Audio amplifier (part 2)

O

Olivier Scalbert

Guest
Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which is
funny as I am doing electronics as hobby to change from being in front
of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png

I have only 2N3055 at disposal so I use a Sziklai pair (at least I
think!)...

BC546 and 556 will be replaced by bigger ones

Questions:

1/ Any big mistakes ?

2/ To move from A to AB, I think I need to change the value of R1 so Q1
conducts more or less. By doing that I will have DC on the load, so I
have to put a cap no ?

3/ What can be improved before building it ?

Thanks for your help,

Olivier
 
Olivier Scalbert wrote:
Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which is
funny as I am doing electronics as hobby to change from being in front
of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png

I have only 2N3055 at disposal so I use a Sziklai pair (at least I
think!)...

BC546 and 556 will be replaced by bigger ones

Questions:

1/ Any big mistakes ?
Click to expand...
I don't think so. It looks like you have a basic
understanding of what you are doing. Of course, that
strongly depends on what you are trying to do.

2/ To move from A to AB, I think I need to change the value of R1 so Q1
conducts more or less. By doing that I will have DC on the load, so I
have to put a cap no ?
Click to expand...
You have two separate but interconnected problems. How to
change the bias point for the two output transistors, and
how to produce a zero signal output of zero volts.

If you change R1 and R2 at the same time, you should be able
to change the bias point and still maintain the desired
output voltage. But this circuit depends strongly on
component matching and power supply voltage stability. More
practical versions use negative feedback to correct for
variations in components and supply voltages.

3/ What can be improved before building it ?
Click to expand...
First, you should make a functional list of "improvements"
(what would define a functional improvement in the
operation). Then you are in a better position to consider
circuit changes and how they interact with those functions.

First, I think you should explore frequency response. Your
test waveform is 100 Hz. Change that to 10,000 Hz and I
think one of the weaknesses of this circuit will start to
show up. Both of your output devices have lots of turn on
drive, but no turn off drive, so once they are on, they will
be very slow to turn off. This will produce increasing
distortion and higher bias current as frequency rises.

--
Regards,

John Popelish
 
Olivier Scalbert wrote:
Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which
is funny as I am doing electronics as hobby to change from being in
front of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png
Click to expand...

You *really* need to add resistors across the base/emitter of the output
transistors, otherwise speed will be an issue, especially once you put this
thing in an overall feedback loop.

I would tend to make them on the real low side, considering driving 3055's
to thier max needs 1A. Losing say, 100ma in these resister would be, 0.8/.1
= 8 ohms. Say, 10 ohms. However, this gives a tad of power in the drivers,
so you may want to consider anything from 20 to 100ohms. I wouldn't go over
100 ohms.

Kevin Aylward
kevin@kevinaylward.co.uk
www.kevinaylward.co.uk
 
John Popelish wrote:
Olivier Scalbert wrote:
Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which
is funny as I am doing electronics as hobby to change from being in
front of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png

I have only 2N3055 at disposal so I use a Sziklai pair (at least I
think!)...

BC546 and 556 will be replaced by bigger ones

Questions:

1/ Any big mistakes ?

I don't think so. It looks like you have a basic understanding of what
you are doing. Of course, that strongly depends on what you are trying
to do.

2/ To move from A to AB, I think I need to change the value of R1 so
Q1 conducts more or less. By doing that I will have DC on the load, so
I have to put a cap no ?

You have two separate but interconnected problems. How to change the
bias point for the two output transistors, and how to produce a zero
signal output of zero volts.

If you change R1 and R2 at the same time, you should be able to change
the bias point and still maintain the desired output voltage. But this
circuit depends strongly on component matching and power supply voltage
stability. More practical versions use negative feedback to correct for
variations in components and supply voltages.

3/ What can be improved before building it ?

First, you should make a functional list of "improvements" (what would
define a functional improvement in the operation). Then you are in a
better position to consider circuit changes and how they interact with
those functions.

First, I think you should explore frequency response. Your test
waveform is 100 Hz. Change that to 10,000 Hz and I think one of the
weaknesses of this circuit will start to show up. Both of your output
devices have lots of turn on drive, but no turn off drive, so once they
are on, they will be very slow to turn off. This will produce
increasing distortion and higher bias current as frequency rises.
Click to expand...
Thanks John for your help.

Do you think it is possible to change the design in order to have only
one potentiometer to change the bias of the transistors, instead of
changing R1 and R2 ?

For the negative feedback, I imagine that I have to measure the DC level
at the load resistor, compare it with 0, negate it and re inject it
somewhere in the input bias, but I do not see how ...

I have explored the frequency response. It is still ok at 10k and even
more . Pehaps the spice model of my components are too ideal. I should
put some parasitic inductances and capacitors ... or find other models ...

