Imported dxf graphic looks fine in the layout but is missing in 3D view. Is anyone else having this problem?
Version: 7.0.8-7.0.8~ubuntu22.04.1, release build
Did you import to a layer that is not shown on the 3D view ?
No, it is on the F.silkscreen and looks fine on the layout page. It is only in the 3D view that it isn’t displayed.
Basically, although Graphics can be loaded and look okay in PCB editor and schematic, their ability for the 3D-Viewer is more about their ability to be used in PCB mfg. Thus, they can be used with limitation’s in mind.
Therefore:
• Basically, PNG’s can be used by the Image Converter Tool to make Footprint and Symbol.
• DXF can be loaded directly into PCB and used for various non-colored/greyscale purposes.
Example shows:
• Squiggle-Lines, Treble-Clef and Note from PNG used in the Image Converter Tool to make footprints
• Image of Face (see info in screenshot)
And, set the Pref’s as needed…
Thanks BlackCoffee. It would be useful to see all silkscreen on the PCB also in the 3D view as a check that it presents as desired but I understand that the 3D view has limitations.
If your graphic is amenable to being a 3D-shape (such as in a Logo) and want Colors, you can build a 3D Step model and create a footprint.
Example shows one extruded 0.1mm… (done in FreeCAD). It’s no different than any Footprint with a colored step file.
Imported dxf graphic looks fine in the layout but is missing in 3D view. Is anyone else having this problem?
Just checked with a example dxf: imported onto the pcb (onto the silkscreen layer), and is displayed on the 3D-viewer. So in principle a imported dxf-graphic should be visible in the 3D-viewer.
(tested with v7.0.8 on Win10)
Could you attach that specific board with the non-displayed dxf-graphic?
thought I was clear about that…
Apparently it is . . .
Apparently the DXF file is not understood by the 3D render yet was understood by pcbnew. I selected a different DXF (not the one that I wanted) and it shows up in both 3D render and pcbnew.
I had only “Show Silkscreen layers” checked. I just checked it and the two subordinate “clip” boxes and rendering is the same.
Please submit a bug report and attach the DXF file that cannot be rendered. This is a bug imo.
Or a badly formed DXF . . .
When I export DXF from Solidworks and then import I get two sets of the same lines/curves overlaid. I have to select each section one by one and delete the duplicate. I’m probably doing something wrong when I export . . . but I need to do this so infrequently that my workaround isn’t much of an issue.
One thing that may be a bug, I specify the line width when I import and this seems to be ignored. If I ever get time I’ll try and check it again to be sure.
Apparently the DXF file is not understood by the 3D render yet was understood by pcbnew
Unlikely. During the import-process the dxf is converted into simple lines+circles+arcs and after that no longer exists as “dxf” inside kicad. To investigate further we would need the zipped archived project (with dxf already imported into the board) which doesn’t show the graphic in the 3D-view. Additionally it would be good to include the original dxf file in the zip-archive.
One thing that may be a bug, I specify the line width when I import and this seems to be ignored.
The specified line-width in the import dialog is named “Default line width” and is only used if the dxf file itself doesn’t specify a linewidth. Every width-specification in the dxf-file supersedes the “Default line width”-value.
1 Like
I submitted a bug report.
1 Like
Your problem appears to be the Scale… If I import your file at scale = 25.4, it shows as below screenshot. Be sure to check your units…
Your scaling made it usable. After I reported the bug this was posted as a comment:
Maik Freitag
@mf_ibfeew
· 1 hour ago
Reporter
This is not a problem with the dxf in principle. The problem is the linewidth of the graphic items: the linewidth in the dxf is set to 0.000018mm == 18nm. Such a thin silkscreen line is not produceable in reality. And in the 3D-viewer the line starts to slowly fade away if the width drops below 0,001m== 1um. At 18nm the line is swallowed by the surrounding green pcb.
So, the problem DXF file had a much too small line width. Apparently pcbnew scales the linewidth up to something usable while 3DView renders at the DXF’s impossible 1um. The bug report is marked :Priority: undecided". Apparently they are thinking the same thing that I am, namely that pcbnew and 3D View should behave the same.
2 Likes
My simple-minded thinking suggests it’s all about your Scale. As shown in my post, I placed a dimension (after importing). The dimension is 39.37. If Unscaled, (39.37/25.4) = 1.55. Pretty darn small for a Logo…
Also, I opened it in FreeCAD and grabbed two points to measure - screenshot below confirms tiny logo (it’s smaller than 1.55 because I didn’t grab boarder’s)
Here I imported it in millimeters and put it next to a 0603 resistor.
Quite small indeed.
And when zooming, the PCB editor renders the lines with a minimum width of 1 pixel on screen, and at maximum zoom the linewidth increases to 4 pixels. When I import the image with units as “feet”, then the letters are quite big, but the linewidth stays the same. Still 4 pixels at maximum zoom level. 