I have to solder a couple wires to a PCB and I’m wondering which schematic symbol I should use to achieve this?
My first guess (BTW I’m using KiCAD 9) is to use a Mounting Hole Pad and then use a (assuming it’s plated through) a Mounting Hole Pad of appropriate size in the footprints?
Regards,
Dan
Just use a generic 1 pin or N pin connector. For the layout there are solder pads.
Yes, that would work, Footprints for mounting holes with pad are designed for accepting a screw though, and they are quite big. Another option is to use a footprint for a single pin header, or one of the “testpoint” footprints, or just roll your own. It takes a few hours at most to get familiar with how the footprint (and symbol) editors work, and then making custom footprints (or modifying them) becomes trivially simple.
One word of caution: when soldering multi stranded wire, there is a sharp transition between the flexible part and the soldered part, and bending forces at that point can easily lead to fatigue in the copper and thus wire breakages. There should always some sort of way to ensure that the wire is not being bent repeatedly at that point. KiCad has a “Connector_Wire” library with SolderWire footprints. Most of these have one or two NPT Holes in addition to a soldering pad. The Idea is to weave the insulated wire though the NPTH before a stripped part is soldered to the pad. The weave though the PCB ensures there is no stress on the solder joint or the transition from the soldered to the unsoldered part.
Edit: You probably forgot this yourself, but Hermit gave you pretty much the same answer to the same question 6 years ago. 
I’m a very new KiCAD 9 user, I haven’t proceeded to ordering a board yet but other than the strain-relief of a NPTH that paulvdh suggests, I was going to use a PTH via. With the proper hole diameter for the wire size and a pad big enough to solder. Are there any down sides to that idea?
Your Memory is better than mine! 
Paul has the uncanny (and always very helpful) knack of having the answers I need at his fingertips!
There was about a three second delay after I posted! 
Regards,
Dan
I went to Tour50-s profile to have a look at what sort of questions he asks, and that old topic was in the “Top Topics” list.
I’m self taught with no formal training or education so KiCAD can be a formidable opponent from time to time. The generous support I receive here makes a huge difference.
Many thanks,
Dan
What still puzzles me a bit is the Mounting Pad I posted. You can connect a wire to it?
Regards,
Dan
The mounting pad you show has a connection so you can join it to a GND net for exapmple.
Typically vias are covered by soldermask.
Wow - I might not have noticed that before ordering. Thanks!
Those “Connector_Wire” footprints impress me as a straightforward, but effective, solution to this problem. They use up a fair amount of acreage on the board, especially the two-hole versions. And the Assemblers will probably complain about threading the wires through the holes. I prefer to use pin headers in 0.1" (2.54mm) or 0.157" (4.0mm) pitch, but when there isn’t enough vertical clearance for the headers these wire attachment footprints would be ideal.
It’s always a compromise. The method definitely works, but a common reason for omitting connectors is a lack of space in the first place. Another reason is for cost reduction. And these footprints accomplish neither of these goals. The footprints are big, and threading though the holes cost a lot of time, which also costs money. In a production environment the wires are often stabilized by using some tie-wraps or by simply gluing the wire to the PCB.
You can also use two holes, but rotated 90 degrees and further from the solder connection, and then use a tie-wrap to sure a whole bundle of wires.
With (BLDC) motor controllers for moles (a.k.a. “ESC”, (electronic speed controller) thick, high amp (60A cont, few hundred A peak) are often soldered to an SMT pad, and then the whole thing is encapculated in shrink wrap.
Also common for mass production: Connectors also often have soldered wires (sometimes via an adapter PCB). and these have the exiting cable fixed to the housing.
Back when I was in college - and Mr Nixon was President - a certain instructor was fond of cynically reminding us,
A lot of engineering boils down to evaluating alternatives. For every solution, there is a problem.
I have used the wire-thru-hole strain relief idea a few times but I wasn’t aware that KiCAD included a family of pre-engineered footprints for it.
A conductor for 60A continuous must be about AWG 8. I can’t imagine soldering that directly to a PCB with ANY kind of strain relief technique that would prevent ripping the copper off a board when the wire was flexed.
It’s pretty common in BLDC / ESC motor controllers. Typically they have a lot of via’s through the pad for additional mechanical strength. Adding via’s to mechanical pads is also common for the mechanical pads of SMT connectors.
Source: https://www.reddit.com/r/PrintedCircuitBoard/comments/lxuc44/esc_pcb_design_review/
Another example is the cheap / chinese spot welders. These often have bus bars directly soldered to the PCB, and the thick wires soldered to the bus bars.
