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

[angelika6ECA3]

Hello,

I am trying to emboss a logo on a curved surface.

I successfully embossed 4 of 5 parts to the same surface but am getting an error message for one of the (closed) sketches. Error: Cannot create emboss feature at specified depth. Adjust depth.

I successfully embossed the same DXF to a large, flat surface previously and I am struggling to find any fault with the part of the logo that throws the error message.

I would appreciate assistance with what I can do to solve this.

[jhackney1972]

Please attach your model and the DXF, if it is not in the model, so the Forum users can troubleshoot your issue.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section of a forum post to attach it.

[angelika6ECA3]

My apologies, I failed to check that it attached properly before. Should be there now.

[jhackney1972]

It is pretty bizarre how I got it to work.  I have no explanation why it will not work in the first place.  I will continue to try and refine the process I used but I thought I would send along the model I have now.  I will get back to you if I can refine it any better.

[g-andresen · Accepted solution]

Hi,

I converted the curves and into arcs and reduced the number of control points.

günther

[jhackney1972]

Guenther, does Fusion have the ability to convert curves into arcs?  If yes, how is it done, trying to learn something here.

[jhackney1972]

@g-andresen has given you a much better solution than mine.  The problem seems to be in the upper part of the "T" in the section that would not emboss correctly.  I guess by my breaking up the profile and Embossing multiple times got around it.  I am glad you have a solution.

[g-andresen]

Hi,

---

@jhackney1972  schrieb:

Guenther, does Fusion have the ability to convert curves into arcs? 

---

No, I do it with V-Carve Pro, which I have used for many years to do various types of machining on a CNC.

For the creation of multi-layer engravings, the conversion and cleaning of paths is a central tool there.

günther

[jeff_strater · Accepted solution]

here is how I fixed this:

step 1 - add some lines to the sketch in the area that fails.  We are trying to narrow down the problem:

Then, see what area the problem is in:

That narrows it down to part of the T.  Repeat:

Then, I just go lucky, and tried deleting this section:

and, replaced it with a fit point spline (I was not all that careful to reproduce the original)

That worked:

Finally, go back in and remove the lines, and this is the result:

repaired model is attached

[angelika6ECA3]

Thanks for solving my problem so quickly. I was successful with drawing random lines to find and fix open sketches before but this one actually extruded and embossed on onto other surfaces alright which really threw me!