Thread function does not respect chamfers on model body

[Careless_]

Here's an example of how the THREAD tool in the F360 Design module does not respect CHAMFER features on models when "Full Length" is turned off.

I created a screw and then made a shank area that will remain unthreaded, and then a longer area that I would like to thread.

On this particular screw, there is a long chamfer where the transition to the threads are, like so:

Then when trying to thread just the remaining smaller diameter section, this happens:

As you can see, it ignores the chamfer, and extends the body section that the thread is applied to all the way to the base where the chamfered area is connected to the larger shoulder.

with "Full Length" off, it should just end the threaded portion at the declared length should it not?

I should mention that the thread tool suggests M7, but I know the thread for this particular fastener is M8x1.25 and these are the exact measured sizes I have put into the model, so that's why this is bothersome. It's not letting me just thread the smaller diameter section, instead it is creating an extension to the root of the chamfer.

Seems like a calculation bug?

[Careless_]

I should note that I've tried other ways;

Extruding from the face/end of the larger diameter shoulder using 3mm length and 170 degree taper, and then create the 12mm small diameter section; applying the thread still creates the additional tool body length.

The problem is that it's adding the additional body at the end of the thread once I change from suggested M7 to M8 thread.

at M7 size, it respects the current body section length:

it's only when the thread exceeds the size of the currently selected body does this become a problem. "Full Length" should not extend the body from end to end, it should only extend the body as far as the threads need it to be.

The only way I found to mitigate this extension that ignores the chamfer is to create the smaller diameter section as a separate body, apply the thread, and then combine the two bodies; a little more tedious than it should be in some cases where that's not possible (like already joined parts).

[wmhazzard]

Can you attach an f3d file of your model? I have done this two ways and have not had your problem. 

[Careless_]

wmhazzard, change your thread size to something that is larger than the body you are trying to thread.

i can see that you are using the suggested size because the major diameter of the thread is the same size as the diameter of the body you are applying the thread to.

go one or two sizes up and the problem will present itself.

[jeff_strater]

I suspect the problem here is in this statement: 

"it's only when the thread exceeds the size of the currently selected body does this become a problem. "Full Length" should not extend the body from end to end, it should only extend the body as far as the threads need it to be."

I assume, @Careless_ that you mean here that you expect that if the thread is not full length, and if you pick a thread size that is different than the cylinder size, that you expect the Thread command to only enlarge (or shrink) the cylinder in the area where the threads are.  Is that correct?

If so, that is not the way Thread works today.  Thread resizes the entire cylinder selected, even if the thread is just a partial thread.  To do otherwise would require that the body be split at the place where the thread ends.  While this is an interesting suggestion, it is not the way that Thread works today.  The other workaround is to us Split Face to split just that cylinder face:

[Careless_]

Jeff, the problem is that the thread tool extends PASSED the chamfer. It is ignoring the end of the cylinder where the chamfer feature starts, and obliterates it.

IMHO, it should end where the chamfer is, as that is the end of the diameter that the thread would be on.

Anything passed the chamfer is part of another portion of the model and should not be included in what the Thread tool can access.

note these images:

Here is the chamfer:

Here is the thread body going passed the chamfered area. The end of the chamfer is ignored:

[wmhazzard]

Yes, it is annoying that the command resizes the entire length even if the thread is not full length. Try drawing a stud that is only threaded on either end then make a 2d drawing of the stud, you will find out that the main body of the stud is undersized by the amount of the thread clearance and you have no way to dimension the body without using a text leader. Then you have to go back and split the face where the threads stop and re save, it is a PITA. 

[Careless_]

yes i ran into the same issue and I ended up having to send a drawing to someone with a step-stud that had no threads on either end and had to modify the text leader for the diameter callout with the thread size manually for what it "should" have been machined to.

I'm sure they had a good laugh at it when they saw it and said "is this guy sending cartoon drawings now?" 

[jeff_strater]

there are two effects at work here.  The first is the one I already mentioned - that selecting a larger or smaller thread size will resize the entire cylinder, even for partial threads.  It is debatable as to whether this is a bug or an enhancement, but this is a fact of life for Fusion today.  The workaround to that problem is to split the face that you want to thread.

The second behavior that is contributing to this case is the way that cylinder offset works with an adjacent cone face (chamfer).  When you resize that cylinder, it will consume the adjacent cone.  In a general sense, this is desirable behavior, but in this case, it does not meet your expectation, which is a valid concern.

[Careless_]

I see that in your latest screencast this would be desirable for push-pull feature. I actually like that it does that. Thanks for the demonstration. It definitely makes the case for why it functions as it does.

Might I suggest a way to include another option to prevent this from happening in cases where splitting the body and recombining them will break other actions further down the line?

perhaps a similar function to Chain faces option:

It seems like the logical approach to this issue.