Not a closed polygon

Hi, DRC complains about an unclosed polygon. Where can I set the tolerance for assuming closedness having in mind that sin/cosine values are irrational numbers in general :slight_smile:

Thank you
Cheers
Detlef

Best I know is there is a small fixed tolerance.
Internally KiCad coordinates are 32 bit integers on a nanometer grid.

I find it quite easy to just snap end points together. When a magnetic snap point is found, KiCad shows a small circle around it:
image

If snapping to graphics does not work, then have a look at: Pcbnew / Preferences / Preferences / Pcbnew / Magnetic Points

KiCad is not a mechanical CAD package, but drawing an outline from some lines and arcs is usually quite easy. I normally also draw outlines on a coarse 1mm grid which further simplifies it.

If you have a complex PCB outline, then it is a better option to draw it in a mechanical CAD program, export it as a .DXF file and then import it in KiCad.

2 Likes

5.1 doesn’t have a tolerance at all – so you need to use snaps as suggested by Paul.

6.0 does have a tolerance. It’s currently hard-coded at 0.02mm.

I find it a bit confusing which KiCad Version does what sometimes…
So I made a little test project in V5.1.10.
Made a square PCB of 20x20mm and then moved the horizontal upper line on Edge.Cuts a bit until I got the “Board outline does not form a closed polygon” error, and then moved it back until the error went away. Apparently a deviation of 5um is accepted without complaining, and 6um results in and DRC error.

2021-06-08_asdf_PCB_Outline.zip (3.4 KB)

Hi, worked with the magnetic snaps, THX.
The small circle that popped up was very helpful.

The outline is composed of arcs. It was very difficult to choose center and start so that the endpoint hits the given coordinate. I had to tie together with short lines :expressionless: . Choosing center as the last parameter of an arc had come in much more convenient.

But no more complaints from DRC regarding that issue (only 136 left on others :)) )

THX
Cheers
Detlef

If you select the arc, then 3 little squares appear, and you can drag them to other coordinates. You can also press e to edit the properties of the arc and type in some numbers directly.
image

The problem is that an arc is defined by the center and one of the endpoints. You can’t set the coordinates for both endpoints and the radius. Moving from an endpoint causes the other end to become unconnected. Click+dragging does two different things depending on which end is used: it either alters the radius or lengthens the arc. Using arcs is KiCad is difficult in some situations.

1 Like

Use a bigger raster “ex. 0.5mm” for this job. This avoid most problems. Switch to a smaller raster for routing afterwards.

The arc definition has also been fixed for 6.0.

2 Likes