Hi My PCB manufacturer in China likes boards butted up for panelising, and then v-scores along the profile (JLCPBC). My European manufacturer (multi-cb in Germany) likes a 2.4mm router gap and leaves bridges.
In the past I have saved a copy of the board to another filename like multi_board, then done repeated block copies and it is easy if you have a few simple rules like the edge is on 1mm grid or similar.
In the latest issue V 4.07 if find that whatever I do to the copy gets done on the original as well, even if it is in a completely separate folder so I finish with effectively 2 copies of the multiple board. Also “Append Board” command is always greyed out.
Another minor issue is that sometimes the front silk text (entered as text) does not copy.
Not sure if these are intended behaviour or just me.
Weird! Today the problem seems to have gone away. I have successfully copied a test board in the same project folder, and it is fine. Maybe I was rushing a bit yesterday!
The “Append Board” function is still greyed out though.
This feature is only available in standalone mode. (The devs consider it a dangerous feature. I seem to remember that the main reason for not allowing it in normal mode is lack of proper testing.)
Not at all. They have thought about it, and a lot.
There is a one-to-one relation between the schematic and the layout components. If you select a pcbnew footprint, its matching component is selected in eeschema and the other way round.
An imported layout into another project makes everything blow up.
I don’t mean to be rude but I still think it’s a bad idea: a menu (in this case File menu) CANNOT change dynamically. It should at least be greyed out and explaining why when hoovering. But it’s not like Kicad devs are considering the User anyway, with all the mouse wraps and focus stealing.
Furthermore importing layout don’t blow everything: I use it daily to copy board contour or mechanical fitting.
Of course, you can think it is a bad idea and not be rude for so. I was trying to explain one of the reasons of why the devs discarded the append board option into a project.
Importing a board edge or mechanical holes doesn’t blow up anything. But footprints with the same references are candidates to make the application fail. And usually we have a reference, for example “U1” in every circuit we design.
With a project I meant schematic+netlist+layout, not a stand alone layout.
You guys should be using a DXF master for this kind of workflow IMHO.
Mechanical design is not one of KiCADs strong sides and if you do designs that are based on the same mechanical constraints a lot you should have a CAD model in another tool anyway, which would be the source for the master DXF that you need.
As for PCBnew not showing the import option when in connected mode… well, if you need it badly, get in touch with the devs or even better become one yourself - I know, easier said than done
We can’t do much about it here really.
Afai-remember there was talk about EEschema needing a lot of work for it to be able to handle ‘modules’, i.e. repetitive circuits or similar stuff, before they could even think about using it in PCBnew.
Well get there someday, but it won’t be next year.
Further than just some practical cases, I think the point of this thread was to figure out an easy way (think “user”!) for being able to panelize boards.
There is no panelization tool (pcb or Gerber level) supplied with KiCAD, therefore pcbnew is the only alternative.
Would you have documentation on the “suggested way” of doing this with the actual implementation?
Though that doesn’t stop us from discussing a more user-friendly solution for KiCAD 6?
It depends on what you mean by panelization.
If you mean adding different circuits in the same panel, use the pcbnew stand-alone version.
If you mean replicating the same circuit many times, use the Create array tool.
I wrote a short private message for somebody last month about panelization. I’ll post it here. It just uses PCBNEW and manual labor; no fancy scripts or coding. My apologies if it seems basic and obvious.
I open the PCB directly in PCBNEW and then use the “Append Board…” command to bring in additional copies of the PCB (or of other PCBs). I space the boards with at least 0.1" between them (for router bit clearance). Then I add a bunch of mousebite tab footprints I have to the PCB outlines and join the PCBs. JLCPCB will route-out the slots and leave the individual boards connected to each other with the tabs. Then I just break the boards apart.
