Thread Milling

Sorry to resuscitate this thread, but I can feel thread milling creeping up on me! I need to cut an M14x1 thread on the backplate for a collet chuck and found the turning tool I was planning to use won't quite fit. One option is to grind a bit off but there is much meat there anyway, and the tool lacks any top rake. I was wondering about making a tool from a tap then though, well, why not grind two flutes off and use my CNC mill to do the job? Interesting YouTube video here. Running the tap much faster will give a much lower tooth load and I shouldn't be so concerned with rigidity. It seems to me that I just need a tap for a 1 mm pitch which is smaller than the tapping size hole (13mm), correct? Obvious one is M6 but I may have a metric fine M8 or even M10 x 1 that could be used.

Anyone with any experience of doing this, please advise!

I would have thought that the smaller you go with the modified tap the more the helix angle will start to become an issue and rub behind the cut .

Plenty of M14x1 taps about too.

Found my invaluable tin of surplus taps had a nice M8x1 second HSS so it has shed 3 of its 4 flutes. Now to find out how to generate the code!

Helix angle of 14*1 is 1.4 degrees, for m8*1 it is 2.3 degrees. As Jason points out you might be in for a disappointment. Grinding a single point tool to go down an M14 hole wouldn't be difficult, you could use a bar with an insert cutter (broken taps are my favourite)

It is not so much the difference in helix angles between the finished thread and the tap used but the fact a thread mill has zero helix angle so there is no rubbing.

I have milled plenty of threads on my CNC mill but I use the single thread type thread mills. They cost around £50 but work very well.

Might want to check out either Cromwell or cutwel tools for that kind of thing. I'd imagine most M.E suppliers wouldn't stock thread mills.

Michael W

Fusion 360 supports thread milling, so that's one simple way to generate the code. I haven't got round to trying it myself yet but the cost of the tools is eye watering. On that basis, I'd want to be making my own tools first.

In Fusion, you can easily create your own form milling tools in the tool library, then use that to cut the thread.

If you are talking about a large diameter female thread that is effectively a very fine pitch, perhaps a standard internal threading insert tool would do the trick - used as a milling cutter. This sort of thing. All this discussion about taps, clearances, expensive single point tools etc would go away. Model it up as a milling cutter and off you go?

Murray

If you use Mach3 & possibly some other controllers, I've written a little program to do internal & external threads assuming a single point cutter (which could be made from silver steel). This is a windows 32 bit program.

Look forCNC thread milling here: www.chestnutpens.co.uk/misc/thread.html

Regards,

Richard

Most thread-mill manufacturers publish utities or web pages which generate thread milling code.

Hello Richard, I have emailed you via your web page - John.

A few years ago I got 2 single point thread mills from America via Ebay for sensible money, I've not looked to see if they are still available though.

They work very well and I use the threading wizard in Mach3, my first one was a twin start M6 brass bolt and it fit perfectly, the great thing about thread milling is you can mess with the mess with the sizing to get a nice fit if it only mating with the one thread.

Steve

Steve, that is what I find so good about using the threading wizard in either Fusion 360 or on the conversational programming on the Tormach mill. Adjustments are easily made but in general if I am using a standard recognised screw thread from a wizard it fits perfectly straight off.

Well, there are a couple of YouTube videos of people successfully thread milling with modified taps so I reckon it's worth a go. Richard's excellent utility starts from the bottom of the holes and climb mills out, so I suspect it might not be so good with a modified tap as it will start cutting on all the teeth which could be quite a load! Best I think to write code that starts at the top and spirals down. Sir John also says near the top of the thread that you can use a tap. Worth a punt I think, on a test piece first. Will report back.

Right! I generated the code using Richard's utility then hand-crafting the result to spiral downwards from the top, a relatively trivial change as it turned out (editing the gcode that is, not the utility itself). Drilled a 12.9mm hole in a miscellaneous bit of 3/4 mild steel bar, centred it on the Novamill table using my electronic centre finder, set the code running and bingo I had a threaded hole M14x1 about 5 minutes later. The thread looked very clean and fits the Unimat spindle well, first go, with little shake and a smooth action as you screw it on.

After some though I decided that the helix angle of the tap isn't really a problem. You have to remember that the tap is significantly smaller than the hole you are threading. Yes, in principle as the tap rotates the helix may cause some rubbing, but both the smaller tap radius and its form relief are quickly taking the cutter surface away from the work, as it were.

Thread milling rocks!

Well done, it's great watching the machine make such a nice thread isn't it.

The first time I used it was to correct a mistake when I accidentally used an M6 twin start tap I didn't even know I had so I had to create a brass bolt to fit.
I've been looking at jigging up a motorcycle cylinder head to thread mill the exhaust nut thread out to a larger size and make a new flange nut to suit but it didn't need to be done in the end.

Steve

Brilliant John.

Possibly I need to add a tickbox to the utility to tell it to mill the way you did it. Originally I had it working that way and changed it to climb milling because my cnc router/engraver can really only cope with climb milling.

Regards,

Richard

That would be really useful Richard, enabling the use of cheap modified taps, though I'm sure proper cutters will give a better result. Thanks, John.

John,

I'll see if I can do it sometime week beginning the 16th. Can't do it before then due to some deadlines I can't miss.

Regards

Richard

No hurry for me Richard, I have done the thread I needed for the moment. But having discovered that thread milling can be so straightforward I think I will be doing a lot more.