You don't need multiple resistors in parallel for the Zobel network (R+C to ground on the output of the amp). A 2 W metal oxide resistor works just fine.
The resistor in series with the amp output (many resistors in parallel) is not necessary.
I suggest lowering the supply voltage from the ±40 V you currently have to ±35 V. Due to the thermal limitations of the IC, you won't get any additional power out of it past ±35-36 V. For 4 Ω loads, I'd lower the supply to ±28-30 V for the same reason.
You can see my rationale here: LM3886 Output Power
You'll want to connect QGND to the speaker GND output terminal. You can see my explanation of why here: LM3886 chip amp grounding.
Tom
The resistor in series with the amp output (many resistors in parallel) is not necessary.
I suggest lowering the supply voltage from the ±40 V you currently have to ±35 V. Due to the thermal limitations of the IC, you won't get any additional power out of it past ±35-36 V. For 4 Ω loads, I'd lower the supply to ±28-30 V for the same reason.
You can see my rationale here: LM3886 Output Power
You'll want to connect QGND to the speaker GND output terminal. You can see my explanation of why here: LM3886 chip amp grounding.
Tom
Yes, it just poops on your DF and costs you power. If you leave it out, you should implement a resistor (~3-5 Ohm) and C (the 'usual' 100nF) in series to gnd after the coil though, that tames the top end power behaviour and also the HF 'sensitivity'.
If the speakers 'behave' or have only a narrow range of lower-than-7-Ohm impedance, +/-40V is fine, the LM3886 can cope very well with short term peaks. If the impedance is lower or for general use, I'd strongly endorse your suggestion on the lower rail voltages though. Your LM3886 page is very nice and really useful btw.
Hey guys,
Many thanks for the feedback.
tomchr:
I got the idea of the parallel resistors in the output from the Czech Gainclone schematic by Pavel Dudek using the LM4780 chip. Reading his circuit description with a little more care, I can see he meant the paralleled resistors are for a paralleled 4780 amp, which I don’t intend to build, so have removed them. From Pavels scree; quote…
“Parallel connection
The parallel amplifier application requires a small external output resistor, in our case 0,1Ω (ten times 1 Ω connected parallel). The amplifier is able to supply a heavy capacitive loading. I have tested the complex load consisting of an 8 Ω resistor and a parallel connected capacitor 100 pF to 5 μF with excellent results”.
So, I can do away with them as you recommend!
My speakers are 4 ohm Elac Uni Fi UB5’s I’ll also reduce the voltage as you recommend.
I’ve had a butchers at the LM3886 chip amp grounding article. Mostly it’s above my electronics knowledge level I’m afraid to admit! Do you mean by moving the Q Ground to the speaker ground, that I just move R1, 4R7 resistor to the speaker terminal and route to it accordingly? I don’t do away with the 4R7 ohm resistor do I?
ICG:
Pooping resistors removed as specified ha ha ha!!!
The resistors and cap at the output of the amp are as per Bob Cordell’s schematic…. 100nf and 3 ohms before the coil and not after as you specify (Hard to see the total R on my schematic sorry!) and 10ohms with 0.033microf after the coil. Have a look at Bob’s schematic please and comment on the values/ positions as you see fit.
Neither of you mentioned my PCB layout! I tried using the best of my extremely limited knowledge to follow some of the basic principles of keeping signal and output far from each other. Does it look like a screamer that’ll oscillate my ears off and make the cat run away, or do you think it may work?
Thanks again for the kind input.
Many thanks for the feedback.
tomchr:
I got the idea of the parallel resistors in the output from the Czech Gainclone schematic by Pavel Dudek using the LM4780 chip. Reading his circuit description with a little more care, I can see he meant the paralleled resistors are for a paralleled 4780 amp, which I don’t intend to build, so have removed them. From Pavels scree; quote…
“Parallel connection
The parallel amplifier application requires a small external output resistor, in our case 0,1Ω (ten times 1 Ω connected parallel). The amplifier is able to supply a heavy capacitive loading. I have tested the complex load consisting of an 8 Ω resistor and a parallel connected capacitor 100 pF to 5 μF with excellent results”.
