Autocad 3D to Inventor assistance

[jeremy_wasserstrass]

I have a layout .dwg that I am trying to work with that has been draw as 3D. I exported as a .iges file and when I open the .iges in Inventor I find that I can only select vertices and edges and I can not constrain to faces. I am looking for help with my workflow in order to get the attached .dwg information as a usable reference in an assembly. The interesting thing is that if I upload the .iges to Fusion360 and export  a .stp I get garbage when the .stp is brought into Inventor.

[johnsonshiue]

Hi Jeremy,

The dwg geometry is non-uniformly scaled block reference. It is not true scaled. Also, the geometry is extremely far from the origin. Such geometry cannot be properly imported to a true-scale modeler like Inventor. I think you will be better off using AutoCAD to edit the geometry or create drawing views. You will need to rebuild the entire assembly in Inventor from scratch.

Many thanks!

[imajar · Accepted solution]

Wow, this one's a mess.  If you can request whoever made this to export it into a different format, do that.  Out of curiosity, do you know what program this was originally created in?

Otherwise, if you only need it only as a reference file, we can get it to Inventor. 

First:  Understanding the problems:

1) As @johnsonshiue  said, the geometry is too far from the origin to work in Inventor, so at a minimum you will need to move everything closer to the origin. (see attached .dwg file for an example).
2) All the geometry appears to be made from primitives and then scaled as blocks- I don't know how on earth this dwg was created, but I have never seen anything like it. Inventor does not appear to respect block scaling on Import, so you wont be able to import directly into Inventor. 
3) Some of the geometry in the dwg is 3d faces (which don't import to Inventor at all).
4) In my years of experience attempting to import dwg's into Inventor, my advice is to try to avoid it at all costs (I have had nothing but wasted time, sorrow and frustration using Inventor's dwg importer). If you have to, I have found fusion 360 to be much much better to import the dwg's and then export to Inventor.

Method 1: (better geometry, but loses 3d faces and lines)
1) move near the origin as in the attached dwg.
2) import the dwg directly into fusion 360. (This will not import 3d faces or lines, but does a pretty good job at everything else)
3) export as .sat (not step or Iges, they seem to inherit the block scaling or something weird- I cant explain) and open in Inventor. (or you could try exporting directly to Inventor).

Method 2: (Mesh geometry, which is less precise, but includes all the 3d faces)
1) move near the origin as in the attached dwg.
2) import the dwg into navisworks, export as fbx
3) import the fbx into fusion 360, use the "mesh to brep" command to convert all the mesh bodies to solid bodies.
4) export as step and import into Inventor

Method 3: (best of both worlds)
Use Method 1 to import just the autocad blocks and use method 2 to import the autocad 3d faces.

Good Luck.

[JDMather]

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@imajar wrote:

4) In my years of experience attempting to import dwg's into Inventor, my advice is to try to avoid it at all costs (I have had nothing but wasted time, sorrow and frustration using Inventor's dwg importer). 

I have no trouble importing the thousands of AutoCAD dwg solids that I have done into Inventor. The key is they were good quality solids when I created them in AutoCAD.  The GIGO principle applies (maybe that is GOGI?).

[jeremy_wasserstrass]

Thanks. When our electrical guys showed me this I originally thought cool this is going to make designing brackets a breeze. Instead the customer provided drawing is a mess that was giving odd results.

[imajar]

That's a fair point @JDMather.  I should clarify that all of the dwg files I import are generated by others - so I get all sorts of weird.

Often I import relatively large dwg's exported from other software (like Tekla, Revit, and so on), and I have spend alot of time working with my subs and suppliers to figure out ideal conversion settings and formats.  The end result of those countless hours of testing and importing is to avoid importing dwg's into Inventor if at all possible.

This thread is a perfect example of what I deal with all the time.  The dwg file at the beginning of this thread opens or imports correctly in less than 5 seconds using Autocad, Navisworks, 3ds Max, fusion 360 (30s) but I had to wait for 6 minutes for Inventor to import it, and the result was complete garbage.  I've had dwg files that Inventor took days to import, gotten incomplete results and had to use other software to preprocess the geometry before I could get it into Inventor.  It's frustrating.