This is the part where your homework comes into play… I suggest clicking every item in Kicad to see what they are and Hover over items and read the Tool-Tip…
(in previous posted, you indicated 70yrs. I’m several yrs older than that and still need to read and click to learn software…)
ADDED: Language-Syntax is a… (you choose the word). But, a ‘Mask’ implies covering up something, however, in the PCB world, a Mask, while covering-up the PCB requires an ‘Aperture’ to expose what’s underneath. Thus, to expose a Track for soldering wire to, you create an Aperture in the Mask…
This should help… I did not fuss with exactness of overlaying it onto the track
(and, you don’t need to do it away from the Track, simply Copy it, then, Hide the Cu layer and paste it, then do the rest of the work to make the aperture… Then, re-enable Track visibility)
Once it’s pasted over the Track, you can Right-Click it and use the Positioning Tools>Move Exactly
That will enable setting it cleanly… (may need to set the Grid to facilitate snapping accurately or, you can use the appropriate Key-Stroke while moving to avoid snapping, thus moving it in finite way…)… the homework…
I’m not suggesting doing this - just fooling around while drinking coffee… Quickly loaded the PCB into FreeCAD and made a Wire, then exported as STEP and made a Footprint in Kicad to use it…
Has nothing to do with making PCB, just a pretty picture without the solder (could have done the solder, too, but, coffee is gone…)
I solder wire onto track to increase cooling for some RF components. I cannot make the track wider as it is a stripline for impedance control. The board is ENIG finish.
Another possibility (unless you have a dense multilayer board where added through holes are a problem) is to add some through hole pads along the trace and solder wire “staple” jumpers into those pad holes. I would think that this might be advantageous, especially if the board is to be used in commercial production. I think the wires could be pre-cut and pre-bent. There would be less variability of exact location, and would not tend to disorient during assembly.
I have designed a few of my own two layer boards where I used jumpers like that instead of breaking up the ground plane on the bottom layer.
Looks correct.
I’d like to point out that in production, you really don’t want to do this. You are much better off using thicker copper (3oz+) or multiple layers to get the current handling you need. I designed a motor control board for a big winch that needs to handle over 100A, and it does it with only two layers of 3oz copper. The connections to the winch are studs that are pressed into the board, and then soldered for mechanical security. We have produced tens of thousands of these boards, and never had a failure due to over-current.
As you can see from Calculator tools, the width of the track must be approx. 4.7 mm and the thickness of copper 0.5 mm for 50Apms. How do you draw this in Kicad for the traces that must have this configuration so that the PCB manufacturer can see this?
I never use any of those Kicad-specific tools.
I just choose the required copper weight when i order boards, and upload Gerber files.
Much less chance of getting something wrong.
Note that it’s very, very expensive to have selective copper thickness on defined areas of a layer. Once you choose a copper weight, that entire layer will be uniformly that thickness. This means that you don’t want to have 6 oz copper on the same layer as a fine-pitched SMT part. If you need very heavy copper, move it to the inside, or the opposite board side from your fine-pitched parts.
I’d hate to be a traction motor driver layout guy… The 4oz copper is not compatible with fine pitch SMT etching.
I have solved it in the past with using a sandwich of 1 oz 2 layer sandwiched to a 4oz 2 layer to create a hybrid 1oz / 4oz board and it wasnt great.
During reflow is where the problems start due to warp . Not warp like warp field. Warp due to different copper weights generating different expansions . The bottom 1oz side had to have copper poured up to an inch of its life, and there needed to be copper pour cutouts on the thick side to control the expansion.
How much current goes though those wires?
How many PCB’s are you planning to make?
Another option is to use “bus bars”
Those bus bars come in many forms. I think there are some standard sizes you can buy off the shelf, but often these are custom products made to size. There are also variants made from a piece of copper wire and connectors you can screw on any location on the wire.
