Fill All Zones results are different in KCIAD 6 and KICAD 8.0.4

Layout
1

hi.
I am testing KICAD 8.0.4 using the KICAD Demo File.
The file saved in KICAD 6 was simply loaded into KICAD 8.0.4.

KICAD6 Fill
KICAD6 Fill1403Ă—965 94.6 KB

Kicad8 Fill
Kicad8 Fill1403Ă—965 84 KB

I simply ran Fill All zones with the B key.
The results generated in KICAD 6 and the results generated in KICAD 8 are different.
Are there any settings added in KICAD 8?
The OutLine Hatch Pitch area is displayed on the screen.

2

Are there any settings added in KICAD 8?

There was a behaviour change regarding the the clearance from zone copper to edge cuts (outline) clearance. This affects the clearing to the board outline as well as the clearance to all holes/cutouts in the middle of the board.:

  • v6: took the generic zone clearance setting for copper<–>edge.cuts distance
  • v7/v8: takes the value from board setup–>Design rules–>Constraints–>Copper–>Copper to Edge clearance.

Notes:

  • this constraint value is set to zero on opening a new project, so copper fill goes straight to the edge.cuts outline - linke in your picture. Bes ure to always set this clearnce setting to a reasonable value (>=0,2mm)
  • If you want individual clearances copper<–>edge.cuts you will have to work with custom rules
  • If you simply load the old designs (without refilling the zones) the old zone filling should be retained in v8
1 Like
3

I noticed this too, and regarded it as a bug. This is a dangerous setting because it can lead to faulty boards.During PCB manufacturing, zones extending to the edge of the PCB can cause shorts. Not only when metal (enclosure for example) touches the PCB, but also because the copper can get smeared around a bit during routing of the PCB.

I just had a look at this and:

  1. Renamed the whole configuration directory.
  2. Start KiCad. KiCad now assumes it is a fresh install and asks me whether to import settings or use defaults. I choose generate defaults.
  3. Create a dummy project, and then look in the above setting.

It was set to 0.5mm, which is a safe value for most designs.

I agree here, if import of an old design in KiCad results in a faulty board, then this should be reported on gitlab.

4

thank you
Well resolved.

5

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.