So, I can do away with them as you recommend!
My speakers are 4 ohm Elac Uni Fi UB5’s I’ll also reduce the voltage as you recommend.
I’ve had a butchers at the LM3886 chip amp grounding article. Mostly it’s above my electronics knowledge level I’m afraid to admit! Do you mean by moving the Q Ground to the speaker ground, that I just move R1, 4R7 resistor to the speaker terminal and route to it accordingly? I don’t do away with the 4R7 ohm resistor do I?
ICG:
Pooping resistors removed as specified ha ha ha!!!
The resistors and cap at the output of the amp are as per Bob Cordell’s schematic…. 100nf and 3 ohms before the coil and not after as you specify (Hard to see the total R on my schematic sorry!) and 10ohms with 0.033microf after the coil. Have a look at Bob’s schematic please and comment on the values/ positions as you see fit.
Neither of you mentioned my PCB layout! I tried using the best of my extremely limited knowledge to follow some of the basic principles of keeping signal and output far from each other. Does it look like a screamer that’ll oscillate my ears off and make the cat run away, or do you think it may work?
Thanks again for the kind input.
That's because they are too polite to tell you the truth. It is bad, really bad.
Start by identifying the (current) loops in the schematic and look at the correct order to connect the parts. As an example. From the power connector (+0-) to the capacitors, to the LM3886. If you place these three traces alongside each other, both inductance and interference will be reduced. Aso, look at the amount of current that will flow through each trace. Are your traces wide enough?
Your layout is a classic beginner's connect-the-dots layout. It will probably work (i.e. wiggle on the input will result in a larger wiggle on the output), but if you want to at least get the data sheet performance out of the LM3886, it will need a lot of work.
I suggest reading: Taming the LM3886 Chip Amplifier
Also have a look at: LM3886 PCB vs Point-to-Point (with data)
Like Mark said, keep the large currents in mind and make sure the traces are wide enough. Also keep the inductance of the traces in mind (both on the supply and the output traces). Wide traces or planes have lower inductance than narrow traces.
Use a ground plane (lower inductance) but keep the current densities in the ground plane in mind. Keep sensitive circuits away from the high current flows - or add a moat in the plane to create a quiet section where you put the sensitive circuits.
Tom
I suggest reading: Taming the LM3886 Chip Amplifier
Also have a look at: LM3886 PCB vs Point-to-Point (with data)
Like Mark said, keep the large currents in mind and make sure the traces are wide enough. Also keep the inductance of the traces in mind (both on the supply and the output traces). Wide traces or planes have lower inductance than narrow traces.
Use a ground plane (lower inductance) but keep the current densities in the ground plane in mind. Keep sensitive circuits away from the high current flows - or add a moat in the plane to create a quiet section where you put the sensitive circuits.
Tom
Thanks guys.
I kind of knew what to expect as I am in fact a complete beginner!
My intention was to fab the PCB as I can get silk screen done locally. This for me would only be single sided though! Is this plausible or do I need another layer?
I’ll read all of the recommended material and see how I get on.
Would you mind recommending trace widths? I can make all of them wider except the power, and output at the 3886.
Thanks again.
I kind of knew what to expect as I am in fact a complete beginner!
My intention was to fab the PCB as I can get silk screen done locally. This for me would only be single sided though! Is this plausible or do I need another layer?
I’ll read all of the recommended material and see how I get on.
Would you mind recommending trace widths? I can make all of them wider except the power, and output at the 3886.
Thanks again.
Polite and lazy from my side. *sigh* Yes, it is. Sry.
You've wasted loads of space (could be done on less than the half the size, easily) and scattered parts all over it unnecessarily. The big caps should be as close to the LM3886 as possible and the width of the circuit path is too small for higher currents. There are a lot of bridges that could be avoided (you can use the surface below parts!). And most important, build a star ground. Yes, I see your ground point but it's not a star gnd just because you've got something resembling a star shape SOMEWHERE on the board. Keep the signal path short; move the DC servo much closer to the amp IC.
