Unable to select cylinder for inner threads

[eplumer]

In the attached f3d file, I have extruded a cylindrical cut (Extrude38) through the side of a ring shape. The extrusion was made from a fully-defined circle in Sketch6. In the photo, the hole in question is in the upper left.

I am able to select the cylindrical face when not in any tool. As soon as I select the thread tool, I can no longer select that face. Other posts I have found indicated that the only way this should happen is if the face was not extruded from a true circle or had some taper to it. Neither of these problems exists as far as I can tell. Only odd thing, perhaps, is that the sketch is on the flat surface in the lower right, not on a construction plane attached to the ring itself.

I have tried a number of ways of specifying the ends of the hole to get the threading to work. The only success I had was to extrude a hole that extends, not only through the outer edge of the ring but also through the square base section that includes the profile plane. That allows me to thread the part I want but leaves me with an undesired extra hole through the base block. Any attempt to "fill it back in" with a join extrude causes Fusion360 to report an error.

[saito.kh]

Hi @eplumer,

Thank you for posting in the Fusion 360 community!

I am sorry to hear that!  I am able to reproduce this on my machine as well.

I will discuss internally on this behavior and will circle back here as soon as I have something to share.

Thanks for your patience.

[eplumer]

Thank you, look forward to your suggestions

[James.Youmatz]

Hi @eplumer,

I can help out here as well. The issue is that the hole that is created on the top is not perfectly cylindrical. We can observe this in two ways - the first if we physically look at the hole, we will notice there is an edge in there, denoting that it is not a perfect cylinder. Also, if we use the inspect tool on that face, we can notice that "Radius" and "Diameter" are not options for dimensions, indicating that Fusion does not believe it is a perfect cylinder. With that being said, I need to investigate what in your workflow is causing this issue - it is possible it is a bug. Let me log this with development and see what they say.

I have found a workaround, and perhaps a better modeling method for this hole as well. I will be creating a Plane tangent to the outer face at a point. That point will be created from your original sketch. My screencast below documents this. Let me know if you have any questions and I would be happy to clear this up. 

[eplumer]

James, thank you for the information. Odd about the hole I bored not being a correct cylinder given how I generated it. Also, If I project the same extrude further to go through the profile plane, then the threading works.

Good deal on the tangent construction plane using a reference point. In the past I have used a tangent plane angled relative to a reference plane. In this model, I had problems with getting it to accept my choice of reference plane. I wonder if that was also related to some odd-ball issue with this model.

By the way, I had simplified my example a bit before posting. In my original approach, I had this circle sketched in the same place as the other two holes to keep all of that specification in the same place.

[Phil.E · Accepted solution]

@James.Youmatz not to step on your shoes but...

@eplumer Here is the issue:

The "from" object is the circular inner face. That is producing a degenerate cylinder, which is what breaks the workflow. That is likely the bug here.

Using a plane as reference "from" object, it works well.

Thanks,

[eplumer]

To paraphrase ... it does not matter that the cylinder, as it enters and exits the "ring", forms non-circular cross-sections at the beginning and ending of the threaded section. It is only important that the full extrusion start on a flat plane?  That also explains why James's workaround succeeded as well.

Phil, when you say "that is likely the bug here", does that mean you would have expected the operation to work without introducing the extra construction plane? Or do you mean the "bug" is in my choice of workflow? Regardless, this gives me a good understanding on what is going on and how to deal with it.

Thank you all for the support.

[Phil.E]

Thanks for asking. Sorry about any confusion.

It's fair to assume that the sketched circle profile is the one that pokes the hole in the ring. In this case, it's obviously not.

When you use another shape such as rectangle, it works well. That's why I called it a bug, because of inconsistent results and a bit of confusion on your part.

Plus, I think we can improve the circle case you present. 

For my own two coins:

I'm a little old fashioned. I am used to extruding from planes, so when a "from" object is most easily a cylinder, I already start to think about other ways to do it. 🙂

Thanks,