What's the best file extension to import from Inventor into Fusion 360 V2017

[Anonymous]

I am very new to Fusion 360 so here goes:

I'm trying to import a simple door and frame into Fusion from Inventor 2017. I exported as a .stl file and brought it into Fusion. Once open in Fusion, I cannot separate the door from the handle and frame to assign it different colors. If i assign one color, the whole door assembly turns into that color. What am I doing wrong? Also, what's with the diagonal lines from the corners leading to the handle? In ShowCase, you were able to separate parts/faces to assign different colors to different surfaces. Any help is appreciated.

[lichtzeichenanlage]

I'm a beginner, but whenever I heard something about good import formats it was *.STP / *.STEP / *.STE files

[ToddHarris7556]

We use both Inventor and Fusion every day as part of our workflow.

The easiest way to import Inventor is simply click 'Upload'  at the top of the Fusion Data Panel. Select your native Inventor file, and it'll import it to Fusion.

[ToddHarris7556]

Neil - I should have also added that the root issue that you're seeing is that once you export the part out to an STL, it becomes a 'dumb' solid - i.e. all feature intelligence is lost. An STL has no mechanism for multi-body anything. The diagonal lines that you're seeing are a side effect of the export process. In terms of export formats in general, STL and SAT are about the most universal/neutral formats you can use - but that's because they force everything to be 'dumbed-down' to the lowest common denominator. IGES and STEP, in my experience, have a little bit more intelligence, and at least allow multi-body parts. 

Sticking as much as you can with native AD files will give you the best chance of maintaining the feature history that you're after. Fusion does a pretty good job with Inventor files. 

If you really want to preserve the assembly / part hierarchy, then jump out to the Fusion Web interface, and choose Upload>Assembly. This will allow you to pick all of the Inventor files, and identify one as the master assembly. Note if you're using Frame Generator, you'll want to dive down into the Inventor Frame folder, and pick all the individual frame members, in addition to the master and sub assemblies.  Doing it this way will give you more usable subassemblies in Fusion. 

AND..... the Holy Grail is... 

If you use Fusion Team (kinda the Fusion workgroup/collaboration upgrade) then AD just came out with the Desktop Connector recently, and IT IS AWESOME. Still in Beta, and only available to Fusion Team folks for now, but it allows 2-way implementation of 'ANYCAD', which basically means I can roundtrip Inventor parts to Fusion and vice-versa. We'll design things in Fusion, and then insert those (live, not exported) Fusion files into Inventor, and use Frame Generator to fabricate the stand. Or generate parts in Inventor, and then our Fusion designers will insert those Inventor parts live into Fusion designs. Update the part in Inventor, refresh the link in Fusion.... everything updates. It works well enough - a couple of minor bugs yet to be worked out in Beta, but it's cool. Just FYI.

[TheCADWhisperer]

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@ToddHarris7556 wrote:

1. ....export the part out to an STL, it becomes a 'dumb' solid - i.e. all feature intelligence is lost.

2. An STL has no mechanism for multi-body anything.

3. The diagonal lines that you're seeing are a side effect of the export process.

4. In terms of export formats in general, STL and SAT are about the most universal/neutral formats ...

5. IGES and STEP, in my experience, have a little bit more intelligence, and at least allow multi-body parts. . .

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@Anonymous @ToddHarris7556 

As an educator - I thought a bit of elaboration might be appropriate here.

1. STL is a surface body format - not a solid body.

2. The attached files exhibit multi-body (or disjointed body) STL.

3. The diagonal lines are because the STL format converts geometry into faceted planar triangles.  For example, if you open the attached files you will observe that the Sphere was converted from, well, a sphere into hundreds of planar triangular facets in the STL.  For this reason, STL format is generally of little use for anything other than 3D printing (and a couple of other limited uses).

4. SAT (ACIS) format is not a neutral format.  It is a proprietary format owned by Spatial.  If you go to the referenced link you might notice that Spatial is owned by Autodesk competitor Dassault Systemes. Autodesk products have not read ACIS files beyond v7 (15 yrs?).

5. STEP is the generally used neutral format in the 21st century.  No feature history with neutral format files, but direct editing tools can be used, feature recognition tools might be used.  STL is only editable in a technique similar to the way an artist might edit a block of clay. Autodesk Meshmixer is one tool that can be used to edit STL.  In some cases the STL can be converted to a solid body (Autodeskmeshenabler) that can then be edited, but the existing planar facets are what they are...

Edit:  I realized that I did not fully cite all of my references, if there are any that you have trouble locating sources, let me know and I will do a bit more research.