Failing to emboss a Voronoi pattern on a cylinder.

[cadTPLWJ]

I have generated a Voronoi sketch with generator default settings.

I have made a cylinder with the same surface area as the Voronoi sketch.

Design file attached.

When I try to emboss the Voronoy paches onto the cylinder I get an error

Error: Cannot create emboss feature at specified depth. Adjust depth.

Embossing by dividing into several subsets of the patches works as intended. 

What am I missing?

[jeff_strater]

it looks to me like there is on problematic profile here.  Succeeds with all the rest selected.  I need to dig into it a bit more.

[jeff_strater]

Strange.  Still not 100% sure what the issue is with that profile.  I created bug FUS-82553 for it.  I was able to get it to work by marking that profile as construction, and fitting a new spline around that set of curves. I did not take a great deal of care doing it - you'd want to do a better job, certainly.  The repaired model is attached.

[cadTPLWJ]

Thanks for looking into this.

What method did you use to find the offending curve?

I tried to offset the offending profile a small amount an then deleted the original profile.

That did also work.

[jeff_strater]

just pure trial and error.  Kept selecting profiles, a few at a time, until it failed...  It was tedious, but I was not paying attention in the meeting I was in, anyway...

[jj.space]

Exactly the same problem here! A few cells generated bij the voronoi generator refuse to emboss. Extremely frustrating...

[g-andresen]

Hi,

The problem is caused by the sketch quality.
In the screencast I show a process to clean it up.

günther

[g-andresen]

Hi,

these are the situations

I have measured distances < 0.01 mm between control points on numerous elements.

This explains for me that problems occur when wrapping.

günther

[cadTPLWJ]

Are these control points that really should be coincident (like begin and end of spline) but due to computing errors are not? 

[g-andresen]

Hi,

The larger the number of points for the definition of a curve, the greater the problems with subsequent actions. Thus, you can extrude the profiles perpendicularly, but the tapering or wrapping then leads to problems.

günther

[g-andresen · Accepted solution]

Hi,

These are the consequences for extrusion with cone:

günther

[ogmios2autodesk]

I am having a lot of issues myself, I had to painfully select each cell to see which one work and still had almost 7 cells that will not emboss.

Any tips would be greatly appreciated.

[g-andresen]

Hi,

As I have written here several times, the sketches are problematic because of the amount of control points.

günther

günther

[ogmios2autodesk]

Hi Günther. Thanks for responding. I did read the whole thread a few times, but failed to see or understand the steps involved for me to be able to fix it easily on my own. The screencast has no sound and the interface is in German, so I am not sure what the process to clean should be. Thanks again.

[g-andresen]

Hi.

The screenshots show the number of control points before and after conversion.
The difference should be visible.
The embossing process in Fusion fails because the distances between the control points are sometimes so small that self-intersections occur when the column is wrapped with the Voronoi sketch. The self-intersections increase as the diameter of the column gets smaller.
This does not happen with the converted sketch because of the smaller number of control points and thus larger spacing.

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@ogmios2autodesk  schrieb:

 ... so I am not sure what the process to clean should be. 

---

To clean up such curves, you need an application that allows conversions for given tolerances.

My tool is V-Carve.

günther

[john]

Came across this thread after experiencing the same issues.

My workaround as follows:

1. Produce the Voronoi sketch as normal - with border.
2. Do a straight extrude of the sketch (1mm will do) to produce a flat panel containing the Voronoi 'holes'.
3. Create a new sketch on the surface of the solid produced by the previous extrude.
4. Hide the solid.
5. None of the problematic areas are transferred to the new sketch - if you select the background area  of the sketch, it will quickly show the missing areas which you can re-create with the spline tool:
   

6. Recreate the missing bits.

7. Delete the lines framing the sketch and complete it.
8. Your pattern should now useable for the emboss.