Olivier
 
Kevin Aylward wrote:
Olivier Scalbert wrote:
Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which
is funny as I am doing electronics as hobby to change from being in
front of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png



You *really* need to add resistors across the base/emitter of the output
transistors, otherwise speed will be an issue, especially once you put this
thing in an overall feedback loop.

I would tend to make them on the real low side, considering driving 3055's
to thier max needs 1A. Losing say, 100ma in these resister would be, 0.8/.1
= 8 ohms. Say, 10 ohms. However, this gives a tad of power in the drivers,
so you may want to consider anything from 20 to 100ohms. I wouldn't go over
100 ohms.

Kevin Aylward
kevin@kevinaylward.co.uk
www.kevinaylward.co.uk
Click to expand...
Thanks Kevin.
Yes you are right !
see: http://scalbert.dyndns.org/electronics/amplifier/schema2.png

Is it because there are too many charges into the base ?
And with the resistors, it is easier for the charges to go out of the
transistor ?

Olivier
 
On Wed, 22 Oct 2008 17:45:04 +0200, Olivier Scalbert
<olivier.scalbert@algosyn.com> wrote:

Hello, it is me again ...

After "jouling" some transistors, I decide to move to LTSpice. Which is
funny as I am doing electronics as hobby to change from being in front
of computers all day long !


I have some questions on this schema:
http://scalbert.dyndns.org/electronics/amplifier/schema1.png
Simulation is here:
http://scalbert.dyndns.org/electronics/amplifier/simul1.png

I have only 2N3055 at disposal so I use a Sziklai pair (at least I
think!)...

BC546 and 556 will be replaced by bigger ones

Questions:

1/ Any big mistakes ?

2/ To move from A to AB, I think I need to change the value of R1 so Q1
conducts more or less. By doing that I will have DC on the load, so I
have to put a cap no ?
Click to expand...
---
Not necessarily.

As John Popelish noted, using negative feedback and providing a little
bias when the input is at zero volts will force the output to be at zero
volts during those times.

Run this to see how it could be done:

Version 4
SHEET 1 1476 680
WIRE 512 -144 -208 -144
WIRE -128 -64 -576 -64
WIRE 224 -64 -128 -64
WIRE 368 -64 224 -64
WIRE 224 -16 224 -64
WIRE -208 16 -208 -144
WIRE 368 32 368 -64
WIRE -576 48 -576 -64
WIRE 0 112 -16 112
WIRE 96 112 64 112
WIRE 224 112 224 64
WIRE 224 112 176 112
WIRE 320 112 224 112
WIRE -128 160 -128 -64
WIRE -576 176 -576 128
WIRE -576 176 -672 176
WIRE -352 176 -448 176
WIRE -208 176 -208 96
WIRE -208 176 -272 176
WIRE -160 176 -208 176
WIRE -16 192 -16 112
WIRE -16 192 -96 192
WIRE 368 192 368 128
WIRE 512 192 512 -144
WIRE 512 192 368 192
WIRE -160 208 -208 208
WIRE -576 224 -576 176
WIRE -448 224 -448 176
WIRE 368 256 368 192
WIRE -208 272 -208 208
WIRE -16 272 -16 192
WIRE 0 272 -16 272
WIRE 96 272 64 272
WIRE 224 272 176 272
WIRE 320 272 224 272
WIRE 224 320 224 272
WIRE 512 320 512 192
WIRE -576 448 -576 304
WIRE -128 448 -128 224
WIRE -128 448 -576 448
WIRE 224 448 224 400
WIRE 224 448 -128 448
WIRE 368 448 368 352
WIRE 368 448 224 448
WIRE -672 528 -672 176
WIRE -448 528 -448 304
WIRE -448 528 -672 528
WIRE -208 528 -208 352
WIRE -208 528 -448 528
WIRE 512 528 512 400
WIRE 512 528 -208 528
WIRE -672 592 -672 528
FLAG -672 592 0
SYMBOL voltage -576 32 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 15
SYMBOL voltage -576 208 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V2
SYMATTR Value 15
SYMBOL voltage -448 208 R0
WINDOW 3 24 104 Invisible 0
WINDOW 123 20 110 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value SINE(0 1 20000)
SYMATTR Value2 AC 1
SYMATTR InstName V3
SYMBOL res 496 304 R0
SYMATTR InstName R1
SYMATTR Value 4
SYMBOL res -256 160 R90
WINDOW 0 -31 55 VBottom 0
WINDOW 3 -26 57 VTop 0
SYMATTR InstName R2
SYMATTR Value 100
SYMBOL res -192 112 R180
WINDOW 0 36 76 Left 0
WINDOW 3 36 40 Left 0
SYMATTR InstName R3
SYMATTR Value 510
SYMBOL res -224 256 R0
SYMATTR InstName R7
SYMATTR Value 82
SYMBOL nmos 320 32 R0
SYMATTR InstName M1
SYMATTR Value FDB2532
SYMBOL pmos 320 352 M180
SYMATTR InstName M2
SYMATTR Value HAT1072H
SYMBOL diode 64 96 R90
WINDOW 0 0 32 VBottom 0
WINDOW 3 32 32 VTop 0
SYMATTR InstName D1
SYMATTR Value 1N4148
SYMBOL res 208 -32 R0
SYMATTR InstName R6
SYMATTR Value 1000
SYMBOL res 208 304 R0
SYMATTR InstName R8
SYMATTR Value 1000
SYMBOL Opamps\\LT1007 -128 128 R0
SYMATTR InstName U1
SYMBOL diode 0 288 R270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName D3
SYMATTR Value 1N4148
SYMBOL res 192 96 R90
WINDOW 0 -31 55 VBottom 0
WINDOW 3 -26 57 VTop 0
SYMATTR InstName R4
SYMATTR Value 170
SYMBOL res 192 256 R90
WINDOW 0 -31 55 VBottom 0
WINDOW 3 -26 57 VTop 0
SYMATTR InstName R5
SYMATTR Value 170
TEXT -640 552 Left 0 !.tran .001 uic
TEXT -440 552 Left 0 !;ac oct 256 20 20000

