Exporting From Adobe Illustrator into Fusion 360

[daschenbrener_0069]

I really looking for the standard or the optimal option on importing Adobe Illustrator files into Fusion. 

The more involved and the more I'm learning this, anytime i import a design from Illustrator as a DXF file, anything circle related imports a splines, and therefore cannot be selected, to extrude etc. 

So is there a way to do this and how?

Is SVG the Answer?

And is there a way to export circles to be identified as holes in Fusion?

I appreciate your time to assist.

[TrippyLighting]

There isn't a standard other than this is generally a not a good idea and this forum is full of threads and posts reporting problems related to imported DXF and SVG files.

[daschenbrener_0069]

thanks for your feedback and opinion. 

[daschenbrener_0069]

What best practices can you share for designing ?

[g-andresen · Accepted solution]

Hi,

Basically I can say that imports are only a stopgap solution compared to the sketches created in Fusion.

There is also no difference in format (SVG or DXF) as for the application from which the file originates.
If a sketch appears after pasting as it was originally created in Fusion, this is a lucky circumstance.

You should only import sketches if you have a sufficient repertoire of error analysis and elimination.

günther

[daschenbrener_0069]

I appreciate your insight and response. this does makes sense.

[TrippyLighting]

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@daschenbrener_0069 wrote:

What best practices can you share for designing ?

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That really depends on what these sketches contain.

The problem with imported geometry is of varying nature and maybe one or all of the following.

• Curve/line ends are not recognized as coincident by Fusion 360 and that prevents Fusion 360 from creating a profile ready for extrusion. Graphics design software does not necessarily have to apply the same stringent rules to line/curve geometry required by Fusion 360 or other CAD applications.
• Tangency or curvature continuity is not maintained between curve segments resulting in near-tangent situations which very often lead to frustrating modeling problems. E.g. you can extrude the profile, but then applying little draft or filleting does not work.
• The imported geometry includes too many line/curve segments and that really slows down the Sketch solver in Fusion 360 making any work unpleasant if not impossible.
• Overlapping and/or duplicate line/curve segments create hard to identify modeling problems.
• Implementation of splines varies between different software packages even in just the CAD world, let alone adding graphics design software to the mix. Such curves when exported are not editable and when joined to other curves do not have to comply with the tangency tolerances required by a CAD application. Those curves also might be tessellated into many small line segments approximating the curve. Extrusion might have many facets if the high line count does not already result in a serious slow-down of the sketch solver.

Often the best solution is to trace imported sketch geometry with Fusion 360 native tools.

But for many projects that would be very labor-intensive and cumbersome.