Hi everyone, I am working on a project and now I don’t know how to design traces in Kicad that can handle 45 amperes, 30 amperes and 77 amperes. I was thinking about copper pour but I don’t know how to do that and I don’t know how much bigger a copper pour should be so that it can handle this amount of current. Also, the Kicad calculator is for a maximum current of 35 amperes but how can I calculate the trace width for the current higher than 35 amperes. Could you help me, please?
My first thought is, if you don’t know, then STOP! I’m mainly a hobbyist but those are some hefty currents and you MUST know what you are doing. 77 amps on a circuit board? Would you like to share a brief description of what you are trying to accomplish? Maybe someone can offer advice as to the best ways to accomplish what you want.
Just looked this up. 30mm copper trace for 77 amps with 4 ounce copper.
I am designing two circuits one that can provide up to 30 amperes and another one that can provide up to 45 amperes and then I want to connect these two outputs to a current sensor then to a screw terminal that provides up to 77 amperes
What circuit board components will you be using to handle these currents? (Link to data sheet) You can use a copper pour top and bottom and then drop in some vias to provide for some connection. @Rene_Poschl has some tutorials. Check the FAQ link. I don’t know for certain he provides pours but those would be your best bet.
Thank you so much for your advice. I will use Mosfets, inductors, capacitors, current sensors to build buck converters.
You will need a less-standard heavy copper, 2oz or even 4oz
The challenge is making connections at these currents to the copper, especially external connections
Davidsrsb, thank you for your advice. Why is it challenging making connections to the copper using screw terminals? Could you explain more?
This is doable but you need to take care in sizing aspects of this
Utilise available track calculators
NOTE: the vast majority of on-line calculators (as well as KiCAD built-in) uses IPC-2221 for the sizing. This isn’t accurate enough and you need a calculator which uses IPC-2152. SaturnPCB (or NinjaCalcs do).
Think about the current flow
If you put a odd shape down with suitable width but there are some tight corners, there will be very high current densities as the current tries to “turn the corner”. Keep the flow as straight as possible
IF you need to change layers, or use multple layers to share current, ensure you have suitably sized via’s an enough. This is a careful balancing act since the via’s will help share the current to other layers, they also remove copper from the present layer and thus reduce the contiguous copper available
Connections to the PCB.
There are multiple methods. I personally prefer the through-hole type from ERNI or the surface mount type from Wurth. Presently I have an M8 surface mount screw for 200A board I have.
always add more copper
Any numbers you calculate should be treated as a “sporty minimum”. If the calculators say 30mm wide, go high! go as high as you can, flood fill. Every time i have done such current carrying PCB’s there has always been more temprise than I anticipated but they have all worked out fine due to additional margin designed in
provision for external busbar
Sometimes you just can’t realise enough copper. There are external parts you can solder to the PCB to act as mini-busbars to remove the strain from the PCB
if you have access to it, consider using it. it is fantastic at visualising the current flow and permitting you to shift via’s to maximise the flow
Do not go above 6oz. Really don’t… it causes etching problems. take care what other parts you are putting onto the pcb with regards to etching. You can just about fit sot23-6 parts onto an etched 3oz card. if the copper weight is increased then the track clearances will fowl the sot23-6.
Speak to your fab house!!! Speak to your assembler. higher copper weights cause issues! make sure the card can be made, make sure your assembler can populate. Consider free-issuing a bare card to help your assembler profile the flow.
last but not least, ensure you have access to at least one bare card and literally test the temprise. Push the target current through the traces of interest (make sure suitable access tabs) and thermal couple the trace. IF you spot the temprise is too high under such testing you stand a chance of adding additional external busbar to mitigate the problem instead of waiting of the traces to delaminate off the card and suddenly open-circuit a charged inductor
Hi @Naib , thank you so much for your advice. Could you provide me the link to the calculator SaturnPCB? Do you have any tutorial for high current traces?
The challenge is the connection from the terminal to the copper. current densities can get very high
You can get 110A rating in a TO-220 MOSFET, but you will have real problems with the source lead connection
@davidsrsb thank you for your advice, I really appreciate it!!
An IPC-2152 based calculator
And a app note
Hi @davidsrsb thank you so much for your help, I really appreciate it!!!
NinjaPCB calc: https://ninja-calc.mbedded.ninja/tool/track-current-ipc-2152-calculator
Reference for high current: http://magazines007.com/pdf/HighPowerNotebook.pdf
There is a high voltage equiv available as well. This has some key point in there.
Totally agree!! I have some collegues at work that are still insisting on using TO-247 to make an inverter “because they can carry 100A+” and every time I keep pointing out to them how are they going to track away from the device with enough copper that the PCB doesn’t delaminate
This is partially why I like the multi-legged through-hole type terminals since they provide multiple places that inner layers can connect to and thus share the current. Its that interface where a plane meets the barrel that always scares me! a plated via is like… 100u thick at the point of contact and people expect all the current to go through that one face!
About (3), the vias. Rather than a big via, use several small vias. This reduces the indcuctance. And if your circuit is sensitive to inductance (example: if you want to switch a laser in a decent amount of time, say around 1 ns from 0 to full power), then don’t use vias if possible, and if impossible, use many of them in parallel as explained above.
Hi @Naib, thank you so much for providing the links and also for your help, I really appreciate it!!
The question of adequate copper width addresses a necessary condition but perhaps not a sufficient condition. (This is like saying that a good engine is needed to make a good car, but it is not sufficient. You also need a transmission and wheels, etc.) I design switching power converters, and I observe that minimizing stray inductance in critical locations (the “hot loops” and other places as well) will make the difference between a regulator which runs great and one which is garbage. For people have not done it, proper pcb layout is the most under-appreciated aspect of designing high frequency power converters.
Here is one of many links to check out:
Unless you know this stuff, I urge you to read up as much as you can regarding the proper pcb layout of your voltage converter. Two mm of avoidable component lead or trace length in the wrong place will make an observable difference and may cause a problem. The better MOSFET packages really pay off. The lead length>inductance of a D-pak can cause ringing and voltage spikes which will be greatly reduced in a MOSFET package similar to Infineon BSC or BSZ prefix device types. (I use these device number prefixes because other package designations get confusing as heck.)
Be very careful with this and your efforts will be rewarded.
As no one else has mentioned it, I’ll jump in. Much depends on if and how you are cooling the board. If you’ve got a fan blowing lots of known-cool air across the board, you can probably run a lot more current through your traces than you can if you’re relying on natural convection.
@JuliaTruchsess Thank you so much for your advice, I really appreciate it!!