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
the easiest way is through DXF import in KiCad
http://docs.kicad.org/4.0.6/en/pcbnew.html#_creating_a_board
6.1.2. Using a DXF drawing for the board outline
Thanks, but Inventor does not have option to export to DXF.
draw the pcb as sheetmetal (or convert it into one)
flatten the part
.
flip the facing side (if needed) - menu accessible via right-clicking on flat-pattern definition in object-tree
.
export flat-pattern as dxf (AutoCAD 2004 format works, use out-of-the-box/standard settings for all options afai-remember)
.
Import into KiCAD/PCBnew is a bit bumpy though, as you don’t get to chose exactly where it lands.
Best advice I can give is to work from the imported dxf outline and import the netlist and do the layout afterwards.
If you need to change the outline, redo it in Inventor, export it again and import it again.
You don’t want to move it around in KiCAD really.
Find a combination of options/values that drop it off conveniently in the PCBnew editor and remember those settings for that project - yes, been there & not done that. Get’s really frustrating after the 4th time of changing the outline and needing to nudge it a couple um after importing each and every time as the selection and move is a bit awkward 
PS: the same workflow applies if you want your sheet-metal cut by a lasercutting company.
Just talk with the laser estimators when you do it… mine want’s the drill centers not in the dxf file (tool centers), as they have to remove them manually.
This is my standard dxf export setting in Inventor:
Yeah, importing the outline really needs to be the foundation on which you start your work.
The import seems to work smoothest with the OpenGL canvas. Regardless of whether you check “Inch” or “Millimeters”, KiCAD is going to interpret the imported DXF values as millimeters. The no-charge version of “CADStd” can read a DXF file expressed in various unit systems, then write the same file in millimeters. (Other programs can probably do the same, but I haven’t found them yet.)
Strip the unused layers, notes, format boundary, etc, out of the DXF before you try to import it.
The imported DXF image will arrive in the KiCAD OpenGL canvas “attached” to the mouse cursor. I haven’t figured out how it decides where the attachment point should be. You can move the cursor around, pan and zoom, to position the imported image to the location where you want it. Once positioned, a click will park the image.
Before importing, you can place some reference markers (outlines, crosshairs, circles, etc) on a spare KiCAD layer to mark the desired locations of salient features in the outline (edges, mounting holes, cutouts, etc). Then you can align the imported image with your markers. With luck and a steady hand on the mouse I can place the imported image within a few mils (about 0.05mm) of my reference points.
After parking the imported image it may be practical to select the entire image and adjust its location using the “Move Exactly” tool. This lets you position the imported outline to an arbitrary precision.
Dale
Ugh… that’s bad. Who thought of that?
The Legacy Canvas drops it and it’s there.
The whole import dialog box with positions is useless then for OpenGL…
Alternative approaches would include trying:
which allows a DXF to be converted into either a gEDA PCB compatible footprint (which kicad can load), or a gEDA PCB layout, which the PCB fork pcb-rnd can export as a kicad layout.
I have not tried dxf2pcb myself, as I have not had the need arise to date.
Alternatively, if you can load the dxf into inkscape, you may be able to export it to a gEDA PCB compatible footprint you can use with an inkscape extension (beta) script like
but I don’t know how the exactitude of your measurements will change during conversion of the paths during the multiple dxf->svg->linear element conversion stages; although scaling (in DPI) can be tweaked during export from Inkscape, there will probably be some rounding.
Best of luck in your quest.
Erich.
the same in GAL … just don’t move the mouse and click ENTER and the DXF path is were the dialog says… if you move the mouse you can drag the DXF wherever you want
