Thread milling a tapered thread

[stuart.higginsA877K]

Hi everyone,

Please help. ha... I'm struggling to program a tapered thread. I need to produce a 3/4 NPT but keep getting a error come up. I've attached the file if anyone could help and see where I'm going wrong? 

Many thanks

[engineguy]

@stuart.higginsA877K 

Not seeing any "Error" here, only a Yellow warning that the "Full Form" threadmills are not supported for Tapered threads and the toolpath will be generated as if the tool was a single tooth, if you want to get rid of the Yellow warning then just edit the tool to be a single tooth tool.

Other than that it appears to be doing the thread correctly in the simulation.

[seth.madore]

And if you ARE using a full-form threadmill, then you DON'T want it going up the full length of the part, but rather, 1.5-2 full revolutions.

Still, you need to define it as a single flute tool, favoring the small end diameter.

[stuart.higginsA877K]

@seth.madore sorry i forgot to say I'm using a tapered thread mill with more than the full thread length - so yes only need to mill one revolution..

also im getting confused as i cant change the angle of thread on the actual tool in the tool library which makes me unsure as to what diameter i should be using the top or bottom of the actual tool?

[seth.madore]

Define your threadmill as a single flute, using the bottom (smallest) diameter. You are going to be using cutter compensation, so it's going to be a crap shoot on how much you need to adjust at the control. For controlling how many revolutions, that will be done in your heights tab. I'd set your Top Height to Bottom Height + 1.5 thread pitch. You can control this with an expression: 

bottomHeight_value+(1.5*threadPitch )

[stuart.higginsA877K]

Ok. That makes sense now. Can you confirm that both face of model being tapered and the tool will not cause a issue with toolpath?

[stuart.higginsA877K]

@seth.madore  Meaning it will still produce the correct thread?

[stuart.higginsA877K]

@seth.madore  would i be right in saying i need to change the model face so its not tapered as the taper is being machined with the tool? 

[seth.madore · Accepted solution]

Hmm, I don't think so. The one time I've done internal NPT threads with a full form, I modeled it with the npt taper:

 This MAY require some experimentation on your part, though

-EDIT to add:

Also, it appears that I too now have that warning and they've properly broken full form taper threadmilling. So......

[engineguy]

@stuart.higginsA877K 

@seth.madore 

Just out of interest I downloaded a Harvey Tapered NPT Thread Mill .DXF and created a "Form Thread Mill" from  it and had a go at the thread in your file to try and get it done with a single revolution, seems to work OK in the attached file 🙂

Yes, it appears do the thread OK if the Boss is not tapered, only downside is that on the first pass the tool is taking off more material at the top of the Boss but after that it will be even depths if you are doing multiple passes.

Single pass could be a bit heavy.

Making the Taper on the Boss the same taper as the tool is probably the best way forward but you will have to stick with the Adaptive to get the taper, getting the depth offset right means a bit of Math or some "trial and error" will do as well 🙂

Anyway, it was an interesting excercise and good info (For me at least 🙂 ) for the future 🙂 🙂 File attached

[DarthBane55]

It is no different than threadmilling a NPT hole.  Most people would just drill the hole, and threadmill with a NPT threadmill, following the proper cone angle.  Same applies for external, no need to try hard and pre-mill a cone (well, that is if you have a full form threadmill, not with single point of course).  Most likely a lot faster to add 1-2 radial pass with the threadmill than interpolating a cone!

[engineguy]

@DarthBane55 

The OP has a full form thread mill for the job, yes, of course we have already all agreed that a single point thread mill is the way to go but as he has a tapered thread mill (Those are not cheap !!) he wanted to use it and was just asking how/what would happen if/when he did use it.

My little exercise is purely to try and show how it would turn out using a Vertical Mill, as the part is circular with a couple of flats which in my little workshop it would be done on the Lathe in a fraction of the time 🙂 🙂 🙂

I am not advocating the exercise is the way it should be done, just an example is all of how it could be done 🙂 🙂

P.S. As the full form Taper Thread Mill only does a one revolution it is quite fast, take longer to go round and round with a single point thread Mill ?? Yes ??

[DarthBane55]

@engineguy 

Sorry, was not trying to disagree with you, was just talking about my own experiences, and I might have lost sight of the original question in doing so.  I threadmill quite a bit on milling machines because we sometimes get some parts which are not round but have a few NPTs on them, "think T shape junction casting" type with NPTs on both ends of the T or whatever part like that, so for sure your exercise with milling machine is definitely something useful!

But... oops...  I did not agree to say single point is the way to go!  haha, sorry about that, but a full form NPT threadmill is much, much faster, and saves you time in preparation of the cone as well.  Again, this is only my personal experience, but I use single point only as a really last resort.  That being said, if you have 2 parts to make and don't have the full form threadmill, then it is not worth getting it, unless you anticipate having more parts in the future with the same thread.  Anyways, I'll put myself outside of your sentence "we all agreed that single point is the way to go", I really disagree on that one!  But as I said, there are exceptions, depending on how many parts you are making etc etc.  and it's only another opinion and not gospel truth!

For the last question, I'm not 100% sure if I understood right, but say you have single point, and you need 8 axial turn (example), and you want 3 radial passes, that is 24 turns around the part to make the thread.  Full form thread is 3 turns (3 radial passes), not even comparable.  Yes, you might go slightly slower in IPT, but that might come into play more in really hard materials, for aluminum and regular steels, it's not even a factor.

EDIT: I re-read your last question, and you basically are saying the same thing I just said lol 🤣 I wasted time on this!😉

[engineguy]

@DarthBane55 

🙂 🙂 Nice to see that "Great Minds think alike" 🙂 🙂

Yes, way quicker and easier to just go round 3 times with the full form instead of 33 times with the single point.

Having said that I would expect that most people would use the single point as being a darn sight cheaper and can be used on pretty much any angle, one single point will do the work of a fair number of  full form thread mills and if the user can balance the extra time using the single point against the extra shop time then good.

I have just a few holders that use have bolt on Carbide tips for different thread types/grooves that work well for me at pretty low cost (If that is possible from ISCAR !! 😞 😞 )

OK, now I`m juat rambling, apologies if I misspoke/misled 🙂 🙂

[leo.castellon]

Sorry for going slightly off topic, but how did you get the dxf file in as a tool? We use a quite a few custom tools and I really miss Mastercam's functionality in regards to this issue. Knowing how to do this would help me greatly.

LeoC

[engineguy]

@leo.castellon 

No problem, screencast link below of how to create the tool shown here 🙂

Screencast link :-  https://autode.sk/3BotGhf

Hope this what you are asking for, the Fusion File is attached for you just go though the steps in the Screencast to make as many as you like for practice 🙂 🙂 🙂

[leo.castellon]

Thank you kind sir!

LeoC