I’m currently working on designing a power distribution board to accommodate up to four ESC controllers, each drawing a continuous current of 40 A (totaling 160 A) from a single LiPo battery. Additionally, this board will power a control board with a maximum draw of approximately 50 W.
My primary concern is determining the appropriate copper pour for the power plane to support such a significant current load.
How can I determine the optimal copper pour or width to meet such a high amp requirement?
Is there a general rule of thumb for correlating copper thickness (oz) with maximum amperage for a given board width? Or is this typically determined through experimentation and testing?
I highly advise reviewing IPC 2152. Within that specification, you’ll discover numerous examples demonstrating how to estimate the width and thickness of a copper plane by considering temperature rise and environmental conditions of the PCB. Additionally, there are calculators aligned with IPC standards that can aid you in this process.
Because ground pours (and sometimes even planes) have irregular shapes it’s close to impossible to predict much in detail. So in that case you need to find the smallest cross-sectional area that your current will be passing through… Then, knowing the cross-sectional area and current you can calculate temp rise and voltage drops. The best collection of data is probably in IPC-2152. With over 100 graphs and tables it’s probably the most complete source. It’s either that or go back to Onderdonk’s work.
You can use Saturn PCB toolkit to calculate current capacity of trace width. For higher current, width would be high( couple inchs). This calc is as per IPC-2152 I believe. This is what your copper pour will be. If there is space limitation, you can go to 4 or 6 layers and have same copper pour in those layers as well. Stitch them with enough no of vias to support current transfer. You can also use 2Oz copper on top and 1 Oz on internal layers.
If at any point your copper pour reduces in size then that will be your limitation so make sure your calculated width is the minimum copper pour size.
Sierra also has this tool: Trace Width, Current and Temp Rise Calculator | Sierra Circuits
Have you tried it, @ronak.sakaria ? Let me know what you think.
I have designed PCBs that can support up to 500A and put them into production, I agree with the suggestion to use Saturn PCB toolkit or other standard trace width calculations as a starting point. In practice, this part of PCB design seems to be more art than science. The standard solution is to avoid high current PCBs. You can decrease current by increasing voltage. Or you can move the current off the PCB onto busbars, external relays, external solid state switches, etc… If you are determined to have a high current PCB, learn from my mistakes and build test PCBs, then thoroughly load test at expected temperatures them before committing to a production design.