output voltage and you know load, you can calculate current.
This is Ie for the transistor, from there you can get Ib. etc. (work backwards).

Once you are done with biasing, you can analyse small signal and verify gain.
If needed you may have to reduce gain by adding negative feedback.

If the one of transistor is in saturation, it's base current is too high.
Adjust the stage before it. From what I can see that is transistor acting as
constant current source (with zener at the base). to reduce that current,
increase resistor at emitter of that transistor.

Btw. you should try to bring those components closer,
your screenshots are not very usable..

Good luck.

5. t_n_k AAC Fanatic!

Mar 6, 2009
5,448
782
I'd change R14 (presently 100k) to something more logical ~ 2.2kΩ. R18 probably could be larger without compromising operation, thereby reducing the current drain.

6. jimkeith Active Member

Oct 26, 2011
539
99
The big problem here is Q4--there is no way to get enough voltage swing because the collector voltage or Q4 can never drop below the collector voltage of Q1 (close to ground potential). In my sketch, I changed Q4 to a PNP that works against the positive rail. Adjust the diff amp current /R1 resistance for about 0.6V drop to bias Q4 properly. This is a standard technique for interfacing from a diff amp.

Then the next thing I recommend is to drop the voltage of D5 to two diode drops--that way the current source can saturate closer to the negative rail.

These two changes will provide near rail to rail drive voltage.

R3 and R4 should be eliminated.

File size:
26.3 KB
Views:
82
7. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
Wow. So far, this has been a HUGE improvement. the bottom pnp is still a little saturated but it's way closer. I tried adding a third diode in the middle of the schematic and that brought pnp's VEB up, but it also made the npn's VBE increase as well. Thanks a lot for the help though. I'll keep toying with it and I'll keep you in touch with how it's going.

8. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
Alright. I've really gotten far with this design so far. My only problem left is saturation occurring around -6V. I'll attached another form of the design to show you. (I tried replacing the zener with two regular diodes, but when I did that the saturation started at -3V). I'll attach the shape of the wave as well

File size:
53.3 KB
Views:
84
File size:
36.9 KB
Views:
62
File size:
37 KB
Views:
51
File size:
136.2 KB
Views:
68
9. panic mode Senior Member

Oct 10, 2011
1,318
304
i am not so sure. i see no sign of calculation and the output is distorted, asymmetrical and clipped.

Btw. your circuit is still waaaay too spread and text is too small to read. there is good inch or two on top of the circuit that is just wasted space. output transistors can be moved good two inches to the left and entire circuit can be more compact, see what circuit in post 6 looks like - there is no need to squint.

question: what is your voltage supply? i guess you picked 13.8V or so? is that correct?

also why in the world you had to pick 15V zener in your constant current source? i'd want to have current source that can operate over widest possible range - even down to 2V or so (no some 15V). the other one is also terrible, monstrous 6.2V (me shaking head). references high like this limit possible voltage swing of the output nodes controlled by constant current. this is bad. as mentioned, your graph shows some problems - perhaps there is a reason for that.

here is my take on same problem. notice that unlike you, i chose my reference small to get maximum swing. also one zener or pair of diode is enough for bunch of current sources. i removed some values so you have to work for it...

• 3-Stage_test.png
File size:
19.7 KB
Views:
77
Last edited: Apr 22, 2012
10. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
Yeah, my teacher told me to make the zener really small, around 1V or 2V. Stupid LT Spice only provides 6.8V zeners at the smallest. I changed the zener in the right current source, but I forgot to change the first. Thanks for the help.

11. panic mode Senior Member

Oct 10, 2011
1,318
304
when you are selecting diode, you can sort the selection list by breakdown voltage and that makes easier to pick 1N750 which is 4.7V. also all components are stored in library that is in the LT Spice folder.

for example symbols are *.asy files:
C:\Program Files (x86)\LTC\LTspiceIV\lib\sym

the library components are in
C:\Program Files (x86)\LTC\LTspiceIV\lib\cmp

standard diodes are in file
C:\Program Files (x86)\LTC\LTspiceIV\lib\cmp\standard.dio

it is just a text file. it is easy to copy one diode and create new one.
help file explains what each of the fields are, although if you look at couple of zeners, it is obvious that BV is breakdown or zener voltage.

then you pick one of them, such as

.model BZX84C6V2L D(Is=1.5n Rs=.5 Cjo=185p nbv=3 bv=6.2 Ibv=1m Vpk=6.2 mfg=OnSemi type=Zener)

and paste copy of it, and slightly modify it, for example, here i create 3.6 zener (change in name, as well as bv=3.6 and Vpk=3.6):

.model BZX84C3V6L D(Is=1.5n Rs=.5 Cjo=185p nbv=3 bv=3.6 Ibv=1m Vpk=3.6 mfg=OnSemi type=Zener)

save and you are done. Note: on Win7 this is not so easy because of UAC. it is much simpler to copy file to desktop for example, edit it, then copy it back into folder
C:\Program Files (x86)\LTC\LTspiceIV\lib\cmp\

and when it asks for authorization, just say yes to overwrite it.
You just added new diode to your arsenal. start LT spice and enjoy...

beatdown31 likes this.
12. Audioguru New Member

Dec 20, 2007
9,411
896
Since you are making a power amplifier then don't you think it should use power transistors at its output?
The output voltage can easily try to be 10V peak which produces a peak current of 10V/8 ohms= 1.25A. Each output transistor will try to heat with 6.5W.

But the little 2N3904 and 2N3906 output transistors you are using have a maximum allowed current of only 200mA (and they perform poorly above only 100mA) and have a maximum allowed heating of only 0.625W.

13. beatdown31 Thread Starter New Member

Apr 20, 2012
6
0
I actually am using power transistors for for the output when I actually build it. I didn't try it in the simulation but I didn't think that would affect the output.