Edge 3d issue with arch

[gallegretto]

Hi, i have just moved from old stable version of Kicad to version 4.0…
It is very nice, I did a porting of my last project in very short time. I have just one issue I can’t fix. In the old project the board edge had rounded corners that I made with the arch function. When I visualize the 3D view I have a list of errors regarding the connections of the drawing…I did not have this problem with the old kicad. The 3D visualization shows just a rectangular board.

Any suggestion?

Thanks

G.

[madworm]

The board edge must be closed. It complains if the end-points of the segments are too far away from each other. This is best observed at high zoom levels & best fixed in openGL mode.

[gallegretto]

thanks for the answer but it looks like my segments are overlapping so there is continuity. it looks like the tool wants each segment to end in another… I don’t know I did not have the problem with the old version. I will chcek openGL as well…thanks

[gallegretto]

I did some more check using OpenGL view and the segments are very well overlapped.
I have also added segments on the joint to make sure there is continuity…but the result is the same…any suggestions?

[maui]

Hi,
the new pcb has less tolerance for board edges…
overlapping should be avoided, also considering the ability to export the board edge to 3D mechanical CAD through IDF export menu.
you may find useful this post

IDFV3 export bug

Hallo, I don’t know if this an application limit or a bug but when I try to export the board in IDFV3 format I obtain a file that’s not useable from other CAD to import (FreeCad or DesignSparck Mechanical). This problem arise often when I use round corners but sometime it worked with such features . The release of KiCAD I’m using is 6097 (64bit version) on a Windows 10 64bit PC. I’m a new user so I cannot upload images or files to further describe this issue. Best Regards

Maurice

[madworm]

The end-points MUST be very close (not more than 0.01mm) to each other. Simply overlapping the segments does not work.

[gallegretto]

It looks like segment start/end must be exactly the start/end of another. I spent a hour to do that and now it works. When I import a dxf with arches, I lose the arches but then I can recreate them knowing that the other segments are exactly placed. This way I can create arches with start and end points which are exactly matching the other segments connected. It is perfect but a bit heavy to do.

[Joan_Sparky]

@madworm

The end-points MUST be very close (not more than 0.01mm) to each other. Simply overlapping the segments does not work.

Best to start/end segments/arcs at the exact coordinates.

I’d first try to set a rough grid spacing… like 1mm or 0.5 mm and draw a simple rectangular outline and go from there… deleting/adding single segments/arcs as I go to keep it consistent, if you do your outlines in KiCAD (*)

*) alternatively you can draw up an outline in a CAD program of your choice that is able to export DXF, as the ability of KiCAD to do arbitrary arcs where start/end points meet other arcs/segments is very cumbersome. CAD programs have that one down as their main function
Naturally with simple 90deg arcs/segments you’d be faster in KiCAD still.

[cbernardo]

The segments must have ends which coincide. This is necessary because KiCad does not have geometry code to perform any trimming. Any seeming correct display in the past, given overlapping segments, was accidental. No overlapping - that’s bad geometry and is the reason kicad is getting confused; IDF export will also fail.

[maui]

Hi,
if you want to import dxf files with arcs and curves you have to follow some rules…
kicad can manage best dxf file if exported from LibreCAD in R12 version…
moreover it doesn’t support polyline

if you respect those rules, you can import very complex shapes

You may find these conversation useful:
http://www.mail-archive.com/kicad-developers@lists.launchpad.net/msg15228.html
http://www.mail-archive.com/kicad-developers@lists.launchpad.net/msg15217.html

Creating an elliptical PCB? [solved]

Thanks @cbernardo I think for the purposes of this one I’ll go with manually tracing it out with short straight segments drawn in OpenGL viewing mode. [image] The first time through there were several where the end vertices didn’t align, which meant the PCB outline wasn’t enclosed, but now I tracked down the culprits this is now sorted. With sufficient patience (and/or red wine) this manual process could be used for any complex shape, though after doing it I’m truly thankful most enclosures…

and the kicad user manual, obviously
http://docs.kicad.org/en/pcbnew.html
at the paragraph
‘6. Create and modify a board’
‘6.1.2. Using a DXF drawing for the board outline’