SparkFun Forums

[bigglez]

Newest revision:
Changed connectors to these, they are rated at up to 6A

Yes, much better!

A revised schematic would be helpful. I see 'placeholders'
for ganging the other amplifiers together, but I'm guessing.

You should revist the mechanical placements of some
parts, as there appears to be overlap. In general
the electrolytic capacitors need a larger space than the
footprints in the library. School of hard knocks, again.

I think the standard EAGLE library does NOT include
the plastic sleeves on the cans, and so these bind when
stacked together.

[TheDirty]

I'm assuming you know, but it looks like you are trying to work your components around that surface mount capacitor (C14). That capacitor will be on the opposite side of the board from all your other thru-hole components, so it can overlap those. You don't need to squish overything together to make space for it.

[SpikedCola]

Im not sure I understand what you mean. The through-hole components (resistors and such) are on the same side (the top) as C14. Maybe Im missing your point

[bigglez]

(C14). That capacitor will be on the opposite side of the board from all your other thru-hole components, so it can overlap those.

In EAGLE Red = top or cpmpoment side and
Blue = bottom or solder side. C14 is on the top,
along with all the other components.

[SpikedCola]

Moved the cap and trimpot around a bit to reduce the wasted space in the corner. Attached is the final-ish board and schem (all I need to do now is x-ref parts)

[TheDirty]

I've been working with single sided boards too long. I just have it in my head, thru-hole on one side, SMD on the other. Sorry about that.

[SpikedCola]

No problem!

[bigglez]

No problem! :)

I should have asked earlier, but this is only my
curiousity and not related to the PCB topic. Why
is the input capacitor so large? 10uF 400V?
Can't an SMT electrolytic do this job? How about an
NP type? Or is this one of those Audiophile folk
laws that can't be violated?

[bigglez]

No problem! :)

Another abnomaly. In the original design, and the
IC datasheet, the amplifier output has a series CR
network to ground. Often used to shift the dominant
pole and provide stability to a high gain closed-loop
stage. It's missing from your PCB. Why?

[SpikedCola]

To be honest, I have no clue why the input blocking cap is so large. Im just going by what the original creator used. Apparently its a good sounding, high-quality cap (Solen or similar brand)

And youre right about the capacitor! I must have overlooked it. Thanks!

[davep238]

To be honest, I have no clue why the input blocking cap is so large. Im just going by what the original creator used. Apparently its a good sounding, high-quality cap (Solen or similar brand)

And you're right about the capacitor! I must have overlooked it. Thanks!

While we're talking about capacitors, the data sheet shows a 100uF cap (your C14) connected between the MUTE pin (8) and GND, not between V- and GND.
-Dave Pollum

[SpikedCola]

Youre right about that too. However, according to my "original schematic" that is correct, but the datasheet (and the one from the designer's site: http://www.shine7.com/audio/bpa300.htm) show it being hooked to mute. I should probably double-check everything as the schematic Im using seems to have a couple incontinuities.

[SpikedCola]

After hooking up the sub and looking at the wires (and connectors) that came with the stereo, there's no way in hell that it will handle the power its "rated" for. Ive decided to use a single LM3886 instead of the three. Here is my next revision of the single board, and an updated schematic. As you can see, I hand-routed a few more traces this time than last time.

Let me just say thank you one more time to everyone who has stepped me through this so far. It has become much easier laying out this circuit than when I started, and I feel thats because of the help you have all gave me.

[bigglez]

Ive decided to use a single LM3886 instead of the three.

For a single stage (IC) amplifier you don't need the
trimpot, which is there to adjust DC offset of each
amplifier when used in tandem.

Your PCB layout needs some clean up work, as we
enter the area of personal taste and aethetics.

(1) Some of your capacitors are too close for comfort,
and may be hard to install. Leave a 25mil or larger
gap from outline to outline.

(2) All thee connectors are hanging off the PCB
outline.

(3) Few of the components have designators. Where is
U1 and U2?

(4) For better appearance the traces should run on
multiples of 90degrees, not random angles.

(5) Have you run ERC on your echematic?

(6) Have you run DRC on your board?

[SpikedCola]

What do I put in place of the trimpot? I assume the datasheet will say, so consider that rhetorical.

1. 25mil. Got it.
2. How far in is the "norm"? Or how far from the edge of the board is considered OK to place them?
3. U1 and U2 were from when I had three ICs on the board. Is there any way to make Eagle re-name all the components automatically? There are no identifiers because tName (I think) is turned off by default and I tend to leave it off when I lay out the board.
4. I forget if I read this somewhere or just dreamt it up, but are 90 degree corners bad? I tried to avoid them because I thought I read that somewhere, but if not Ill straighten out all my traces.
5. Yes, it gave me four errors, three telling me the connectors have no value (doesnt matter to me, I dont think its an issue), and one saying pin V+2 of the IC is hooked to V+ (again, it should be connected that way, its just a matter of how the pins are named in the library)
6. Yes, passed with no errors.