Extrusion failure

[etfrench]

The attached drawings demonstrate two errors with extruding shapes from imported dxf files.

Rosette_000.f3d has one shape that was successfully extruded and one shape where it doesn't recognize the shape. I don't know of a way to force Fusion 360 to join all of the arcs.

Rosette_001.f3d has two shapes that appear to be extrudable, but Fusion 360 fails to extrude.

Is there a change I can make in the original dxf files or another way to force Fusion 360 to join the arcs? The 2d CAD program is Visual CADD.

p.s. I'm getting this error when attaching the diagnostic files:

Correct the highlighted errors and try again.

The attachment's Fusion360DiagnosticLogs.zip content type (application/x-zip) does not match its file extension and has been removed.

p.s.p.s. The forum doesn't like copying the error message either: Your post has been changed because invalid HTML was found in the message body. The invalid HTML has been removed. Please review the message and submit the message when you are satisfied.

[Discussion_Admin]

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@etfrench wrote:

The attached drawings demonstrate two errors with extruding shapes from imported dxf files.

Rosette_000.f3d has one shape that was successfully extruded and one shape where it doesn't recognize the shape. I don't know of a way to force Fusion 360 to join all of the arcs.

Rosette_001.f3d has two shapes that appear to be extrudable, but Fusion 360 fails to extrude.

Is there a change I can make in the original dxf files or another way to force Fusion 360 to join the arcs? The 2d CAD program is Visual CADD.

p.s. I'm getting this error when attaching the diagnostic files:

Correct the highlighted errors and try again.

The attachment's Fusion360DiagnosticLogs.zip content type (application/x-zip) does not match its file extension and has been removed.

p.s.p.s. The forum doesn't like copying the error message either: Your post has been changed because invalid HTML was found in the message body. The invalid HTML has been removed. Please review the message and submit the message when you are satisfied.

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Could you please mail me the zip file that recieved the error to moderator@autodesk.com. Also let me know what program you used to zip the file?

Thanks
Discussion_Admin

[Discussion_Admin]

Update: I have received your file and have escalated this issue.

Thanks
Discussion_Admin

[etfrench]

Any update on the original issue?

[jeff_strater]

Sorry for the lack of response here.

It seems like the small arcs in the one sketch have not been connected.  If I manually connect them, I can get the extrude to work:

But that is a painful process, and should not be necessary.

Can you share the original DXF files, so that we can try to see why these endpoints are not connected?

Thanks,

Jeff Strater (Fusion development)

[etfrench]

I had to increase the resolution in Visual Cadd to 8 decimal places in millimeters to measure the gap 🙂

The attached RosetteConstructor4.dxf gap is 0.00001605mm.  It will not show the objects as being extrudable in Fusion 360.

Rosettes5.dxf gap is 0.00000618mm. It shows the objects as extrudable, but fails the extrusion with the following error:

  The operation failed.
    Try adjusting the values or changing the input geometry.

[etfrench]

Attached is another example where Fusion 360 isn't joining the dxf shapes into extrudable objects.  The purpose of the drawing is to machine cutouts for a fan, so it should be obvious which lines and arcs should be considered individual extrudable objects. The cutouts are on the "FanCutouts" layer.  One segment in each ring was created, then radial copied, so I would expect all of them to be treated equally in Fusion 360.

[ShirleyShi]

Hi

I tried in AutoCAD and Fusion, neither of them can open first two dxf files. The last file (SwitchAndFanCutouts_005.dxf ‏) can be opened by Fusion and AutoCAD. I investigate it a bit and found the points on the left-side is truly connected while the points on the right-side is not connected.See below picture for reference.

Fusion is not able to auto-repair the gap for now. We are going to make some improvements to visually distinguish coincident sketch points from non-coincident points. If you have some suggestions/comments, feel free to let us know.

 Thanks,

[etfrench]

1. The zoom levels in Fusion 360 don't go deep enough to find 0.000001mm gaps.  It should be able to zoom to the minimum gap size where Fusion 360 considers points to be co-incident.
2. Have an option to show all of the construction points in a sketch (If there is one now, I can't find it in the preferences dialog).
3. Have a tolerance setting for minimum gap size.
4. Have a join command with trim, extend, and move endpoint options.

[ShirleyShi]

Hi etfrench,

Thanks for all your great suggestions.

Yes, zoom level is a limitation of Fusion graphics system now.

We are making some improvement (available in next release) to visually distinguish those unconnected point. (similar to your option 2, but not in preference dialog). An example of the improvement is as below.

We will investigate your suggestion 3 and 4 to make Fusion better for handling those tolerance issues. I noticed the precision of the values in your dxf is not high, for example, an arc center point is (6.474098, 2.61295), does Visual CADD have any settings to enhance the precision of the output dxf?

Thanks,

[etfrench]

Visual Cadd can display 8 decimal places, but seems to only export 6 decimal places.  For some reason, Fusion 360 requires the units in the dxf files from Visual Cadd to be centimeters.  This limits the resolution in Fusion 360 to 10 nanometers, which is usually good enough for me 🙂

Identifying the problem areas is a good first step.  Adding the tools to correct the problem would be even better.

Thanks for looking at this issue.

Ed