Full Form Tapered Thread Mill

[mitchghmgarage]

I am trying to use an NPTF full form thread mill to cut a internal tapered pipe thread. I am using a Guhring 3/8 18 TPI NPTF thread mill. See link for thread mill details.

https://www.guhring.com/productsservices/sizedetails?edp=9037570175700

I get the following message:

Warning: Full form thread mills are not supported for tapered faces. Toolpath will be calculated as if the tool is single form.

1. Will the resulting tool path work despite the warning message. It used to work and I did not get this message before with this exact same program.
2. How do you use a full form thread mill with Fusion 360
3. When will Full Form Thread mills be supported. They are very standard and produce the best threads. We use a lot of these, especially insert type thread mills.

[Farzati.Scott]

We do full thread NPT's at or shop all the time.  I just describe it as a normal threadmill diameter based off the small end of the cutter.  The drill size will be like a std thread but to the size for your NPT.  The NPT Threadmills are designed to cut the thread as well as the taper.  Usually if there is clearance I go depth wise about .05 less than the full amount of threads on the cutter.  On the manufacturing side you will need the pitch, few stepovers since its cutting the tapper as well, and the diameter to step out too.  Example:  3/4-14 NPT ( use a 3/4 spot drill, 59/64 drill, NPT threadmill for 3/4-14 & a 90 deg chamfer tool for the lead since will be around 1.04 diameter.  So Threadmill in my tool description is a standard threadmill selection using one for 1/2-14 threads (same pitch), .496 diameter & .929 flute length.  On threading toolpath the pitch is .0714 with a diameter offset of .120, 3 stepovers at .010 and a springpass.  The diameter offset will change depending on what size NPT you use and the depth you choose.   I made it easier and set up Templates for my various threadmill operations so I know tools, pitches, offsets will work every time.  Hope this helps...

[mitchghmgarage]

<meta charset="UTF-8" />

Thank you for your response.   We have been doing that for a while.  However, we just started getting this message and the resulting tool path has now changed from the previous tool paths.  It would be nice if Fusion 360 "officially" an properly supported full form tapered thread mills without "tricking"  the system.

[Farzati.Scott]

Attached your part with toolpaths & tools

[Farzati.Scott]

I agree, ran into this problem as well in the when using the hole option it wants to always pick nominal drill size.  However that is not correct in that the drill size depends on the percentage of thread you want.  So continue to do things old school.  They seem to concentrate on the modeling and presentation side of things & not real world application of manufacturing...

[mitchghmgarage]

<meta charset="UTF-8" />

Thank you.   I just hate getting warning messages and find myself spending hours (sometimes many) verifying that the warning message can be ignored.   Would be much better if they added full form mill npt support.