Hello All,

A few years back, I made a stereo amplifier, using a couple of LM380 ICs. I fabricated two separate mono amplifiers on their own PCBs and then mounted them in a case. The circuit that I used was taken from an old textbook at my high school.

The other day, I gave the amplifier to my brother and decided to fabricate another one, all on one PCB. I reverse engineered the PCB pattern to obtain the schematic and tested the design on breadboard, all seemed to work as expected... then I designed a PCB, fabricated it and soldered it up and started having issues. The volume control was making horrendous noises and the ICs were getting very hot, compared to the other amplifier I had built. I thought that the pot might have been faulty and got another one, but still had the same issues.

I've replaced every component in the board, with those that were in the breadboard and still the ICs get hot. Although the amp still functions, albeit noisily! So I decided to start disconnecting things to see if I could identify where the fault was occurring. I discovered that disconnecting the 3.3R resistors that are in parallel with the speaker stops the ICs getting hot and cures all issues with noisy pots etc.

So I was just wondering if you could tell me what the function of the resistor and capacitor in parallel with the speaker is? I assume it is some sort of filter? Do I need it in there? It seems mighty odd that the circuit with those resistors and capacitors in would work on two separate mono boards and also on the breadboard, but not on the stereo PCB? I've checked the stereo PCB design against the schematic and can't find any faults with it. I've attached the LM380 datasheet (which shows the resistor and capacitor in parallel with the speaker in the example circuits), the schematic and also the PCB pattern.

Any ideas or suggestions would be much appreciated.

Kind Regards

Edward Holmes

 

The resistor cap pair is a zobel network. Very common on the output of a power amplifier.

Is there a problem with your cap? Possibly failed as a short.

Did the same thing happen to both ICs?

 

Power supply decoupling -

ALL audio power amp ICs are notorious for breaking into oscillation if the power supply decoupling is inadequate. The two-capacitor approach is correct, but there needs to be a pair per amp chip. Also, they must be as close as possible to the power and GND pins. An extra few mm of capacitor lead length and pcb trace length matter.

Also, the system GND is a skinny little trace that wanders all over the place. First, fatten them up and break it up so the GND from each chip goes directly to its output connector and to the power input ground pin. This is called a star arrangement, and eliminates or greatly reduces the number of traces that have ground currents for both devices combined.

ak

 

Hello All,

A few years back, I made a stereo amplifier, using a couple of LM380 ICs. I fabricated two separate mono amplifiers on their own PCBs and then mounted them in a case. The circuit that I used was taken from an old textbook at my high school.

The other day, I gave the amplifier to my brother and decided to fabricate another one, all on one PCB. I reverse engineered the PCB pattern to obtain the schematic and tested the design on breadboard, all seemed to work as expected... then I designed a PCB, fabricated it and soldered it up and started having issues. The volume control was making horrendous noises and the ICs were getting very hot, compared to the other amplifier I had built. I thought that the pot might have been faulty and got another one, but still had the same issues.

I've replaced every component in the board, with those that were in the breadboard and still the ICs get hot. Although the amp still functions, albeit noisily! So I decided to start disconnecting things to see if I could identify where the fault was occurring. I discovered that disconnecting the 3.3R resistors that are in parallel with the speaker stops the ICs getting hot and cures all issues with noisy pots etc.

So I was just wondering if you could tell me what the function of the resistor and capacitor in parallel with the speaker is? I assume it is some sort of filter? Do I need it in there? It seems mighty odd that the circuit with those resistors and capacitors in would work on two separate mono boards and also on the breadboard, but not on the stereo PCB? I've checked the stereo PCB design against the schematic and can't find any faults with it. I've attached the LM380 datasheet (which shows the resistor and capacitor in parallel with the speaker in the example circuits), the schematic and also the PCB pattern.

Any ideas or suggestions would be much appreciated.

Kind Regards

Edward Holmes

And don't, don't, don't, put a solder pad for your components in the middle of the trace. Look how skinny that poor copper trace is! And, how skinny is it after you drilled? Did you remove even more copper? That is your main power supply filter cap! Remember, solder does not conduct as well as copper. Don't make your solder the bridge for all of your power.

Instead, make a pad and branch off to the pad - leaving your main power rail (trace) in tact.

 

Yep - I agree with AK - add some decoupling caps from pins 14 to 12 on your amplifier chips - as close to the chip as possible. 0.1uF, 50V, X7R ceramic is a typical choice for this circuit.

 

Can you define what "horrendous noise" means? Is it squealing or something else?

The power traces go all over the place with loops between the amps. For starters tack one 100nf cap directly at each amp. That might kill a squeal.

