Hey Everyone,
I am seeking some suggestions for high current PCB design. I am not able to figure out should I go for the 2 layer or 4 layer PCB for the 100 amps current carrying capacity PCB.
Also, can anyone please guide me with the trace width too, as the calculator included in Kicad show the disclaimer that, it is valid upto 35amps. So, I am bit hesitating to go ahead with it.
Thanks in advance.
What type of connectors are you going to use?
Excuse the pun, but you may not get anyone to touch this with a 10 foot pole. 
The two parts I quoted are a red flag when taken together.
Generally speaking, you shouldn’t be putting 100amps on a normal circuit board if you don’t know what you’re doing. It probably (just a guess) is going to require two full layers of 3oz copper to be safe, and that’s just for something like a backplane where you are just passing a relatively low voltage along. As mentioned earlier, the connectors are also critical.
Please consider providing context to what you are planning to do with this. Perhaps someone can suggest an off-the-shelf alternative or a more beginner-friendly approach.
I gave hermit a 
Designing for 100Amp is not trivial. Bad connectors can easily lead to overheating, distributing power from a single point entry of a connector is non trivial because of high local current density, and long term damage can occur because of repeated thermal stress on solder joints, and solder does not handle this well.
And there are probably other factors too, but I do not have enough experience in that area myself.
Yeah. At 100 amps I would think of wire. Maybe planes. But traces? I was going to ask voltage but, why? I’ve looked up a couple online calculators and they stopped at 35 also. One site had the needed formulas but this is a case of, if you have to ask then you probably shouldn’t.
So the reason the calculator doesn’t go above 35A is that is as far as the IPC testing goes to. It was all empirical testing and all calculators are “best fit” against these curves … there is always a small amount of error but once you go above 35A the divergence is totally unknown…
The KiCad calc follows IPC-2221 and it needs to be updated to IPC-2152 (I keep meaning to start working on this again )
You need some FEA tool to manage this but if you want to manage it via the calculator you need to split it into manageable chunks, ie 35Amps. Treat all as internal (for worst-case) and view whatever you read as MINIMAL.
Put as much copper as you can.
I used 20mm wide, 3oz copper on 3layers to conduct 80A continuously with 5-10C temprise. I however had a few area’s where I was extracting heat as well. This however had the luxury of Ansys and Hyperlynx to cross-check. There is work interacting KiCad with freecad to use some FEA solvers for exactly this reason
A couple items…
• You can do a FEA on the Circuit (use a test circuit with a single trace and desired PCB thickness and material
• Can set the material parameters in the menu’s and/or create a Materials panel with desired properties
• For a NOOB/Inexperienced designer, you face a good bit of Homework and it may not be easy (depends on your knowledge in related areas)
That said, here’s a Link to my Older post on doing Thermal analysis…
Good Luck
EDIT: Added… Here’s my Properties for Copper Trace and FR4 pcb material
(Also, but not shown: you can create a Calculation (Equation) for Temperature Rise/etc but, that’s far beyond a NOOB’s need, so just FYI)
I designed an H-bridge motor controller board that handles well over 100A. It uses two planes of 3oz copper, with many vias stitching the planes together. The connectors are PEM studs that are soldered after then are pressed in. The mating AWG 4 cable uses ring connectors with Belleville washers to provide even contact. We have run many thousands of these boards and never had one fail due to overcurrent.
Consider:
100A for industrial wiring is a #4 AWG. It has a area of 21.2 mm2.
So even if you divide the above by 4 (because the above is very conservative) you will have about 5mm2.
2 oz copper is approximately 0.07mm thick
you would need a trace 5/.07 = 72 mm
You might consider using copper bus bar on a insulating substrate. This way you can get thicknesses impossible with a PCB.
I will not say it is not doable. The folks above have covered that pretty well. But the safety margin is going to be difficult to maintain. In addition, the FEA thermal analysis it an estimate at best as the hardware is never as uniform as the analysis considers.
@Ashesh223 We don’t know your background and these comments aren’t to question your abilities but in a forum like this we must assume some caution when someone starts asking questions about circuits that can cause some serious harm or death.
Calculations like that are pretty much irrelevant.
Firstly those cables are usually round, and have a much smaller cross section to surface area, and it’s made much worse because they are usually wrapped in a thick layer of isolating plastic. Take for example the IRF3205 in a pretty standard TO220 housing. It’s apparently rated for 110A while it’s legs have a cross section of just 0.93*0.55 = 0.51 square millimeter. I would not trust it to push 100A through that FET, but it does show that such simple calculations are too far off to have much meaning.
I disagree:
I was not suggesting a design rule, I was trying to put what the OP was planning into some perspective they might better understand.
Remember physics applies everywhere, if any part of the clad reaches the glass transition point its pretty much on a path to failure.
You apparently didn’t read the notes on the IRF3205 (see below) and consider a typical TO-220 lead is only a couple of mm long before connecting to the board copper.
Either way, this really isn’t trivial and certainly isn’t something for a beginner.
Even though I have designed and tested “high current PCB’s” in the 100A range, it still scares me because there isn’t really a clear steps/equations
I didn’t want to go into details to keep the post short. But the 21 square mm compared to the 0.5 square millimeter of a TO220 leg is a very big difference.
But I think we can agree that designing a PCB that can handle 100A reliably is not a trivial matter.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
