Importing DXF to PCB new creating illegible blobs

[vulcanraven188]

Hi all,

New to Kicad here as we’re using different software at work now (using 4.0.6). I have a board outline made with DXF. I have to import the dxf into Kicad for board layout. When importing the DXF, it’s coming out as a blobby mess. Everything is too bold. It’s an annoying stressful thing. Hopefully it’s easy to solve. Any ideas?

[dchisholm]

You may be looking at the problems mentioned here:

Does anyone know how to set all the selected line widths in one go?

When I import DXF files the line width defaults to 2.54mm. On the OS X version I can only change the widths one line at a time, except for one time I selected the lines and an option appeared to set them all at once to the default width set in Preferences. I cannot find that option again. Does anyone know how to set all the selected line widths in one go?

I have imported *.DXF files into KiCAD a couple of times. There was always a fair amount of “fumble around until you find something that works”. KiCAD’s file importing capabilities seem to range from “crude” to “basic”. I am grateful that KiCAD can import at all but it’s still quite a bit short of importing “well”.

Two recent threads that touched on this subject are:

How to import PCB made in Inventor to PCBnew

As a part of a bigger project I have made PCB in Inventor. It shape and holes is hard to make in KiCad because of its complexity and needed precision. Is it possible to import Inventor file to PCBnew? If the answer is yes is there any step by step instructions how to do it? Software versions: Autodesk Inventor Professional 2016 KiCad 4.0.6

and

Pcbnew import coordinates from DXF file

Dear Kicad community. This is my first post, just saying ;). I am working with a graphic illustrating program, called CorelDraw, here I draw layouts for components placement, for pcbnew in Kicad. Currently I’m using a Github extension to convert the file, so that it is readable for Kicad(pcbnew). Afterwards I Import the layout and use a symbole as a reference, for the component placement In pcbnew. I manually place the components in pcbnew, based on the coordinates which I have from CorelDraw…

Here are some of the things I concluded in the course of my fumbling around with DXF. (My conclusions may be incorrect, but they seemed to be valid at the time, and I may not recall accurately, so don’t take these comments as the Definitive Truth.)

• The file needs to be saved in an older version of DXF. I think the DXF version from Autocad12 works well.

• The DXF file should use metric (millimeter) units.

• The no-charge version of CADStd (www.cadstd.com) seemed to produce DXF files that were easily imported.

• Did I define something like “Default Line Width” when I created the DXF file? I vaguely recall that, but not sure.

Dale

[vulcanraven188]

Thank you so much Dale, i will try these things at work tomorrow.

[cbernardo]

There are a few DXF formats supported by KiCad, though I can’t remember exactly which ones. To be safe, view the file in LibreCAD (or it’s parent qcad) and if there are no problems then KiCad can probably import it but there is no guarantee since the DXF library used by KiCad was forked out of LibreCAD so long ago.

The DXF units should not matter at all provided that the DXF file specifies the units. If units are not specified then they are interpreted as mm. In the first 4.x stable release things were worse - all files were interpreted as mm regardless of the actual unit. There is a small catch which probably doesn’t matter to anyone - if you specify parsecs (and a few other large units) then they will be interpreted as mm. The only other catch with DXF is that everything must be within a radius of about 1470mm of the origin or else there will be numeric overflow problems.

[cbernardo]

There may be a bug in the handling of default line widths if your units are not mm. Can you send me the DXF (cirilo /d o t/ bernardo at gmail com) so I can check? If the bug is what I suspect then the default linewidth being used may be 2.54mm rather than 0.1mm

[edit]

I’ve submitted a patch to the dev list for the development branch. Hopefully it won’t be too long before similar changes are made to stable.