 

a resistor in parallel alters current but not voltage, allowing some to be redirected through it

a capacitor in parallel converts AC to DC and smooths (not as much as a coil inductor), so a sound wave should not be clipped because of course it will ride above 0V but not float above 0V

as to if that is right for your speaker - i dunno. is your speaker designed to push out on pulses only, or will it perform better if it pulls out and in?

distortion sounds like either (1) being over-amlified by an xfrm (but if you used IC amp i dunno) (2) clipping issues - something is clipping part of the wave

you dont somehow have a diode blocking in a place in a circuit before the wave became riding above 0V did you?

 

Also - Very good layout. I can see you spent a lot of time considering how to get all of the traces on one side of the board.

It looks like this is a single sided board with all of the traces on one side and the parts on the other. I'm just making sure this is the plan. If you place the parts and the traces on the same side you could possibly not be getting good connections in some places when you solder them down.

Finally - I'd probably flood that layer with ground. Put at much ground down as possible. This makes the ground line lower impedance and keeps the reference voltage at one single voltage (theoretically).

 

one use of parallel R C could be for "powered speakers"

you didn't switched from powered to non-powered speakers or what? no huge difference in impedence of speakers either? (your circuit "expects" a certain resistance range, if the resistance of speaker is far out of that range - say far less - it could cause serious issues unless the circuit had self-protections built-in, which is often omitted in small schematics)

 

Also - Very good layout.

Don't think so. All of his problems are layout-related. Also, even if you value single-sided-ness above signal integrity, there are many places for improvement.

Example. In this application a Zobel network works only if it has a very low impedance, and particularly low inductance, high-frequency return path to the chip's power GND. Note that the network's corner frequency is 500 kHz, the lower end of the AM broadcast band. Now look at the total loop length of the right-most chip's Zobel network. It is 10 times what it could be. If the output cap and 3.3 ohm resistor are moved to the right, and the 100nF cap is placed to the left of the resistor and rotated 180 deg, the trace length back to the 380's power pins is reduced by over 90%. Things are even worse for the left-hand circuit, and the improvement is more like 99%. Power routing has similar deficiencies. In both cases the layout still would be single-sided.

I'm not trying to dump all over the TS, merely pointing out that there is more to pc board layout than just connecting all the stuff on the schematic, and simple adjustments can turn a mess into a success.

ak

 

Hello All,

A few years back, I made a stereo amplifier, using a couple of LM380 ICs. I fabricated two separate mono amplifiers on their own PCBs and then mounted them in a case. The circuit that I used was taken from an old textbook at my high school.

The other day, I gave the amplifier to my brother and decided to fabricate another one, all on one PCB. I reverse engineered the PCB pattern to obtain the schematic and tested the design on breadboard, all seemed to work as expected... then I designed a PCB, fabricated it and soldered it up and started having issues. The volume control was making horrendous noises and the ICs were getting very hot, compared to the other amplifier I had built. I thought that the pot might have been faulty and got another one, but still had the same issues.

I've replaced every component in the board, with those that were in the breadboard and still the ICs get hot. Although the amp still functions, albeit noisily! So I decided to start disconnecting things to see if I could identify where the fault was occurring. I discovered that disconnecting the 3.3R resistors that are in parallel with the speaker stops the ICs getting hot and cures all issues with noisy pots etc.

So I was just wondering if you could tell me what the function of the resistor and capacitor in parallel with the speaker is? I assume it is some sort of filter? Do I need it in there? It seems mighty odd that the circuit with those resistors and capacitors in would work on two separate mono boards and also on the breadboard, but not on the stereo PCB? I've checked the stereo PCB design against the schematic and can't find any faults with it. I've attached the LM380 datasheet (which shows the resistor and capacitor in parallel with the speaker in the example circuits), the schematic and also the PCB pattern.

Any ideas or suggestions would be much appreciated.

Kind Regards

Edward Holmes

You might try a bypass capacitor (4.7 Ufd.) on pin 1.

 

The resistor cap pair is a zobel network. Very common on the output of a power amplifier.

Is there a problem with your cap? Possibly failed as a short.

Did the same thing happen to both ICs?

Thank you for identifying what it is called. The capacitors worked in the breadboard version but not the PCB version, which was when I transferred all of the components instead. Both ICs seem to get hot, but only when both are inserted, removing one seems to stop the other getting hot.

Power supply decoupling -

ALL audio power amp ICs are notorious for breaking into oscillation if the power supply decoupling is inadequate. The two-capacitor approach is correct, but there needs to be a pair per amp chip. Also, they must be as close as possible to the power and GND pins. An extra few mm of capacitor lead length and pcb trace length matter.

