I have a schematic which i want to spiit into 3 pcb board. i will connect these boards with pin header and fpc cable. So i wonder to know is there a way that can do this when i generate gerber files, i can directly spiit them in 3 files ?
or can i draw in a pcb but with edge cuts line to split them in one geber file, the pcb factory can Identify it has 3 boards and produce 3 different boards?
You could separate the three parts of the board with edge cuts and ask the factory to do the cuts (which might require paying more, for different designs, and the cuts). When you get the board, you can separate by bending so that the board breaks at the cuts. Remember that edge cuts must be edge to edge; in other words, the cut cannot stop in the middle of the board; so the geometry of your boards is constrained.
Here’s an example by a well-known factory:
Search for V-cut and pcb mouse bites.
Both methods snap apart.
Remember, they will likely identify them as three separate designs and will charge for them individually - even if the whole board fits within their 10cm x 10cm ‘cheap rate’ size.
The Official viewpoint is that each KiCad Project is one PCB.
This may change in the future, but currently there is no work or testing done in this direction.
However, some time ago I did a small experiment in which KiCad projects were nested into each other, and it did seem to work.
This way you have a “global” project to work on a hierarchical schematic (So full ERC), and for the PCB’s, each PCB has it’s own KiCad project, which uses the schematic sheets from the “global” project. See:
2 Likes
could i just split the pcb into tree pcb file, then i will generate three geber files from three geber file?
yeah, they dentify them as three separate designs, so i may split the pcb in three pcb files.
Did you read my post about a “Multi PCB Project Idea”?
It is a combination of one “Master” project that sees the whole schematic, and sub projects for each PCB.
I’ve done this with hierarchy pages. I create new projects for each board and put them into separate folders. Because KiCad lets you use relative references I then make a new project that lives in the root directory and link the hierarchy page to each of the separate boards. This lets me connect everything together. When I do layout, I go to the sub folders and layout the board as normal.
this gives me separate boards for each and a primary project to keep references and so I can easily trace signals.
Here is a difference with my multi-pcb-experiment:
I put all the (sub) projects in the same directory.
This let me switch quickly between the projects by just double clicking on one of the project files in the KiCad Project Manager.
In case you had not noticed:
I attached the whole zipped experiment to that writeup I linked to earlier. That would be a quick way to check if this method works for you.
- For the system schematic diagram use ref des prefix (A1, A2, A3, etc) for the ref des of each part depending on which PCB the circuitry is on.
- When you are done with the system schematic copy it over three times (or how may PCBs you are going to have.
- For the A1 schematic delete all A2 and A3 ref des parts. Then delete the A1 ref des prefix from the parts on the A1 PCB. This will leave you with basic ref des.
- Repeat for the A2 and A3 schematic diagrams.
- You now have three projects or three separate PCBs.
–Larry
1 Like
This is also a solution, 
There is one way to do this but it is not supported and could introduce bugs, which require direct editing of the sch files to fix - so tread carefully.
What you do is separate your boards onto different hierarchical sheets and have sheet 1 be a table of contents linking to each board. If you have multiple sheets for one board they must be sheets of the board for the sheet you want. Make sure you annote so each sheet number is a precursor to the reference. so items on sheet three are 301, 302, 303, …
Then you create a project file for each PCB named the same as the master schematic page for each PCB and keep it all in the same folder. You design your large design using the nested table of contents project and then switch to each PCB project for making the PCB.
Warning… There be bugs in here: If you open the schematics while in different projects and change the annotation, your schematic file will save both annotations with different time codes and not change the annotation on the larger parent project. you then have to manually change it on both projects or go into the sch file in a text editor and delete the superfluous data. It also seems to happen at random and is hard to reproduce. Finally this is UNSUPPORTED so we are exploiting a bug to do this. Kicad developers could slam the gate shut on us at any moment to fix something else and lock out this functionality. As we are not using the program as intended there are no recourse, bug report options, etc. tread carefully and keep many backups.
Another bug you will have to deal with is the one that randomly reorders sheets of the schematic after re annotation. This is fixed by reordering the sheets and all their contents in the sch files using a text editor. Someone could write up a python script for this or something, but I just do it directly. You can find other pages on this bug that describe the solution in more detail. This bug is a real bug and has a bug report. It’s not just a problem for multiple board schematics - but any project with multiple sheets.
Good luck
Thanks for your patient reply, for this is not such a large design, so I just split the kicad_pcb into three files and send these gerbers to pcb factory with three orders.
1 Like
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.