Unexpected OD change when partially threading a cylinder - bug?

[Anonymous]

I have a cylinder and have tried to add a partial thread to the outside of it.  The original cylinder was 0.312 inch OD.  The thread was "(5/16)-18" male.

The thread was not the full length of the cylinder though, only the first half or so.  No errors or warnings were encountered during this, but the end result was most definitely not expected.

After adding the partial length thread, the OD of the remaining unthreaded section of the original cylinder (the smooth part that should not have been affected) had shrunk to 0.308 inches!  I did not notice this until way later when I was doing the 2D drawings for the part.

This makes my bolt shoulder (the smooth section) 4 thou smaller than I had designed it (enough to push it out of acceptable tolerances!).

Were this a real lathe-threading operation, the shoulder would not magically shrink by 4 thou.  This problem does seem to be reproducible.

The original cylinder was 1.5 inches long and the thread was set to affect only the first 0.750 inches. All of this takes place within the "Model" environment.

[laughingcreek · Accepted solution]

That's expected behavior for the thread tool.  it will change the size of your cylinder or hole to be what it needs to be for the thread you pick. 

If you need a shoulder on the cylinder, split the face where you want the shoulder to be.

[Anonymous]

Okay.  Strangely enough, splitting the face was what I had originally tried because I didn't know the threading tool had this facility built in.

It was a bit worrying to find unexpected dimensions after the fact, though.

Is it reasonable to ask that some kind of "build warning" message be added to the (partial) threading tool to notify the user that the partial threading will actually affect the entire surface?

Thanks for the help 🙂

[davebYYPCU]

You have not confirmed the thread is to specification, yet.

Does the cylinder get changed if you untick Model THread?

How far does a drill run out?

[Anonymous]

1. I have no reason to suspect that the thread is not to spec.  My concern is only for the bolt shoulder.

2. It seems not, but changing this seems to cause a warning in subsequent operations.  But since this is "expected behaviour", this isn't a problem.

3. I'm not using a drill for the hole this bolt goes into.  Runout is very small indeed.

[Anonymous]

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@davebYYPCUwrote:

You have not confirmed the thread is to specification, yet.

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Same thing happens if you use standard ISO Metric Profile threads.

If you have to split and model the geometry anyway - then what´s the use of a "partial thread" function?

At least Autodesk is aware that it is a "problem" -> https://forums.autodesk.com/t5/fusion-360-design-validate/modeled-thread-diameter-problem/m-p/730951...

@Phil.E

is there some update what will happen regarding this "expected behaviour"?

Manfred

[Phil.E]

@Anonymous

Unfortunately no. 

The work required is actually a huge task. The thread command would have to improve in order to allow the customer to pick their own shaft size, and that would vary with every customer potentially.

Perhaps I should explain a bit about the results you are seeing.

Fusion does not include the concept (as Inventor does) of modeling using Major, Minor, and Tap diameter as a user preference. What Fusion does do is provide a shaft or hole size in the nominal spec range for the thread, or at least it tries, for the purpose of tapping or threading by machine. (if you find exceptions please post them!) But not nominal bolt shoulder sizes.

For instance, using M8 x 1.25 as an example, and applying partial thread.

The size of the hole for internal threading is modified to be within the tap drill size range.

The size of the shaft for external threading is modified to be within the major diameter size range.

Both of these options are directly intended for CAM operations, not modeling standard hardware that may have completely different specs.

Bolts have very different "shaft" sizes, because the shoulder is not part of the threading calculation. Some bolt styles have different shaft sizes too, for the same thread. So it gets complicated fast, perhaps too much so for the Thread command dialog. 

So what is really needed is a bolt generator, perhaps? What do you think?

Regards,

[Anonymous]

@Phil.E

Thank you very much for the insight and information about the underlying concepts and ideas.

Bolt generator? Sure. But I assume you (=Autodesk) do not really need feedback like this. The "3D-Mechanical Design and Product Development" market is decades old and matured, there are a lot of well established solutions, Autodesk with Inventor is one of the key players in this market - so there should be no real surprises regarding customer requirements for this specific market.

I guess the more important question regarding the mechanical market is the overall positioning/focus/concept/strategy of Fusion 360. Of course I don´t expect public answers here. Time will tell, it will be exciting.

Manfred

[Anonymous]

@Phil.E, may I suggest a potentially simple workaround?

If the current accepted solution to this issue is for the user to perform a surface split on the cylinder, then how about an option to make the Thread tool perform the split on the user's behalf?  That would be quite a neat way to do it without actually having to rework the entire threading system.  The axis of the cylinder and the thread length and offset are known, so the split plane is known. 

It wouldn't even matter if the auto-generated surface split appeared in the timeline.

This feature could be a configurable option that is OFF by default.

Anyway, I'm a Solidworks guy who's used to having to spend an hour painstakingly modelling the helical cut path and the threading profile the hard way.  F360's thread tool is a huge timesaver even though it is a compromise between control and efficiency.  I can live with doing the surface split by hand 🙂

[chrisplyler]

Bolt generator? If you want. But that seems a separate issue.

How about this... If I have a 50-ft long x 2-ft diameter rod, and I want the last inch of it to be 1/4-20, how about just DON'T reset the diameter of the whole thing, huh? At least not by default and without notification. That's just silly.

[Phil.E · Accepted solution]

@chrisplyler Got it. Suggested improvement is logged as such: "split the body where the thread ends when user applies partial threading to a cylinder in order to preserve as-designed diameter of holes/shafts". 

[Anonymous]

@Phil.E

A slight nitpick:

"...split the face where the thread ends..." 🙂

That's kind of important, the body must remain intact.

[chrisplyler]

I think - to be technically correct within the context of how Fusion works - it should be "split the body, apply the thread to one of them, and then join them back together."

[Anonymous]

Under "Modify", there's a "Split Face" tool.  That's all I was referring to 🙂

How that works under the hood... I have no idea.  AFAIC, the end justifies the means.

[chrisplyler]

Yeah, you're totally right. I didn't think a split FACE would allow a diameter change of the underlying feature. But I was wrong.

[Phil.E]

Oops, pardon my typo. I meant "face". While you could split the body and later combine them, I would not recommend it. Splitting face is the underlying desired behavior.

[autodeskHCGNN]

Totally unexpected and illogical to have a partial thread reduce the diameter of the entire rod. I modeled a 20' piece of 1" black pipe with only about 1" on each end threaded -- why should the entire pipe have its diameter reduced?

The kludge of splitting the pipe is awkward and totally non-intuitive.

How about just fixing the function to do what is expected!!!