As Bertrand already mentioned. You draw the lines for the bayonet hole on the Edge.Cuts layer in the footprint itself. This way the pads will always have the correct relative position to the hole and you can move the whole footprint in the PCB editor. When the bayonet hole is part of the footprint, you also draw it once, and then just insert multiple instances of the footprint on your PCB.
Also, there is no need to exactly replicate the track layout. Once you have the schematic and the footprints set up, and also created / adjusted a net class (which defines clearances and default track widths) you can simply draw tracks (KiCad knows in between which pads you have to draw tracks, and shows this with ratsnest lines on the PCB) and KiCad applies the rules in the net class for track width and clearance. This is one of the main reasons for having a schematic. With the schematic and thus also the netlist, KiCad can help you with which connections to make.
On a flex PCB, you also want to avoid all corners and sudden width changes. Anything that can cause a stress concentration should be avoided. KiCad can help here with filleted corners and teardrops.
Fantastic - that sounds perfect. I wasn’t sure whether Edge.Cuts layer detail would carry forward.
How do we ensure the generated routing doesn’t go over any large holes (such as the cutout for the speedometer)? Can I exclude regions of the board, or does making a shape in Edge.Cuts do that automatically?
The original board has large sections of copper, for example, like this:
The original layout is clearly hand drawn. Made with today’s software it would look very different. We can guess that those details don’t matter much, but if you’re not sure you IMO should copy it exactly graphically, which requires different strategy (either converting the image to graphics to the board, or roughly following the area edges with hand drawn polygons/zones).
KiCad automatically keeps a clearance between copper tracks and Edge.Cuts lines. KiCad does not route tracks over Edge.Cuts. There are also various things you can do with keep out area’s (Zones), but that is not needed here.
For the wide copper. I am not sure. My best guess is they want to “balance” the ratio of copper to bare flex and keep this ratio approximately uniform across the whole PCB, with the goal to prevent warping during production.
Also, copper features are made by selectively etching away some part from a half fabricate fully covered in copper, and this uses up the etchant (acid). By etching away less copper they can save a very minuscule amount of money, but it may be just important enough when making a few million cars for a PCB designer to spend an hour extra on the project.
Are there any parts that might rub against the flexi? The resist on top of the copper is no a reliable insulator.
Those holes look like they were for some sort of locating peg.
Paul, I must tell you again how grateful I am for the detail you go into. You’ve helped me so much already. I learned a ton and am very much enjoying working with KiCAD.
Other than a tangle of British automotive wiring from the 1970s, it’s pretty clear behind the instruments, and I don’t think it’s likely to rub against any metal parts.
Little metal clips hold the instruments in. For example, this is the front (instrument) side of the fuel gauge. There are three holes for three pins on the back of the gauge.
This is the back (circuit board) side of the console. The metal clips come through the plastic and the circuit board and are bent and screwed onto the PCB.
This is the back of the fuel gauge. To the right is one of the three metal clips that are bent back onto the PCB to make electrical contact. The front of the gauge is held in place by two screws.
Yes, that was exactly what I initially felt. I’m not sure. I started by tracing the original tracks using the place polygon tool.
It seems like the other person (@Toggesh) applied a similar approach for his old French car, which seemed to work out well for him.
However, I’m slowly coming around to the approach @paulvdh advocates. The large copper areas are likely due to the board’s mechanical properties or fabrication limitations, which probably won’t apply in my case. I like the idea of doing it properly, as it will mean I can evolve and customize the design.
Cutouts were created using polygons by tracing the contours of a circle and rectangle on a User layer.
Somehow, I made through-hole pads for the illumination lamp but SMD for the warning lamp. I changed this to SMD on both - since I don’t want a hole. Is that correct?
THT pads are yellow, have a hole and exist on all copper layers, while SMT pads don’t have a hole and have only one copper layer, and their color is the same as the color for the copper layer they are on. If you put an SMT pad on the bottom it turns (by default) blue, because the back side of the PCB has blue for the copper layer. Using SMT pads is correct here. You don’t want the hole, and you only want pads on one side.
You probably also want to round these corners:
Sharp inner corners are stress riser points and they can very easily be the locations where cracks start to appear. I’m not sure for flex cable, but both for regular FR4 PCB’s and solder stencils sharp internal corners are a manufacturing problem. For the PCB, the manufacturers often silenty just round it (because of the diameter of the routing bit used. For stencils, you also have a minimum radius which depends on manufacturing method (for example the diameter of the laser used). It is also part of the reason IPC recommends rounded corners for pads. This makes the stencil apertures less dependent on the manufacturing method, (and it helps with solder paste release). But this is a side line. Only for flex PCB’s is the stress riser corners an issue, but it is an important issue. If you look closely at your original flex, these corners will also have a radius in them. The easiest way to draw them in KiCad is to select the lines, then right click and then from the context menu select: Shape Modification / Fillet Lines. This option may be missing if any arcs are already part of the selection.
I would have probably made them a bit bigger myself.
On the other hand, The flex is held firmly in place by the connected light bulbs in those places, so the holes and their corners don’t experience any flex at all, and this greatly reduces the importance of this issue. When there is no movement, there are also no fatigue cracks. So your 0.2mm will probably be just fine.
