PCB DESIGN

[gsingh11]

Hi, I am making my first ever PCB for my project. I have some questions in mind. Actually, i am driving a 3A motor with it and i am not sure what should be the track width of my traces to support my current. And if you find some more errors please help me resolve it before I send it to manufacture.

[ataradov]

High current tracks should be as wide as possible. And depending on the situation, it might make sense to make them out of filled polygons, not the tracks.

Layout is pretty messy, but this is typical for a first board. Most of the vias here are not necessary with careful rearrangement. And remember that component holes are vias on their own. Look at the track between the IC and R2. It all can just go to the blue layer. Same with R1. You already did it for the R3, why add 4 vias for the others?

And add ground fills on both layers. This will further eliminate messy routing.

[woody]

Kicad has a nice calculator tool that gives you an idea as to how wide a track should be for a given current (and copper thickness, temperature rise etc). Without taking it as gospel it shows you how these variables influence each other.

[Doctorandus_P]

It's a combination of temperature rise and voltage drop, and you can get a quite good idea from that from KiCad's built in calculator (from the project manager menu) as woody already mentioned.

On top of that PCB layout also has a very big influence. Consider an extreme example of a power distribution board. One connector with 10A goes in, and 10 connectors (each with 1A) go out.
If you put the 10A connector on the side of the board, then you have a 10A PCB track that has to go all the way to the 10th output connector. Just by moving the 10A connector to the center of the PCB, you split the PCB tracks in two 5A tracks right at that connector, and the average lenth of the copper track has also halved, so that is a factor of 4 improvement (in temperature rise and voltage loss) just by moving a single connector.

[woody]

An example of what @Doctorandus_P meant I used in a proto recently. Including the fat tracks used for high currents and cooling.

[EPAIII]

You can usually do most of the traces with a single width. But the high current traces need to be considered on an individual basis. That calculator that has been mentioned is a good tool.

But another thing is to consider those high current traces before you finalize the placement of the components. Resistance and power lost to heat depends on the length of the traces as well as their widths. So, by keeping those traces as short as possible you can be taking your first step at optimization. But parts can be moved after trace routing so you don't necessarily need to start from scratch.

[Infraviolet]

If U4 is what I think it is (atmega328p or other atmega, board acting as an arduino of a form) then C3 probably ought to be ceramic not electrolytic, and the circle in the silkscreen suggests you were planning on putting a can shaped electrolytic there?

If it is indeed at atmega chip, then I assume you're either going to program it with fuses set to use an internal clock, or otherwise you'd need to add a crystal and some 22pF caps to the board to clock the chip with.

You've easily got space for much thicker traces in many places if your current requires them, I can't really judge from an image though if they are wide enough yet, I'm sure it will work as it presently is (assuming you've got your circuit concept and net list correct), but if the traces aren't thick enough they'll heat up when in prolonged use and you'll waste some power. For high currents, I'm not sure which traces of yours carry them, but above 1A I'd usually make sure to have several vias in parallel whenever a high current trace switches layers, however thick the trace is a standard sized via is only "good" for a certain current, widening a via (unless widened an awful lot) doesn't increase current carrying ability so well as simply having multiple vias, so several vias in parallel does better when currents are larger.

Left of J5 you have a trace joining in to a corner at a 45 degree acute angle, I'd recommend reshaping this slightly to not have that sharp acute point, acid traps during manufacture aren't that common with modern fab houses, but I was always taught not avoid angles tighter than 90 degrees and use a bit of extra trace to fillet off the corner.

As a personal preference from my designs, I'd recommend putting component values (or abbreviated versions) in the silkscreen layer beside the relevant parts, makes the board self-documenting when you're assembling it by hand so you don't have to keep referring to a spreadsheet of what value R5 takes and so on.

[bson]

Trace width has not only a thermal impact, but consider also that it brings a voltage drop.  Since less is better, it's almost never a bad idea to use filled zones whenever possible rather than plain old tracks.  Basically, use as much copper as possible, and add matching copper fill or hatching on the other side to keep the board from warping.