Why does tapering extrusion not work for text?

[m.a.peletier]

When I create a letter 'e' (for instance) in a sketch, explode it, and extrude it, Fusion does not allow me to set any non-zero tapering angle. The error message is 'Tool body creation failed. The end of the sweep could not be created. Try changing the profile or the taper angle.' It does not depend on the angle; any non-zero angle gives the same error. On the other hand, if I draw something resembling an 'e' by hand (with the Line tool) the error message only appears when the tapering leads to some form of self-intersection.

Am I missing something? Why does the text object not allow for tapering?

(The workaround in http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/drafted-extruded-text/idi-p/5630507 does not seem to work for me)

Mark

[jeff_strater · Accepted solution]

This will depend on a lot of things:  What font you used, what size of text you used, how far you are extruding it, etc.

Using the standard font, with size = 30mm, and extruding 4.5mm, I was able to apply up to a -8 degree draft to the letter "e".

Here is a screencast of doing that in Fusion:

Hope this helps

Jeff Strater (Fusion development)

[Anonymous · Accepted solution]

Hi Mark, I found that you can create any taper you want if you go through the trouble of lofting text, such as shown below.

I used the built in text generator, then to turn that into sketch geometry I extruded a short distance and defined another sketch on that (I think there is an easier way to get the sketch geometry from text generator, but cant remember off hand).  Proceeded to copy the text sketch geometry and past it in another sketch defined on an Offset construction plane.  Finished that sketch, then selected it in browser tree, and went to Modify > Scale which actually allows scaling that whole sketch.  I then turned the other sketch visibility off so that I could selection box everything in the 2nd sketch, turned 1st sketch visibility back on, and proceeded to move the 2nd sketch into desired position (without entering the sketch, which would go back in time before scale operation).  An alternative method would have been to make a point in the center of the text to use as the Point in the Scale tool.  I had to do two lofts, the second being the inner part of the letter "e", being a cut operation for that loft. 

Just something to keep in mind depending on what you're trying to do. 

Jesse

[Anonymous · Accepted solution]

I just noticed the Offset sketch operation works pretty good for generating the reduced e loft profile that in many ways gives better results for the loft. 

Jesse

[m.a.peletier]

Jeff and Jesse, thanks for the great suggestions and quick reply!

Jesse, I tried both your suggestions (scaling and offsetting) and they work well.

Jeff, the only difference between your suggestion (which works) and my initial attempts (which didn't work) seems to be the size of the letter - I took it at 10 mm, you at 30 mm. I now find that at 30 mm I get no errors, while at 10 mm, otherwise doing exactly the same (and replacing 4.5 mm extrusion depth by 1.5 mm), I get the errors. Is this expected behaviour? Does it have something to do which thresholds for closeness of vertices and such?

Again, thanks for the quick response.

[Anonymous]

Great to hear you got it to work.  If I did this again, probably would trace the letter with splines and lines, then select and right click on the splines and choose Toggle Curvature Display, to allow adjustment of the spline points to get decent curvature smoothness. 

Jesse

[jeff_strater]

Interesting that it does not work at 10mm.  I verified the same thing.  I will investigate this, it could be a tolerance thing.

Yet another choice (although also a more bit labor-intensive) would be to use the Draft command to add the draft afterwards.  Do the extrude without draft, then choose Draft, select the planar face as the pull direction, and select all the side faces to draft.  I find it easier to do this using a window select from the side.

This seems to work well for the default 10mm size (which further makes me wonder why extrude with draft fails...).

Here is another screencast:

Jeff

[Anonymous]

Ah yes, right click on the text to explode it, forgot about that, and the draft tool as well, which seems pretty darn capable.  Thanks Jeff!

Jesse

[m.a.peletier]

@jeff, thanks for pointing out the alternative of drafting - that also works well. And thanks for the quick responses!

Mark