I was looking at making a PCB which is going to be used as a power bus to connect multiple DC stepper motors for a dispensing solution similar to the Ultimaker 3D printer whose schematics and layout can be found here . The stepper motors are going to be running on the xyz axis and there will also be other peripherals powered from the same power source.
The power input is going to be around 220W at full capacity and I have no clue how to begin designing for such a board with a high current input. Is there a guide or some information I can find useful being someone who is just starting to design high power boards??
For a PCB, the amount of copper determines the amount of current, and the clearance around the copper determines the maximum voltage.
For steppermotors, voltage is likely below 100V and hardly a concern, so that leaves the current.
I assume something like 24V @ 10A total.
Stepper motors usually use much less current then their specifications suggest. The inductors in the motor themselves act as a buck converter, so even if you have a 2A motor (coil) current, the current from you power supply likely is closer to 500mA. (Unless when the motor rotates fast).
10A is enough to heat up bad connections to a point that it can become a fire hazard, or the PCB may get damaged, so you want to use decent quality connectors.
Concentration of the current is an issue. Ideally you use both side of the PCB and stitch them together with via’s in area’s where the current is concentrated in a small area, for example near the power connector.
Location of the power connector is an important decision.
Take for example a 30cm wide PCB with the power connector in the left side (Conductors are 30cm long and carry the full current), and compare that with the power connector in the middle. (Conductors are only 15cm long and half the current goes left, and the other half to the right. That is a factor of 4 improvement for the voltage loss over the PCB.
Stepper motor drivers work as SMPS circuits. You want decent size decoupling capacitors (470uF maybe bigger) and put them close to the stepper motor drivers. All the regular concerns for SMPS circuits apply (research “hot loop”)
KiCad has a built-in calculator for voltage loss over copper tracks (Rightmost icon in the project manager) That can give you a fair idea of what track widths yo should use. 10A is not exceptional though. For 10A you can even use regular (35um) copper thickness, and even then a 10mm wide track can handle that current safely. Wider tracks do lower the resistance and power loss though.
I have taken into consideration the decoupling capacitors and the thermal vias/copper pours shown in the image above.
Would I be using the same precautions but instead would widen the traces, size up the passive electronics, and add more layers or copper thickness to accommodate for the larger power rating??
Would a 2 layer board with 1oz copper weight and 1.6mm thickness be enough for my new design??
If you are using a double sided board, there is an OSH Park PCB that uses 2 oz. copper. The board is thinner- about .032" which may affect mounting holes. support for screw terminals, etc.
I prototyped a 4 layer PCB with OSH Park, then when it went to production had the board made with 2 oz copper on the top and bottom layers. The efficient went up by 2%.
At the high current level, taking a signal to another layer requires a bit more though. I used vias with larger holes, and on some made a one pad “part” so there would be no silkscreen covering it so I could fill it with solder.
Finally, if you have a good meter (4.5 to 6.5 digits), or scope, measure the drop on key runs and figure out how much is being dissipated by the board itself.
I was under the impression Kicad could import an Altium board, which I think your link has the Altium design file.
Your link shows a 4 layer board, typically only the outer layers can be 2 oz copper. You should first see if you can simply import that board. Then find the high current paths to determine how to handle those currents.