C22: What happened to it? That does not look like a 1nF. Why is C22 on the schematic only on the + side and no counterpart on the - rail? Especally the voltage regulators need high frequency eliminating 1nF caps, really close, it can become very ugly if they start to go haywire and these looong circuit paths are great antennas.
Move the output connectors closer to the LM3886, think about the spaghetti wires all over the board you'd need, it's not only the board, think about how it has to be wired and avoid long wires with high current.
You also forgot mounting points/holes for the mounting screws. I'd also suggest test points for the voltages (with written voltage and polarity beside it), even if that's more of a bonus.
I'm sure I still forgot a lot. I hope you find it constructive and helpful anyway.
I had an idea that there would be a lot to do, and for that reason alone decided not to try and do more than my present knowledge allowed before getting some very welcome expert opinion from you chaps.
Just for your information, my background is helicopter engineering, all grease, oil, gears, vibration, hot gases and noise, so you can maybe understand why my electronic attempts are troglodytic at best!
I will do my best to follow all of your very good tips and see what I come up with.
Just for your information, my background is helicopter engineering, all grease, oil, gears, vibration, hot gases and noise, so you can maybe understand why my electronic attempts are troglodytic at best!
I will do my best to follow all of your very good tips and see what I come up with.
No worries. We all started somewhere.
It's possible to make an LM3886 board like that, however, I strongly recommend using a ground plane. It's actually not that hard to make a two-layer board even using a home fab. I can usually get the registration between top and bottom layer to within ±0.25 mm on my home-made boards.
Sadly, the output and power traces are the ones that need to be wide. I suggest looking into copper pours. Normally, you can define a polygon in the layout and have the tool fill in the available space with copper.
Tom
If there isn't much room and the layout would be nice and super-compact otherwise, it can be an option to solder a solid wire onto the path as a reenforcement but that can usually be avoided.
The polygon and fill is an excellent method, why not use the advantages of software designing boards? Leaving more copper on the board also saves enviroment because less acid is used up.
A Slightly Different Take on the Cordell SGC w KK
Ok Fellas!
Time for you to have another giggle at my attempt at the Cordell SGC with Klever Klipper.
I thought it might be easier to use a quad chip (I think I might have been mistaken ha ha!!); the OPA4134 to be exact. I'm not sure which is the better route to follow. The previous idea using dual OPA2604's or the OPA4134. I'll make a final decision based on your input regarding this.
I've kept the OPA604 as the Buffer and used the entire OPA4134 for the remaining IC's.
I know, the board is still huge, no mounting holes and the routing a complete mess but that's my best effort to date!
I know there is still a lot to do and I'm going single sided as before, so routing has been a torment!
I've tried to put the quiet Ground close to the speaker output as recommended. Get the decouple caps close to the LM3886. Keep the power, ground lines close together. Increase track width. Use a power plane. Here is where I was not sure what to do, so made the entire board into a Ground plane.
Anyway, please feel free to pull out the flamethrowers. I look forward to all input and thanks for all the previous advice.
Best,
Mike
Ok Fellas!
Time for you to have another giggle at my attempt at the Cordell SGC with Klever Klipper.
I thought it might be easier to use a quad chip (I think I might have been mistaken ha ha!!); the OPA4134 to be exact. I'm not sure which is the better route to follow. The previous idea using dual OPA2604's or the OPA4134. I'll make a final decision based on your input regarding this.
I've kept the OPA604 as the Buffer and used the entire OPA4134 for the remaining IC's.
I know, the board is still huge, no mounting holes and the routing a complete mess but that's my best effort to date!
I know there is still a lot to do and I'm going single sided as before, so routing has been a torment!
I've tried to put the quiet Ground close to the speaker output as recommended. Get the decouple caps close to the LM3886. Keep the power, ground lines close together. Increase track width. Use a power plane. Here is where I was not sure what to do, so made the entire board into a Ground plane.
Anyway, please feel free to pull out the flamethrowers. I look forward to all input and thanks for all the previous advice.
Best,
Mike
Would you attach your layout as screen shots (images) rather than .pdf files? That makes it much easier to view.
You have an error in your schematic: When the mute switch is opened, the mute input of the LM3886 is floating. That's no good. You need to connect it either to GND (for mute) or to VEE through a resistor (for un-mute). You can take C24 out. It's not doing anything for you.
