You should always be mindful of traces that need to carry current but how you capture this information is down to where you are getting your card fabricated.
Fundamentally it is about cross sectional area: wider tracks = thinner copper for the same capability.
SaturnPCB toolsuite has a fantastic section on current capability (note: the calculator that comes with KiCad uses IPC-2221A, which is incorrect and you need a calculator that aligns with IPC-2152
So take 17A and assuming you want to limit self-heating to say … 5C
1oz copper -> 60mm wide track
2oz copper -> 30mm wide track
3oz copper -> 20mm wide track.
With a number of combinations of parallel tracking in between.
HOWEVER, this doesn’t actually answer your question as to how do you set the thickness. Typically you don’t in PCB tools, well not for information like this.
KiCad-6 does come with a stackup editor and this will give you an idea of overall thickness but this does not influence how wide a track should be, likewise this does not instruct the board fabricator as to the thickness.
So during your design you will need to settle on the thickness of the copper to manage your trackwidth while also considering etching limitation (3oz is ~ 0.25mm track and clearance, rules out SSOP devices). Once you have this settled on and you have a design with an acceptable amount of compromise its about how to request a 3oz PCB.
If you are using the online proto sites they pretty much come with standard weight and stackups so your early design needs to consider this - if a boardhouse only does 1oz then you will need wider or many traces etc.
Now if you are paying the extra for a custom stack up where you can have different weights on different layers (assuming you produce a balanced stackup to mitigate warping), its then down to communicating the information to the fabricator. I typically do two things
- add a stack of infomation to the Eco1.User layer
- Provide a fabrication pack
This is a 100A card I am presently working on
