Failed to perform boolean operation error

[timothyhinessr]

I'm working with a DXF file of a customer's logo provided by the customer.  I want to engrave the outline of the logo onto a slightly convex surface using the trace tool path.  I've done this on different parts that are flat with no issues.  When I  go to extrude/cut the logo into the convex surface, I can do so with all the letters except the large A.  When I try to extrude/cut that letter, I get the "Failed to perform boolean operation" error.  I can't see anything obviously wrong with that particular letter in the logo but there seems to be some issue with it that is causing the error.  I've tried extruding/cutting it onto a flat surface but get the same error.  I've tried a variety of work-arounds but can't find a way to get the geometry onto the convex surface as needed.  I know I can edit the DXF file if necessary but I don't know what is wrong with it so don't know what to change.   I've burned about four hours on this now and am out of ideas.   I've included the CAD file below.  Any help would be appreciated.

 

[jhackney1972 · Accepted solution]

At first glance, I to do not know the reason but what I would do is use a different method of cutting the "A" and move on.  The Screencast will explain.  Model is attached if you cannot get success yourself.

[TrippyLighting · Accepted solution]

Before selecting the bottom surface, change the Extend Type from "Distance" to " To Object".

@jhackney1972 I don't seem to be able to tag Autodesk Folks to take a look at this case. Could you try ?

If a subsequent, separate boolean operation works, then this error message seems unnecessary!

[jhackney1972 · Accepted solution]

@TrippyLighting I tried what you mentioned but it gives me the same error the original poster was getting.  I too cannot add either Jeff Strater or Bill E "@" attention to this post.  I will drop a Private Message to Jeff giving a link to this Forum post so he can hopefully take a look.

[jeff_strater · Accepted solution]

it's the scale factor applied to the sketch.  0.037 is an awfully small scale factor to apply.  DXF geometry is already notoriously inaccurate.  If you take already-inaccurate data and scale it by that amount, I'm not surprised that there are errors.  My guess is that one of the curve segments becomes so small that it starts to interfere with the solid modeling kernel's accuracy.  I rolled back before the scale, created a new, larger cylinder, and was able to extrude the "A" OK.  However...  The "V" was not recognized as a profile.  I had to edit the sketch, and use divide-and-conquer to find the bad curve, delete it, and replace it with a line.  Then the whole string works OK.  So, in addition to @jhackney1972 's approach, you could create the entire thing at full scale, and scale afterward.

[timothyhinessr]

Jhackney1972's solution worked great.  I played with both extrude and combine for over an hour but never combined them correctly to make it work.  In the future I will try modeling and extruding it at the scale the DXF file comes in at and then scaling everything afterwards.  Everyone's responses were helpful and educational, thanks so much!