You need to add a 10-22 uF decoupling cap on VCC and VEE on the LM3886. The decoupling network needs to be 470 uF + 10 uF + 100 nF, according to the data sheet. I recommend 1000 uF + 22 uF + 1.0 uF (or 4.7 uF if you can find it). The 1.0 uF or 4.7 uF should be ceramic caps (X7R dielectric). The 22 uF and 1.0/4.7 uF should be right up against the IC. The bulk cap can be further away.
If you eliminate the 10/22 uF, the LM3886 will oscillate as the output approaches the supply rail, especially with 4 Ω load. Ask me how I know...
I think you're shooting yourself in the foot with the single-sided layout. If your goal is to be able to manufacture the board in your garage, I suggest putting a solid ground plane on the top. Protect this ground plane with some enamel when you etch the board. Once etched, you drill the component holes and make countersinks in the ground plane where you do not want connections. See the last image on this page for an example: DC RX Module. A properly executed ground plane will improve the performance of your amp and clean up the routing considerably. The only drawback of this approach is that for some components - like electrolytic caps - you might have to solder under the component, so you'll have to leave some room between the bottom of the component and the PCB. That's usually not a big deal.
While C13 is currently connected to the "ground plane", its connection is basically through a wide trace. That's not fantastic. Also note that the main current flows are from the supply connections to the reservoir caps and from the reservoir caps through the IC to the speaker. You need those current flows to see the lowest impedance (i.e. both resistance and inductance) possible.
Also note that R13, R14, and R15 should be 2 W types. It doesn't look like the footprints you're using will support those.
Tom
You have an error in your schematic: When the mute switch is opened, the mute input of the LM3886 is floating. That's no good. You need to connect it either to GND (for mute) or to VEE through a resistor (for un-mute). You can take C24 out. It's not doing anything for you.
You need to add a 10-22 uF decoupling cap on VCC and VEE on the LM3886. The decoupling network needs to be 470 uF + 10 uF + 100 nF, according to the data sheet. I recommend 1000 uF + 22 uF + 1.0 uF (or 4.7 uF if you can find it). The 1.0 uF or 4.7 uF should be ceramic caps (X7R dielectric). The 22 uF and 1.0/4.7 uF should be right up against the IC. The bulk cap can be further away.
If you eliminate the 10/22 uF, the LM3886 will oscillate as the output approaches the supply rail, especially with 4 Ω load. Ask me how I know...
I think you're shooting yourself in the foot with the single-sided layout. If your goal is to be able to manufacture the board in your garage, I suggest putting a solid ground plane on the top. Protect this ground plane with some enamel when you etch the board. Once etched, you drill the component holes and make countersinks in the ground plane where you do not want connections. See the last image on this page for an example: DC RX Module. A properly executed ground plane will improve the performance of your amp and clean up the routing considerably. The only drawback of this approach is that for some components - like electrolytic caps - you might have to solder under the component, so you'll have to leave some room between the bottom of the component and the PCB. That's usually not a big deal.
While C13 is currently connected to the "ground plane", its connection is basically through a wide trace. That's not fantastic. Also note that the main current flows are from the supply connections to the reservoir caps and from the reservoir caps through the IC to the speaker. You need those current flows to see the lowest impedance (i.e. both resistance and inductance) possible.
Also note that R13, R14, and R15 should be 2 W types. It doesn't look like the footprints you're using will support those.
Tom
Last edited:
I really would second the idea of going double sided. It will help a lot and small PCB really are cheap if you order from China.
The second thing I would suggest is to drop the DC servo. Properly sized caps aren't bad and it would simplify your layout quite a bit. Without the servo, you can treat all the input section with opamps as one clean sub section and the amp as another. You can then find plenty of example of lm3886 layouts to emulate for the amp section.
The second thing I would suggest is to drop the DC servo. Properly sized caps aren't bad and it would simplify your layout quite a bit. Without the servo, you can treat all the input section with opamps as one clean sub section and the amp as another. You can then find plenty of example of lm3886 layouts to emulate for the amp section.