Hello Everyone,
I am new to the forum. I’ve been working at learning to use KiCad over the last couple years, when I have time. I am an electronics hobbyist with no formal training. Most of my experience is working on and building vacuum tube guitar amplifiers. I have done some repairs to PCB based electronics in the past, but haven’t really designed a layout before. I have done a lot of research on LED drivers and buck/boost converters. I also have studied the data sheet for the particular AL8843chip I based this design on. Anyway, here is my design as of now. Could any knowledgeable forum members please have a look at my design and layout? I would greatly appreciate any insights!! Just a few key points about the board…It is a constant current LED Driver board, powered from and external 24VDC power supply (accepts 4.5-40VDC) and used to power some high power LEDs (up to 3 amps). R1 and R2 (current sense resistors) values can be changed to limit the overall amount of current, while the pontentiometer is used to vary the current within a specific range with the 2.5V supplied by the TL431 chip. The evaluation board for the AL8843 had three input capacitors, but I chose two so far. (My values may be low only using two?) I’m also not sure if using a combination of different types of capacitors would be beneficial? ie… MLCC and electrolytic, film, etc.?? Also, the eval board had ground planes on the front and back. Seems to be some conflicting info on this? Anyway, please pick it apart, as I am trying to learn the RIGHT way to do things! I hope to be able to focus more time on learning electronics in the near future! Thanks for your help!!
BTW…I can’t post the schematic yet because I am a new member…
Schematic now posted!
From a superficial analysis, I like the way your layout looks. But it is difficult to say much without seeing the schematic. Is it possible for you to zip and post the entire project folder?
By the way I am a fan of powering circuits from spare 18V laptop power adapters. This might be a good candidate. I have a bunch of them. Some were mine and some from dumpster diving…
Quick glance and are the sense resistors in the right place please ?
I think so. Here is the schem from the data sheet and the eval board…
Yes, all is well, at first glance I thought there might be an issue 
If I get some time will go further, best of luck.
That would be great!! I would appreciate the help!! Thank You!!!
I do not know if you are a newbie, but this layout looks orders of magnitude better than that from most newbies.
A quick look at the datasheet does not tell me whether DI recommends a direct (zone or track) connection between pins 1-2 and the EP? I don’t think it will matter much but there is a slight chance that adding such would be better. Especially if this is a 2 layer board.
Wow! Thanks for the compliment BobZ!! I am a noob at PCB design and layout. I’m just try to do the best job I know how to on anything I do! I did a lot of homework before submitting this design for review. I don’t want to waste anyone’s time!
It is, in fact, a 2 layer board. Back side is all a ground plane except for one trace. The footprint for the AL8843 shows pins 1-2 connected to EP. So are you suggesting adding traces from pins 1-2 to EP on the TOP side of board, instead of the ground vias like I have used?
If you’re going to hand solder this, you can leave vias in pads. On the other hand vias don’t need to be there, there’s no benefit. For machine assembly it’s necessary to avoid normal vias in pads as much as possible – they wick in the solder paste and may cause bad joints.
Thermal vias are another story, they are difficult in any case. Hand soldering the IC1 thermal pad may be difficult. There’s probably too little space for solder paste for machine assembly/soldering.
There exists a hack for manual soldering a thermal pad. Put only one THT pad under it, with a hole large enough that you can heat it with a soldering tip from under and fill it with tin. You can also make the top side zone around it larger and put some more vias outside the part bottom area.
I will be hand soldering the board. Won’t the additional vias I added to the EP help with cooling? If I use a single plated thru hole instead of vias on the EP, what would be the recommended diameter of said hole to allow hand soldering??
I do that sometimes. I did not know that anyone else did.
The other thing might be to extend the EP North and/or South enough so that a wide screwdriver type soldering tip can be applied. But I do not see that you have a lot of room for that.
Yes but make sure that this is consistent with any recommendations from Diodes Inc.
Their datasheet does not get deeply into layout. Do they have a layout example somewhere such as an eval board design?
I’d agree, very good for a newbie!
I have two suggestions for the layout.
1 - on a two layer board there’s no real reason to have via-in-pad, I see 7 vias in pads that could easily be moved to just outside the pad.
2 - get in the habit of using the thermal relief for your zone fills. you can fine tune them per layer or net and you can override it on some pads if really necessary.
another suggestion is if you’re going to hand build this, then take a look at some of the “hand-solder” specific footprints that are already available. those will enlarge the pads so that you can get a soldering iron on them easily.
good luck!
Thank you! I’m trying!
Does this look better? Thank you for your suggestions!
I already thought of that. 
All the resistor and capacitor pads are hand solder footprints…
I will work on the other changes and ideas tomorrow.
I agree with others - good job.
My thoughts when looking at last layout:
Via near VR1 center pad seems senseless.
I would consider going with this one bottom layer track little higher to let IC1 GND connection be with the general GND region and not cut off from it (by this track).
If it were my design I would be trying to shift all VR1 stuff as much as possible to the left as in this circuit ‘real’ GND is only on the left and R3 connection to GND as you did is as longer from what it is expected to reference as possible. See at your schematic - R3 and IC2 are clearly referenced to C1,C2 GND connection and I’d be trying to make it as short as possible.
I’d also be trying to not have that bottom layer track at all (I always prefer continuous GND). Going with this signal under R1,R2 makes it possible - I’d certainly do that.
For such, signal tracks I use 0.25mm width so going under resistors is no problem.
At schematic using 1234-5678 order symbols seriously complicates reading for others than its author. I suppose mousey doubts were caused by this. Use symbol like they have in datasheet.