First ever PCB layout for SMPS to linear PSU

[ramphands]

Hello there all!
I'm currently getting ready to build a modular synthesizer which requires a stable bipolar +-12v supply.
As transformers are very expensive over here, I decided a better route would be to take two 15v SMPS supplies and link them in parallel to create a bipolar supply with a common ground.  I will then run the supply through a LM350/337 combo to have a regulated 12v supply.  On the board I have it so that I will use a multiturn trimmer to dial in the precise voltage with resistors set to limit the adjustment range.
My only concern is the layout of the board.  I have the SMPS inputs coming in on the left side, with the common ground being tied together on the board.  The power traces are mirrored on the top and bottom of the board with vias along the traces and the output section of the regulators so that it can handle the expected 2-2.5A being drawn.  I've also put vias on the ground plane as that seems like a logical thing to do, although as I said it's my first ever pcb.

Any comments or criticism would be greatly appreciated.
Many thanks!

[floobydust]

It looks very good for a first ever 

I would add the reverse-polarity and backfeed protection diodes, see https://sound-au.com/project05.htm
With two 15V supplies, one might not be up, or come up/down before or after the other which can cause damage.

I would think about adding ferrite beads or inductors because SMPS are noisy and the linear vregs filter out some of it. Like 10uH on the input spades. But this depends on your synth design. Don't you need a 5V rail too?

Flat on an LED is the cathode, the footprint might be wrong. I use dim 4.7k-10k resistors for them.
I would have bigger pads (annular ring) for the spade terminals, they do get pushed around a lot.

[T3sl4co1l]

Don't worry about trace width, one is plenty.  It's only a couple amps.  More significant (which is to say, not really all that significant, but as long as you're asking, kinda thing) is the doubled-up traces block top side ground fill, making the ground vias not very useful, or useless.

The layout could be a lot tighter, but it's not like you're hurting from those few square inches, and the assembly will probably be easier this way.  Maybe a few bucks difference from most PCB fabs, your labor is easily worth more.

Tim

[ramphands]

Thanks for the kind words both of you.

Floobydust:
I've beefed up the pads as you recommended and will read up on how to add the ferrite beads and inductors.  I didn't add the protection diodes as I read in the TI datasheet for the LM350 that if the output voltage is under 25v and the capacitance is 10uF, they can be omitted due to the built-in protection.

Ooooooh and nice catch on the LEDs.  What on earth was I thinking?  Doh!

T3sl4co1l:
Regarding trace width, it's my first foray into power stuff so I was worried about stuff going awry and also trying to minimise voltage drop.  I guess my approach is overkill though as you pointed out.  I was also worried about getting the caps too close to the heatsinks so I didn't want to go too compact.  That and, as you stated, assembly.  Thank you for the advice about the ground fill - a complete, unbroken topside ground plane would be better, then? 

[nali]

Just wondering, what type of trimmers are RV1 & RV2? If they're like the side-adjusting Bourns you might not have access to them. Partly from the heatsink but also partly because they're mounted the same way instead of mirrored.

[ramphands]

Just wondering, what type of trimmers are RV1 & RV2? If they're like the side-adjusting Bourns you might not have access to them. Partly from the heatsink but also partly because they're mounted the same way instead of mirrored.

They're top-adjusting Bourns 3296Y trimmers.  Not entirely sure why I chose the staggered leg variant to be honest.

[MagicSmoker]

Well done, first layout or not. I strongly agree with Tim floobydust <ahem> on making the annular ring on the quick-disconnect (aka "Fast-On") tabs much larger. In some CAD software this will be done automatically by a restring rule under the design rules check (DRC), but it's best not to rely on that.

Oh, and trimpots with a staggered pin package are a little more sturdy.

EDIT - wrong attribution of the right advice... mea culpa

[T3sl4co1l]

Thank you for the advice about the ground fill - a complete, unbroken topside ground plane would be better, then?

Yup.  Breaks in either layer are fine (i.e., the negative space created around a trace), as long as they are stitched around with vias.  In this way, you can make even fairly complicated (though not very dense!) circuits, where traces mostly run on one layer at a time, always over ground plane (so, the fewer traces/buses crossing, the better -- trace crossings make a hole with no ground top or bottom), and the performance averages out to having two routing layers over a solid middle ground plane.  It's very good, without having to buy a 4-layer board.

Like this for instance, imagine the whole board looking like this:



Here, priority is on top routing (red), with pour filling around traces.  That pour is pretty sparse due to the routing on top, and it's stitched to the bottom (blue) where possible (with a preference for placing vias near trace crossings and peninsulas).  Also, obviously purple is copper top and bottom, a transparent view.  Meanwhile, the blue traces are short, and isolated where possible (so ground can fill between them).

Terrifically over the top for a simple linear regulator, but the strategies will benefit greatly as you move into more complicated circuits.

Well done, first layout or not. I strongly agree with Tim on making the annular ring...

Is flooby a Tim?  I never noticed...   For the record, I wholeheartedly agree; I recommend pad O.D. a bit less than twice the hole I.D.  Typical pad sizes:
ID  OD (mils)
 8  18*
12  25
20  40
30  50
35  60
40  70
60  100
80  130
etc.

*Budget fabs usually balk at holes this small.

Tim

[ramphands]

Thanks to all of you for the encouragement - I really appreciate it.  The pad sizes have been increased a lot following the advice given.  I actually had a quick look at some other PCBs with similar faston/quick connect terminals and... yeah they're all uniformly massive.  Goes to show you shouldn't blindly trust the pad sizes on footprints supplied by the manufacturer.

That image showing via usage makes it crystal clear - thank you!  I recall some old one-sided PBCs having ground pour islands and wondering what the point of them was (none, as it turns out), but it makes perfect sense that on a two-layer board you would be able to connect them into the ground plane with vias.

Really appreciate it, thanks!