Also, the system GND is a skinny little trace that wanders all over the place. First, fatten them up and break it up so the GND from each chip goes directly to its output connector and to the power input ground pin. This is called a star arrangement, and eliminates or greatly reduces the number of traces that have ground currents for both devices combined.

ak

Thanks for the advice, I wasn't sure if it was to do with the power supply decoupling or not. In the past I have used 100nF capacitors over every IC supply, especially on logic circuits, but as the original amplifier made with two separate boards didn't have them, I didn't bother using them. The trace width of all tracks is 40mil, which is double the width of the tracks that I used on the original ones I think.

And don't, don't, don't, put a solder pad for your components in the middle of the trace. Look how skinny that poor copper trace is! And, how skinny is it after you drilled? Did you remove even more copper? That is your main power supply filter cap! Remember, solder does not conduct as well as copper. Don't make your solder the bridge for all of your power.

Instead, make a pad and branch off to the pad - leaving your main power rail (trace) in tact.

Thank you for the advice, I suppose I have never really thought about that. The holes were drilled at 0.8mm.

Yep - I agree with AK - add some decoupling caps from pins 14 to 12 on your amplifier chips - as close to the chip as possible. 0.1uF, 50V, X7R ceramic is a typical choice for this circuit.

It's going to be difficult to add extra to the circuit without re-designing/manufacturing it unfortunately.

Can you define what "horrendous noise" means? Is it squealing or something else?

The power traces go all over the place with loops between the amps. For starters tack one 100nf cap directly at each amp. That might kill a squeal.

The 'horrendous noise' is like popping and squelching when you turn the potentiometer. Other noise is just distortion when playing music with it. Any mains hum from the power supply is very little and the same on both the breadboard layout, original mono PCBs and the stereo PCB.

you dont somehow have a diode blocking in a place in a circuit before the wave became riding above 0V did you?

There aren't any diodes in the circuit.

Also - Very good layout. I can see you spent a lot of time considering how to get all of the traces on one side of the board.

It looks like this is a single sided board with all of the traces on one side and the parts on the other. I'm just making sure this is the plan. If you place the parts and the traces on the same side you could possibly not be getting good connections in some places when you solder them down.

Finally - I'd probably flood that layer with ground. Put at much ground down as possible. This makes the ground line lower impedance and keeps the reference voltage at one single voltage (theoretically).

The board is single sided. I try to minimize the number of wire links, but it is inevitable in some cases... there are two, labeled as 0R resistors. The reason I don't tend to flood a ground plane or similar is because although it reduces the amount of etchant required, it greatly increases the amount of tin plating solution that I use... and the tin solution is the most expensive chemical! Not to mention, the toner transfer method doesn't always work very well on large blocky areas.

one use of parallel R C could be for "powered speakers"

you didn't switched from powered to non-powered speakers or what? no huge difference in impedence of speakers either? (your circuit "expects" a certain resistance range, if the resistance of speaker is far out of that range - say far less - it could cause serious issues unless the circuit had self-protections built-in, which is often omitted in small schematics)

I haven't used either of the amplifiers with powered speakers and usually try to use 8R. I think the IC has built in protection, but I may have misread the datasheet.

Don't think so. All of his problems are layout-related. Also, even if you value single-sided-ness above signal integrity, there are many places for improvement.

Example. In this application a Zobel network works only if it has a very low impedance, and particularly low inductance, high-frequency return path to the chip's power GND. Note that the network's corner frequency is 500 kHz, the lower end of the AM broadcast band. Now look at the total loop length of the right-most chip's Zobel network. It is 10 times what it could be. If the output cap and 3.3 ohm resistor are moved to the right, and the 100nF cap is placed to the left of the resistor and rotated 180 deg, the trace length back to the 380's power pins is reduced by over 90%. Things are even worse for the left-hand circuit, and the improvement is more like 99%. Power routing has similar deficiencies.

I'm not trying to dump all over the TS, merely pointing out that there is more to pc board layout than just connecting all the stuff on the schematic, and simple adjustments can turn a mess into a success.

ak

To be honest, I have never really been taught about PCB layout. When I was at school, we used to use the 'auto-router' but I always found that I made incredibly messy layouts. I now manually route the tracks and just try to condense the layout as much as I can. I appreciate your feedback with regards to the layout, but the board is made now, so unless I fabricate another board, it kind of has to stay as is unfortunately.

You might try a bypass capacitor (4.7 Ufd.) on pin 1.

Again, the PCB is already made sorry, so I can't easily modify it unless I re-manufacture it or bodge something onto the underside of the board.

---------------------------------------------------

I really appreciate everyone's feedback so far... I hadn't anticipated so many replies in such a short space of time! So these 'Zobel' networks which are in parallel with the outputs, at the moment, with the 3.3R resistors removed are effectively disconnected... When they are disconnected, they stop the ICs from heating up and eliminate all noise (other than that from the mains hum), therefore, can they be left out or would it damage the IC over prolonged use?