JF
 
Olivier Scalbert wrote:

Do you think it is possible to change the design in order to have only
one potentiometer to change the bias of the transistors, instead of
changing R1 and R2 ?
Click to expand...
Yes, though it might produce other problems. The most
common way to produce the approximately 3 diode drop bias
voltage between the driver bases is to multiply the base
emitter drop of an additional transistor, with the
multiplication ratio set by a potentiometer (instead of
connecting 3 diodes in series).

The Vbe multiplier is described in this reference:
http://en.wikipedia.org/wiki/Voltage_source

You add a potentiometer in series with R1 and R2 to make the
ratio variable over a small range to set your output device
bias current. You choose the resistor value to make the
total current through the resistor divider to be about
1/10th of the current through the transistor, so that the
divider current times the current gain of the transistor
dominates the transistor conduction. The potentiometer
value compared to the fixed resistors should allow only
enough multiplier voltage variation to cover all the part
tolerances and a bit more. You can simulate the
potentiometer as two resistors in series that add up to the
pot total, but making the extreme value no lower than about
1 ohm (to keep the simulator happy, since it doesn't like
zero ohm resistors, and this is pretty close to the contact
resistance of many small trim pots).

Unfortunately, this bias generator eliminates the feed point
you are using for the amplifier that best balances the input
offset from zero. You could get his back by using the
adjustable Vbe multiplier to only replace the pair of diodes
on one side of the feed point, making only the drop of that
pair adjustable.

Or connect the output load in series with a capacitor so
that it is not possible for the amplifier to pass DC through
the load. If the load does not need to have a connection to
the supply ground, you might use a pair of capacitors, in
series across the total supply, and reconnect the grounded
end of the load to the common point in that series string.
This places a predictable DC bias across he capacitors, and
they help filter the real supply.

For the negative feedback, I imagine that I have to measure the DC level
at the load resistor, compare it with 0, negate it and re inject it
somewhere in the input bias, but I do not see how ...
Click to expand...
Since your amplifier stage has a gain very close to 1, just
adding more negative feedback would not do much good. You
also need to add gain to that operation. Say an opamp
connected as an inverting integrator. But normally, this
additional gain and inversion is produced by additional
transistors that make up a gain block ahead of this unity
gain output current booster.

I have explored the frequency response. It is still ok at 10k and even
more .
Click to expand...
Including the transistor collector currents? I think you
should start to see some distortion in the current wave
forms with this configuration.


Pehaps the spice model of my components are too ideal. I should
put some parasitic inductances and capacitors ... or find other models ...
Click to expand...
Are you using the models that came with LTspice?

A couple suggestions that would make the circuit more practical:

Connect the lower transistor pair without the 0.5 ohm
resistor between them. keep that resistor between them and
the output node, so it is more similar to the upper darlington.

Add a pair of 10 to 100 ohm resistors between base and
emitter of the two output transistors to make them turn off
faster.

--
Regards,

John Popelish
 
John Popelish wrote:

Thanks John, I need some times to digest all you told me !!!

Olivier
 
Olivier Scalbert wrote:

Thanks Kevin.
Yes you are right !
see: http://scalbert.dyndns.org/electronics/amplifier/schema2.png

Is it because there are too many charges into the base ?
And with the resistors, it is easier for the charges to go out of the
transistor ?
Click to expand...
"Too many charges" is not quite the right concept.

It is necessary to store charge in the base emitter junction
to turn the transistor on. It is necessary to remove that
charge to make it turn off quickly, after it has been on.
The junction will consume that charge, eventually, if you do
not drain it out, but that is a component and temperature
dependent process and most applications cannot tolerate the
long and variable self discharge time.

--
Regards,

John Popelish
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top