A more convenient basic lm3886 pcb

In order not to pollute the earlier "open source" lm3886 thread, here's a thread for the successor board, trying to benefit of the lessons learned along the way.

The new PCB has been rethought to be easier to integrate, with a bit less wiring too (the intended use for this redesign is integration into an active speaker). Which means:

- Its size is 4.75cm*10cm. This allows it to fit on a common 50*50mm, 2mm thick aluminum corner (if needed, cut to 50*40). If one picks 25*30mm caps (which go up to 6800uF/50V at mouser), the total height can be: 2mm (bracket) + 5 mm (diode bridge) + 1.6mm (pcb) + 30mm (cap)= 38.6mm.
- The PS is fully onboard, including the diode bridge, meant to go under the pcb and be heatsinked by the aluminum bracket. Main caps are 25mm wide. If height isn't an issue, you can find up to 10.000uF/50V caps in that diameter.
- There is no DC protection onboard as it isn't really necessary in most cases but there's an header to power an external board if so desired (see the open source thread).
-Ground loops are managed through both the possibility to use a 10R resistor between signal and power ground and the possibility to use a CL60 NTC between the power ground and chassis ground.
- Power inputs/outputs can be screw terminals or spades (vertical or angled connectors).

Obviously, all "optional" components are onboard (this is a completely standard datasheet implementation) and attention has been paid to the advices received in the past (thanks again to Tomchr, Mark Whitney, DPH, Bozoc, among others).

Comments, suggestions for improvement ?
 

Attachments

  • lm3886.PNG
    lm3886.PNG
    119.6 KB · Views: 742
Member
Joined 2009
Paid Member
You could easily make better use of the copper around the rectifier. I think you can also find some optimizations in the feedback path and in the connection between the quiet ground and the non-quiet ground. Further, I'd scrap the SMD resistor for Rmute and just have a leaded part over by Cmute.

"Managing" the ground loop by a resistor is often about the worst you can do. But you'll figure that out... ;)

Tom
 
Thanks for taking the time to have a look at it and comment. :)

Going back to in order:

- Yes, there's empty space around the bridge. Otoh, currents are clearly defined and the tracks are still 200mil wide. Compared to the situation where I'd have an external bridge and wires, it isn't too bad.
- Yeah, the feedback could be taken as close to the terminals as I can. It's quite easily done.
- The smd resistor is a leftover of an earlier layout... it kind of became an automatism. Yes, I've got more room here.
- Well, yes, the ground loop breaker and the hum breaker resistors are band aids. But in stereo or multichannel operation, they come handy. I'm aware that they increase thd a bit. I'd be worried about it with amps as good as the modulus. But with the barebone lm3886, it worries me less.
 

Attachments

  • lm3886.PNG
    lm3886.PNG
    124.8 KB · Views: 597
Member
Joined 2009
Paid Member
- Yes, there's empty space around the bridge. Otoh, currents are clearly defined and the tracks are still 200mil wide. Compared to the situation where I'd have an external bridge and wires, it isn't too bad.

You're paying for the copper anyway. Why not use it?

- Well, yes, the ground loop breaker and the hum breaker resistors are band aids. But in stereo or multichannel operation, they come handy. I'm aware that they increase thd a bit. I'd be worried about it with amps as good as the modulus. But with the barebone lm3886, it worries me less.

Given the number of "my chipamp build hums, now what?!" threads here, I'd worry more. But that's me.

Tom
 
You're paying for the copper anyway. Why not use it?
I'm often joking that the sentence best defining the people of my region is "leave well enough alone". More seriously, it's going to be hard to reclaim copper to use for the power groundplane and the power rails without moving a lot of things. So if I gain more copper, it's going to be for the connection between the bridge and the big cap or between the CT connector and the power groundplane. Unless I'm missing something, I won't gain much by further reducing the impedance of those tracks. What I could easily do is extend the CT return track a bit.

Given the number of "my chipamp build hums, now what?!" threads here, I'd worry more. But that's me.
Actually, I keep that option open because of those threads. In my experience, the hum breaking or ground loop breaking resistors did more good than harm to reduce audible hum. It hurts thd a bit but the trade off is sometimes useful. :scratch1: This has been discussed quite a bit in this thread, especially page 3 and 4.

