Hi
Check if you have checked the compatibility constraints option in the import window.
Everything works for me.
Kacper Suchomski
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The AutoCAD drawing contains 'proxy objects' (things drawn using something other than "plain AutoCAD"). If you explode the object, you'll see it isn't drawn using continuous lines - so Inventor will struggle to make any sense of it.
In the attached copy of your drawing, you'll find a red polyline created in AutoCAD which follows the contour you are trying to follow. Note I didn't add the radii - the contour flange will do the bends for you based on your sheet metal rule.
If you are looking for shortcuts for getting AutoCAD profiles into Inventor, get to know the polyline command - it'll save you lots of time because it creates a single connected shape that Inventor loves. I'd also recommend 'bpoly' for creating a boundary polyline around a closed shape (like hatching, but without the hatch).
Second thing I'd recommend: Don't use Copy and Paste. Don't quote me, but I vaguely remember something about the Windows clipboard only being 16bit accuracy - and that kills some of the accuracy when pasting vector data between applications. In your drawing, I copied and pasted the polyline and found errors on the first dimension I added at the 4th decimal. Ok - it's not much, but the errors accumulate in more complex profiles.
Use either Import, or "Insert" when you're in a part file - then use the "Project DWG Geometry".
Both are slower than Ctrl+C Ctrl+V - but you will get better data in Inventor.
Hey, thank you very much. I didnt see this option. When I click "Import", I then chose the DWG file, then a plane, and that's it. maybe I am missing something?
When I click "Insert" I got this page:
is it relevant maybe?
Regarding "Import" - You click the plane for the sketch - and then it asks for a point. If the Inventor part file is empty, select the part origin point in the browser. Note that this this point represents the WCS 0,0,0 point in the AutoCAD drawing. So if you have a point on your sketch in AutoCAD that you would like placed on the origin in Inventor, move the sketch in AutoCAD.
Regarding the red polyline - this is how it works for me. Are you following a different workflow?
What you got in the AutoCAD file is not polyline. Part of it is polyline. Some of it is not:
Looks like import dimension is accurate:
The section looks like a long straight is in fact 3 lines and 2 arc.
Not connected.
Garbage in, garbage out.
Clean up the AutoCAD before import to Inventor.
Hi! I suggest you look into DWG Underlay workflow. You will need to start a new part -> Import -> pick the dwg file -> pick an origin plane -> pick the origin point. The dwg geometry will be linked to the Inventor part. Then create a 2D sketch on the origin plane -> Project DWG Geometry -> pick the dwg geometry. After that, the sketch can be used to create new features.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Hey. eventually I want to achieve that:
I got this ACAD from my colleague. So I measure the angles between the lines and the length of the lines and than sketch it by myself on a plane in Inventor, without including the bending, just straight lines. Then Contour Flange...
This process is easy but when it come to bunch of profiles and more complicated (though still quite simple) geometries, I wonder maybe I could just copy what already found in the ACAD, but it seems Inventor doesnt like it.
