'Offset face' on threads fails on simple shape

[matthewjschultz]

I've been experiencing a failure of 'offset face' on a very simple shape:

When trying to apply a -1/128" offset to the thread face I receive the error: "The operation could not create a valid result. Try adjusting the values or changing the input geometry." 

To validate/test this error, I created a plain rectangular cube of the same width and height, cut out a centered cylinder of the same .5" diameter, applied the same 1/2-12 UNS threads, and attempted the same 'offset face' operation. And it worked with no problem.

So what is it about this body/shape that prevents the offset from being applied to the face of this thread?

These two bodies are in their own component, and they're the only two bodies in the design.

• I've tried both 'full length' and a specific length for the threads; both fail
• I've tried the offset as a direct entry and a user parameter (shouldn't matter obv., but hey… I'm testing)
• I've tried changing the diameter of the original hole; doesn't seem to matter
• The body was extruded up from the sketch; the arc'ed hole (where the back of the threads end) wasn't cut out

Any ideas?

[g-andresen]

Hi,

Please share the file.

File > export > save as f3d on local drive  > attach it to the post

günther

[TheCADWhisperer]

@matthewjschultz 

Does it work if you enter the decimal equivalent of the fraction instead?

[matthewjschultz]

Same error.

[matthewjschultz]

Attached as both .f3d and .zip

[HughesTooling · Accepted solution]

I think the problem is the C shaped cutout leave parts of the thread unattached. If you cut the C shape after creating the thread and offset it works fine. See attached file.

[matthewjschultz]

I've also uploaded another version with a control body that has a successfully applied 'offset face' to both sides of the thread, for comparison.

[matthewjschultz]

Oh, interesting! 

I still think F360 should be able to figure out how to properly execute the thread on the shape, but I do appreciate the work-around!

Thank you!

[HughesTooling]

I also made the hole a bit deeper as it didn't go all the way through the C shape.

[matthewjschultz]

I'd have to go back to my original file to see if I extended the hole further than in my test file, so good catch.

Either way, your work-around WORKS, so I'm accepting that as my solution.

Thank you!

[matthewjschultz]

I just edited the extrude feature to extend the cutout to ensure it clears the c-shape… same problem. So it wasn't that, but still… good catch.

[HughesTooling]

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@matthewjschultz wrote:

Oh, interesting! 

I still think F360 should be able to figure out how to properly execute the thread on the shape, but I do appreciate the work-around!

Thank you!

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It's probably because when you start to offset you get to a point where the face has to extend past the centreline and then remove the unjoined part of the thread. This sort of situation tends to give CAD programs problems.

In the version where I cut the C shape after you get this.

[matthewjschultz]

Mark,

I appreciate the time you took to detail this for me. While I use F360 a lot, I'm very much a novice, so the time you've taken out of your day to illustrate the difference and educate me is important to me.

Thank you!