Multiple filled zones with rounded corners make file size large. Tips to decrease it?

[pab44]

I am working on a pcb design that requires multiple zones be filled and have rounded corners.

I am using python scripting to place & fill zones, and fillet method to round corners.

What can I do to decrease the file size for gerbers and pcbnew?
The filled zones make up most of the file size.

Any advice?

Edit:
I am using KiCad 5.1.4 release build.

[eelik]

Can you show an example, a screenshot maybe?

[pab44]

It is just hundreds of zones in the shape of a rhombus with corners rounded and zones filled.

[eelik]

In v5, hardly. In the development version (nightly builds, 5.99) there’s new zone fill strategy in Board Setup -> Constraints. Based on my simple experiment it may cut the size of a zone in the generated gerber file to half, although the kicad file stays the same.

It’s impossible to reduce the size of a zone in the kicad pcb file - it must describe the polygon corners in any case. In the v5 filling method KiCad draws lines around the fill edge. In the new filling method it’ just a polygon (rounded corners made with short edges and more corners, like in the old method). I think it affects both KiCad view rendering and exported file generation.

A fillet corner in the gerber with the old method:

And with the new method:

[twl]

@pab44

What can I do to decrease the file size for gerbers and pcbnew?

If you can migrate to the V6 nightlies:

File->Board Setup->Zone Fill Strategy->set to smoothed polygons
File->Board Setup->Arc/circle drawing maximum deviation: increase the value. This is the maximum arc approximation error. More means more jagged polygons, but smaller files.

Tom

[eelik]

If you can live with non-rounded corners, it’s the fillets which require data in the pcb file. Even changing to chamfer saves quite much. That’s because of “filled polygon” is kept in the file, not just the basic polygon.

[pab44]

Thank you @eelik and @twl, I will try those suggestions.