Chamfer the end of a threaded bolt

[segallyscott]

I need to chamfer the end of this threaded bolt.  I originally drew the bolt with the chamfer then just threaded the shaft.  The thread call out wouldn't lock on until I removed the chamfer because the edges didn't line up correctly.  Is there something technique wise I can do differently?

[TrippyLighting · Accepted solution]

This is requires a workaround that is as old as modeled threads in Fusion 360.

1. Extrude the stud.
2. Chamfer the stud.
3. Apply the thread to the stud.
4. In the timeline, pull the thread feature to before the the chamfer feature.

[HughesTooling]

If you first create the thread as a cosmetic thread, add the chamfer after the thread in the timeline then edit the thread and change it to modelled you'll get the correct result.

Mark

[g-andresen]

Hi,

When creating a thread, only the lateral surface of the cylinder is captured, but not also the chamfer.

I would do it this way.

günther

[patSS3DT]

Newbie here.  That procedure causes the chamfer in the timeline to turn red and report: "compute failed".

I checked my work numerous times, have not found any deviation from the solution steps.  What am I missing please and thanks?

[g-andresen]

Hi,

Have you tried the suggestion from @HughesTooling ?

günther

[HughesTooling]

@patSS3DT If the thread has a filleted form like a BSP for example, chamfer will not work.

For a thread with fillets you'll need to create a sketch then use a revolve cut to create the chamfer after adding the thread.

[patSS3DT]

That's exactly the problem!  Neither work-around process worked with a chamfered thread.  I was trying to save time over revolve cut, but fine.  Problem solved, thanks so much. 

[TheCADWhisperer]

@patSS3DT 

There is an easier way than Revolve-Cut.

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[patSS3DT]

Thanks.  This is just an arbitrary cylinder - to isolate this procedure as a learning tool prior to making real parts.

[g-andresen]

Hi,

try this way, as @HughesTooling   (post3) has desribed

günther

[HughesTooling]

For fileted threads you can add the chamfer first then delete the face under the chanfer to avoid the need for a sketch and revolve. I think this is what @TheCADWhisperer was going to suggest? See attached file.

[patSS3DT]

Brilliant! Thanks!