So previously the experimental printheads have been constructed out of 2.54mm and 1.27mm perf board fiberglass PCB's. It was a very cheap build, but took a while to assemble correctly. While designing the two Driver and Controller boards, I pondered how difficult it would be to design a printhead out of a customized PCB stack that just bolts together.
Well, in the end it took me a week to bend KiACD to my wishes. KiCAD does not allow you to easily host more than one PCB design at a time, and I needed at least four of them. It would help if they where all in the same KiCAD project, because I could then move each PCB outline over another PCB and quickly make sure everything was aligning up correctly.
First off, I started with a Design Spark Mechanical CAD drawing of each layer:

- PCB Tank-cutaway-and-rivet.jpg (29.08 KiB) Viewed 538 times
I then could export each layer as a DFX file into KiCAD edge layer (this would come back to bite me later). It appeared to work well. There isn't much to the schematic diagram:

- Printhead-schematic_Gen3.1.jpg (31.27 KiB) Viewed 538 times
Funnily enough the nozzle filament connections gave me the biggest problem, as of course I had to make a customized footprint for them. It took a lot of different designs before I was happy with them.. Even at the end, I realized I hadn't included a solder mask opening. They are so tiny, that they looked ok in the KiCAD 3D viewer, but it wasn't until I upload the board into JLCPCB and the online Gerber viewer that I realized it just didn't look right.
I worked around the one-PCB-per-project in PCBNEW, via just deleting all but one PCB, then either exporting the STEP file (for viewing back in CAD), or the Gerbers. Then restoring the deleted parts, and repeating down the stack of PCB's. One of the last issues I had was that JLCPCB was reporting an incorrect minimum hole size in my designs. It took a while to sink in, but I realized that although I had imported the initial CAD DFX files into the KiCAD Edge layer, the holes would/could only be routed out, not drilled. Of course, you can't route out a 0.25mm edge based hole via current JLCPCB specifications. You need to drill those. We have a LOT of drill holes. This meant I had to first move each Edge based hole over to the KiACD Drawing layer, as I needed to know where to place the drill hole. I then added a drill hole object for each of the needed Printhead holes into the schematic:

- lots-of-drill-holes.jpg (24.13 KiB) Viewed 538 times
Then in PCBNEW, I had to manually and as accurately as I could, place each drill hole over each of the corresponding Drawing hole. The entire four layer PCB stack is put together with M2 bolts and the Nozzle plate can either be screwed on via M1.2 pan head screws, or bolted (countersunk head underneath), on via M1.2 bolts and nuts. Yes, I have picked up a range of M1, M1.2 and M2 bolts and nuts and hollow M3 brass rivets etc. It's amazing what you can find on Aliexpress.
Once all the PCB layer Gerbers had been exported, I could then import them into
Gerber Paneliser and build up a snap away Printhead:

- PCB-Panel.jpg (33.69 KiB) Viewed 538 times
These will come in at around A$6.89/Printhead - just add the filament, bolts, nuts, screws, tighten up together and your done. Well, there might need to be a bit more than that...