I attach the pcb layer by layer, it's a bit clearer. As usual with Eagle, red is top, blue bottom.

PS: @Tom: ygpm
 

Attachments

  • lm3886-2.PNG
    lm3886-2.PNG
    113.3 KB · Views: 572
  • lm3886-3.PNG
    lm3886-3.PNG
    114.5 KB · Views: 556
Is any improvement when the feedback resistor is positioned like that? I just checked a picture of Tom's Lm3886 DR and looks similar, but in modulus 86 the feedback resistor is v. close to the lm3886 pins.
Is this still valid information?
 

Attachments

  • IMG_9902.PNG
    IMG_9902.PNG
    401 KB · Views: 488
Is any improvement when the feedback resistor is positioned like that? I just checked a picture of Tom's Lm3886 DR and looks similar, but in modulus 86 the feedback resistor is v. close to the lm3886 pins.
Is this still valid information?

Yes, there is an improvement. The shorter the path, the better. I solder them directly to the ICs legs, so there is no space for optimization.
 
There is a slight improvement. I see no reason why these posts would be any less true:
https://www.diyaudio.com/forums/chip-amps/295665-neurochrome-lm3886dr-build-3.html#post4815099
https://www.diyaudio.com/forums/chip-amps/321922-source-layout-lm3886-4.html#post5420338

The necessity of having very short connections for the feedback is only true in the lack of a Thiele network. If you look more closely at the mod86 pictures on neurochrome.com, it appears as if the global feedback is taken in a similar fashion as in the lm3886DR
 
Btw, here is the intended use for me. The black background is a 100*160*40mm heatsink. Two modules can fit on it, with a 10mm border all around, to mount it to the back of the speaker.

A small 40*47.5mm pcb can be mounted next to each amp. I intend to have a balanced line receiver and a LR4 filter section in one and a small DC-DC converter and another LR4 filter on the other. That would allow either a simplistic two ways or a FAST. What I'm considering is more a passive two ways driven by one amp, with the other amp driving a small sub.
 

Attachments

  • tempsnip.png
    tempsnip.png
    6.8 KB · Views: 201
Here is the kind of pcb that can easily be added.

Onboard there is an input buffer (SE or bal), a buffered BSC, a LR4 lpf or hpf and a level control. All through hole except for the opamps, good dual dip8 are getting harder to come by anyway.

A similar pcb will hold a second LR4 lpf or hpf plus a small dc-dc converter to power the two boards from the amp power rails.

PS: I will publish every eagle files once I've built a proto.
 

Attachments

  • lr42.PNG
    lr42.PNG
    19.4 KB · Views: 373
  • lr41.PNG
    lr41.PNG
    76.5 KB · Views: 374
  • Like
Reactions: 1 user
Neat little crossover board, I like the BSC being included. I've been sketching out some ideas for something similar, I just wanted to find a way to do it with Jfets, although a version using basic opamps will still perform well. I've got one up on perfboard with OPA2132P's that works great... in only one channel. I need to find out what's wrong and I've been tearing my hair out troubleshooting it, I may just build another one, but I'm out of suitable capacitors at the moment.

My suggestion- make it so that you can double up capacitors on the low pass (that run to the opamp output), and use series resistors to ground on the high pass at the opamp input. It'll make it much more versatile in getting the values just right, and reach a LR alignment with commonly available values. Think like the ESP project 09.

It'll make biamping with a big fat Class D subwoofer amplifier easy as pie :)
 
  • Like
Reactions: 1 user
What's the idea with the cutout in the board? It doesn't seem to serve any function and will increase manufacturing cost.

I think you could eliminate the cutout completely if you scooted some of the components a bit further right and dropped the mounting holes down a bit and moved the left ones to the right.

Tom
 
Some vendors will charge more for the more complex board shape. One vendor I used had a maximum of six route points before they started to charge more. Your board has eight points...

You could scoot the multi-turn pot and connector to the upper right of the board. That would allow you to pull in the mounting holes. You could then use short standoffs between the filter board and the amp board if you wanted to share the mounting holes. Just a suggestion.

Tom