I look forward to hearing from you.

Kind Regards

Edward

 

Hello All,

A few years back, I made a stereo amplifier, using a couple of LM380 ICs. I fabricated two separate mono amplifiers on their own PCBs and then mounted them in a case. The circuit that I used was taken from an old textbook at my high school.

The other day, I gave the amplifier to my brother and decided to fabricate another one, all on one PCB. I reverse engineered the PCB pattern to obtain the schematic and tested the design on breadboard, all seemed to work as expected... then I designed a PCB, fabricated it and soldered it up and started having issues. The volume control was making horrendous noises and the ICs were getting very hot, compared to the other amplifier I had built. I thought that the pot might have been faulty and got another one, but still had the same issues.

I've replaced every component in the board, with those that were in the breadboard and still the ICs get hot. Although the amp still functions, albeit noisily! So I decided to start disconnecting things to see if I could identify where the fault was occurring. I discovered that disconnecting the 3.3R resistors that are in parallel with the speaker stops the ICs getting hot and cures all issues with noisy pots etc.

So I was just wondering if you could tell me what the function of the resistor and capacitor in parallel with the speaker is? I assume it is some sort of filter? Do I need it in there? It seems mighty odd that the circuit with those resistors and capacitors in would work on two separate mono boards and also on the breadboard, but not on the stereo PCB? I've checked the stereo PCB design against the schematic and can't find any faults with it. I've attached the LM380 datasheet (which shows the resistor and capacitor in parallel with the speaker in the example circuits), the schematic and also the PCB pattern.

Any ideas or suggestions would be much appreciated.

Kind Regards

Edward Holmes

There's a noise reduction modification floating about for the LM 386 - might be worth seeking that out and see if its any use for the LM380. The LM386 is often dubbed; "the cockroach of audio amplifiers".

The TBA820 might be a bit quieter, but they're all very old types so there should be better parts in the catalogues.

 

It's going to be difficult to add extra to the circuit without re-designing/manufacturing it unfortunately.

Then your amplifier will probably never work - unfortunately. After looking more closely to the datasheet - there's a bypass pin (pin 1) that goes to signal ground (pin 7). Note that the maximum power output spec of the amplifier is spec'd with a 0.47uF cap on that pin. Add that cap at least - and probably the cap I told you to as well. You see - adding 470uF of capacitance will pretty much set any opamp to oscillating. Op-amps can't generally drive this much of a reactive load without going unstable (i.e. oscillating). The zobel network is meant to offset this to some degree - but it won't work if the chip is not properly decoupled. The issues you describe screams to me that the source is higher impedance than required. Do what you want - but this is probably the problem. Surely you can get 4 caps dead-bugged to you board.

The board is single sided. I try to minimize the number of wire links, but it is inevitable in some cases... there are two, labeled as 0R resistors. The reason I don't tend to flood a ground plane or similar is because although it reduces the amount of etchant required, it greatly increases the amount of tin plating solution that I use... and the tin solution is the most expensive chemical! Not to mention, the toner transfer method doesn't always work very well on large blocky areas.

On homemade boards I've seen people use other things as platting. In fact I've never heard of someone doing tin platting at home before. Solder is a great alternative if you just want to keep the copper from oxidizing and be cost efficient. I generally don't put solder all over the bare copper of my boards though. Sure they are a little uglier - but I have not seen any issues with a oxidation layer on my boards over the years - but I usually never use my prototype boards more than a few months. I will admit that I have not done any of my own home etched boards and at $1.67USD/sq inch for a two sided hobbyist board - I just don't see it being worth my time to deal with the chemicals and processes involved. In my quest to lower the impedance of your power source - a flooded ground plane is just another thing that will help.

 

This may be of some help, the circuit AWA model B411 was a commercial stereo record player from the late 70s. The other was a 1980s ETI magazine project. I never had the problem you are having using this IC. Took a while to find where I filed these circuits.

 

View attachment 100688 View attachment 100689 View attachment 100690 This may be of some help, the circuit AWA model B411 was a commercial stereo record player from the late 70s. The other was a 1980s ETI magazine project. I never had the problem you are having using this IC. Took a while to find where I filed these circuits.

Do you have more schematics of this LM380 ic in record players?

 

This thread ended over five years ago. If you have a related question, start your own thread and reference this one with a link.

ak

 

I also wasted my time reading 17 posts in this thread because the website software did not say at the beginning that it is a Very Old Thread.
Why not say the age of the thread on the first page in bright red??
The date is shown in pastel letters that can barely be seen.

 

I think this may also happen when someone clicks on "like" for very old threads. I have been caught out like that.

Les.