SpikedCola:
Newest revision:Changed connectors to [these, they are rated at up to 6A[/quote]
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.](http://www.sparkfun.com/commerce/product_info.php?products_id=8084)
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.
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
In EAGLE Red = top or cpmpoment side andTheDirty:
(C14). That capacitor will be on the opposite side of the board from all your other thru-hole components, so it can overlap those.
Blue = bottom or solder side. C14 is on the top,
along with all the other components.
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)
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.
No problem! 
SpikedCola:
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?
Another abnomaly. In the original design, and theSpikedCola:
No problem!
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?
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!
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 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
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.
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.
For a single stage (IC) amplifier you don't need theSpikedCola:
Ive decided to use a single LM3886 instead of the three.
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?
What do I put in place of the trimpot? I assume the datasheet will say, so consider that rhetorical.
-
25mil. Got it.
-
How far in is the “norm”? Or how far from the edge of the board is considered OK to place them?
-
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.
-
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.
-
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)
-
Yes, passed with no errors.
Why does the input cap need to be rated at 400 volts? This seems like serious overkill to me. BTW, what is the voltage rating on the power supply caps (C17, etc)?
And to make the traces look nice, only use 45 and 90 degree angles. And while some people will say not to use 90 degree angles at all, 90 degrees will work out OK, especially for your wide traces.
-Dave Pollum
To be honest I dont know. Its supposed to be a high-quality cap, Im just following the original design in terms of parts. The power supply caps are rated at 63v.
Is there any way to have Eagle auto-rename all the parts, so it changes U3 to U1, and starts again at R1, C1, etc
EDIT
Next revision with straighter traces:
http://img132.imageshack.us/img132/6509 … v11fd4.png
Just outta curiosity, I ran it through the DRC bot on BatchPCB and the production price is <$8, way better than $40 for the original gerbers
I just thought i’d mention that you may have trouble mounting the LM3886
on your heatsink, as the tab isn’t off the outline of the board…
As the creator of the original project did, i like to use bars to clamp devices to
heatsinks rather than relying on the tabs of them to make proper contact, with
a unpunched piece of Mica and thermal compound, you gain superior electrical isolation…
Oh, and it looks like you have an airwire on the surface-mount capacitor… 
Thanks for pointing out the airwire! Turns out I had a trace under the pad that didnt get ripped up when I manually routed some other ones.
As for mounting a heatsink, I was planning to use a heatsink that was just large enough to cover the back of the chip, but protruded towards the back of the case and perhaps even out the back - I personally dont think it will be a problem mounting, however I trust your judgement and I moved the IC towards the back of the board (as far as I could without moving the power trace off the board). I actually like this layout better as it gives me more room for the larger input signal capacitors
v1.2:
http://img89.imageshack.us/img89/2033/singlev12qe6.png
Also, still wondering how to rename all the parts automatically if possible. How would I go about adding tNames to the silkscreen? Would that be part of the cam processor?
EDIT I also moved the caps and connectors down a bit to give me room if I decide to go with a larger heatsink
SpikedCola:
“How would I go about adding tNames to the silkscreen? Would that be part of the cam processor?”
That is to do with the CAM Processor… Oddly, i have actually just [posted about that to someone else 'round here!
BTW, your getting a good layout there… ](EAGLE Silkscreen Names - SparkFun Electronics Forum)