I have a question regarding creation of a Rub-Out area. We are using a milling machine and our milling machine software accepts Gerbers and so theoretically, KiCAD can produce what is needed.
To explain the basics, we manufacture boards using a milling machine that performs isolation milling. That means, by default, the milling machine mills around each track creating an isolated track within the copper. All unused copper is by default left on the FR4.
Now our requirement is to remove/mill copper from certain areas to improve isolation. I could imagine two ways to achieve this:
Plot a filled area that respects the copper on layer B.Cu but creates the filled area on the Eco1.User layer.
Plot a filled area as normal on the B.Cu layer but then move the filled area to the Eco1.User layer.
As far as I know, neither options are supported or maybe I am too new to KiCAD and have not found the correct method.
It is quite easy to set the machine to remove all unused copper. But due to time consuming process, It is more convenient (if possible) to remove copper from a smaller defined area.
In that case you can use zones for your benefit. If you have for example a GND zone covering the board, you can use the “Remove islands: Never” option. Then it leaves the isolated copper areas there when you fill the zone. You can clean some area by adding a zone cutout (RMB menu → Zones → …) or by creating a keepout (rule) area.
KiCad makes a clear distinction between graphics and copper tracks and zones.
And KiCad can create gerber files for all layers, and in the gerber files such distinctions are not present anymore. In a Gerber file (except maybe the latest standards) it’s just all graphics. Flash codes and vectors.
Maybe it is an option for you to set KiCad to use 4 copper layers, and then use one of the internal layers as a GND zone with cutouts in them, and use the gerber file for that layer for milling. You would have to draw the contours manually. Clearances from other copper items are always generated dynamically and there is no real option to copy them to another layer.
Another option is to use a “Gerber Editor” to post-process the files generated by KiCad. Or, to make it complicated, you can probably plot to a .DXF or .SVG format, then post process the output in some external software, import the result again in KiCad as graphics and then create gerbers for your mill.
But in the end it’s mostly a limitation of your mill and the software with your milling machine, and this workflow is not part of a normal PCB design.
If you have some experience with scripting languages…
You could create zones in KiCad, assigned to a specially created net name (for example add a “test pin” with a single SMT pad to a net), and then extract that data from the KiCad file itself.
Yet another possibility:
In the selection filter in the lower right corner, delete everything from the PCB except your zone of interest:
Then generate a Gerber file from what is left over. Be sure to exit KiCad afterward without saving, or (safer) do this on a copy of your project. By default KiCad ge-generates zone-boundaries during Gerber creation, but this step can be skipped.
Hi,
Thanks for the response. I don’t fully agree but I am grateful for the response in any case.
The software for the milling machine allows me to plot any gerber file as a Track (signal), cutout, rubout etc. So if I was able to create a filled area and then move this to an independent layer (i.e. a layer that does not include tracks) I could then plot this and instruct the milling software that this is a rub-out layer.
I have searched a lot regarding this issue and I very often read the statement, “This is not a normal PCB manufacturing process”. And to be honest, I agree to an extent. However, it is still a valid requirement to move PCB objects between layers. Post processing is also possible, but then what we see in KiCAD is not a true representation of what will be produced. Not ideal but not a show stopper I guess.
By trade, I am a software developer and I would therefore assume adding the abilty to move something from one layer to another is quite trivial. But I do understand if there is not a large enough demand, this wil never get focus.
It is quite easy to move copper tracks from one layer to another in KiCad By first selecting them, and then editing their properties and change the layer.
There is a similar settings for zones. Each zone can be present on multiple copper layers. But it is just the zone boundaries that are then also present on those other layers. In KiCad, the internal geometry and clearance calculations are always done by KiCad itself. This is enough for normal PCB production.
