1
\$\begingroup\$

The objective is to make an audio amplifier. We have decided to make one that has four stages: a pre-amp with a gain of around 120, the next one is a CE amplifier with a gain of around 5, the third one is a bandpass filter, and the last one is the power amplifier.

We are in the second stage now, but the problem we are facing is that there is no DC offset observed at VBB, which is to be present. Don't know why we are facing this issue.

This shows that the there is no DC offset observed in the circuit. 12 V is coming from the source and the sine wave is that after the 220 kΩ resistor:

There is no DC offset observed in the circuit1

Circuit implementation in LTspice:

Circuit implementation in LTspice

Note that the CE amplifier circuit is working fine with the same values when run separately.

The voltage just before the buffer and the voltage after the buffer are overlapping, meaning no gain:

The voltage just before the buffer and the voltage after the buffer

Should we add extra DC voltage so that the amplifier circuit starts working? If yes, how should we do it? Or is there an entirely different reason?

\$\endgroup\$
3
  • 2
    \$\begingroup\$ If you are allowed to use opamps, why are you bothering with a discrete long tailed pair and a discrete CE stage??? Just doesn't make any sense. You can go straight to the output stage design and implementation and call it a day. \$\endgroup\$ Commented Feb 6 at 7:05
  • \$\begingroup\$ How are we supposed to know what V(n008) is? It's obviously not V(Vout). It would help a lot if you labeled nodes on the schematic. And besides the question about using opamps, the long tailed pair isn't right. You almost certainly will need to include emitter degeneration resistors (yes, that will degrade the voltage gain) because there's almost no way you will have matched BJTs there. (Or some other way to adjust for BJT differences.) You will also need resistors from base to ground and use a DC-blocking capacitor to the single-ended input of the long tailed pair, as well. \$\endgroup\$ Commented Feb 6 at 7:17
  • \$\begingroup\$ U1 (+) input is undefined at DC \$\endgroup\$
    – Designalog
    Commented Feb 6 at 9:02

2 Answers 2

1
\$\begingroup\$

This shows that the there is no DC offset observed in the circuit.

You are directly coupling the output of op-amp to the base of Q5. This will override the bias provided by R4 and R6, as long as the op-amp is not saturated, has sufficient drive, and has sufficient negative feedback. To DC bias Q5, add an AC coupling capacitor between the op-amp output and the node connecting R4, R6 and the base of Q5.

Be aware that the AC coupling capacitor and the parallel combination of R4 and R6 and the input impedance of Q5 form a high pass filter with cutoff frequency of

$$f = \frac{1}{2\pi R_{effective}C}$$

\$\endgroup\$
1
\$\begingroup\$

First a suggestions on drawing schematics in LTspice, set up your supply voltages apart from the rest of the schematic and label them, then use the labels in the circuit. This makes the schematic less cluttered.

Now some observations on your circuit:

You have two -12 V supplies, you can combine them into one.

You are using opamp buffers between stages for some reason, you don't need those. That's the main problem you're having, the first buffer has no DC reference, if you had left it out entirely you would have avoided this.

You have a current mirror for the input stage tail current, replace this with a current source. It's a lot easier during the design stage to know the exact current you're using, then once you get the circuit working you can go back and change it to a discrete design. In my experience unless you use a really bad current source design you'll get the same results with a discrete one that you get with the built in one, so make it easier on yourself early on.

Here's your circuit with the changes I've suggested, it looks like it works okay, with around 30 dB gain and around 1.4% distortion which isn't unexpected with no feedback. Note the spice directives I've used to improve simulation accuracy and measure harmonic distortion (view the log file to see distortion percentage).

enter image description here

Update: Here's the circuit with a few more modifications. I've AC coupled the input (forgot that in last schematic), added emitter degeneration, eliminated one collector resistor on the input stage and bypassed the base resistor for that transistor, and upped the gain of the second stage. Total gain is now 41 dB, harmonic distortion less than 0.1%, frequency response is flat through the audio range.

enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ That's funny! Here's what I'd tossed up, yesterday, when considering writing. ;) I'm still blocked by their use of opamps, which I cannot get around for now. It annoys me since there's little need to attempt to re-invent the wheel in that case. \$\endgroup\$ Commented Feb 7 at 2:22
  • \$\begingroup\$ @periblepsis That’s pretty close, I feel a bit validated now. :D I don’t know what’s up with the opamp buffers, have seem that in a couple of questions lately. \$\endgroup\$
    – GodJihyo
    Commented Feb 7 at 2:45
  • \$\begingroup\$ I'm just confused about the juxtapositions in the OP's schematic, I guess. And I'd be looking up to you for my validation (which is how I felt seeing that you'd produced something similar to me.) Hardly, the reverse. :) – \$\endgroup\$ Commented Feb 7 at 4:34

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.