Before a send of an invalid board I want to make sure I understand the correct way to make a independent “through hole”.
I want a pad on both the front and back of the board, and both of these to be interconnected such that regardless of which side I solder a connecting wire the current is transmitted to associated traces on either side.
A via with no associated net serves this purpose does not have a schematic representation and it is not clear if the hole in the middle is filled. Simply putting a pad on both the front and back layer of the board does not imply interconnection. I have “stolen” a through hole from some stock throughhole components but do not see how they are interconnected.
If you select any PAD, and inspect Properties, under PadProperties.PadType, you fine 4 choices of plating/type. (thru-hole means drilled and plated, SMD means not drilled at all.)
There is a choice for NPTH (not plated thru hole) which generates into a separate drill file, and those holes have no electrical connection front to back. They are drilled last, after the board is plated.
Generally, because NPTH is a separate process step, it adds cost and is done only when really needed by the mechanical assembly.
In KiCad at least, the default assumption is that all holes are plated through, unless you specify NPTH.
Provided your hole has pads which meet the fab house minimum for “annular ring”, there should be no problem. I guess if you are soldering wires to it the pad size will be generous.
The KiCad library comes with solder wire footprints both in THT and SMD. (Found in the Connector_Wire library). Make sure you select the footprint to fit your wires diameter. The footprints available at the time of writing do not include protection against bending.
There is no special symbol for these in the library. The standard connector symbols might be a good option. (Most likely the Conn_01x01 symbol)
Explore the footprints in the “Connector_Wire” library to see if they meet your requirements.
I have a pull request open to even improve them further by having specialized footprints fitting typical (currently metric only) wire sizes. (They are scripted so adding sizes for AWG should not be too much trouble.)
On the topic of physical direct wire connects, one thing to be wary of, is the low strength of the copper plating. We have seen failures of high current wires, that bottom soldered but traced on the top side.
The physical stress of the stiff wire, fractures the plating, and the connection is unreliable.
A rule to have a fillet on both sides gives some mitigation, but is very operator dependent, and much slower to assemble.
Best solution is to either ensure bottom only routing connection (so you do not rely on plating) or add multiple vias, to give many paths, with no stress elements, to the top layer. that way, things still work, even if the wire hole does fracture.
For very high current, connector vendors offer multi-stake wire to board solutions.
All good points here and I appreciate the responses so I can move forward.
I have lost copper with soldered wires on occasion but I only use wiring points on my eval-boards and they usually are light gauge for signal traces. Anything production is connected via headers etc.
In the end it all depends on what the PCB fab does with your Gerbers.
For double sided PCB’s a common procedure is to start with a PCB which has 18um copper on both sides. One of the first steps is to drill all the holes. Then the inside of the holes is coated with a conductive material, which is just good enough to give electrolysis a chance of further plating.
In the next step the whole PCB (Often a square meter or so) is dipped into an electrolysis bath, where copper is added to anything that conducts on the PCB. Both faces are thickened to 35um, and the insides of the holes will then roughly be 35 - 18 = 17um.
Only then the mask for etching the tracks are applied and the PCB is etched.
If you’re curious about more of this then I recommend to watch some video’s about PCB fab’s. If I remember well, the ones from Euro Circuits are quite nice in details and also handle multi layer boards.
