MEW 342 CNC thread milling

[Ian Johnson 1Participant @ianjohnson1]

<p style=”text-align: left;”>Not posted for a while, but the article about CNC thread milling in August MEW No.342 by Bob Reeve interested me.  For some time I have wanted to do some thread milling on my little Sieg KX1,  I use Vectric Vcarve 10.5, which has thread milling capabilities, although I’ve not used this part of the software so far,  the program from Bob’s article will be a useful alternative.</p>
Looking forward to the next part

Regards IanJ

[JasonBModerator @jasonb]

I only skimmed over it, seems a lot of g-dode in there when it can be done with a few clicks of the mouse in a CAM program. I’ve only done a little using F360 and it was quite simple to do.

Be wary of using such large diameter cutters a sthey may not have sufficient clearance which will then produce the wrong profile.

The full form internal cutter mentioned at the end is not just suitable for M10 x 1.5 it can cut any diameter metric thread at 1.5mm pitch provided it will fit down the hole.

[John HaineParticipant @johnhaine32865]

There is also a good program available here:

http://www.chestnutpens.co.uk/misc/index.html

No need for a CAM program (but if you have one fine).

This just requires you to input the required thread parameters, press a “button”, and it spits out the g-code.  It has an option (which I requested) to start either from the bottom of an internal thread (which is climb milling and easier on the machine, but needs a single-point tool), or the top (which can be done with a tap smaller than the hole, possibly with some of the flutes ground off).

I haven’t tried external thread milling but internal is a blast.  I have used both, a ground away tap and an internal carbide threading tool.  As Jason says, either can be used on any metric thread of the same pitch.

[Ian Johnson 1Participant @ianjohnson1]

Sounds like I need to butcher some old taps!  Don’t fancy spending a fortune on a purpose made cutter only to crash and burn on the first cut!

I’ll have a look at that program thanks John

IanJ

[JasonBModerator @jasonb]

They can be had for a few quid, the single ring of teeth style are not expensive just have a look for that same make. Also faster as you get about 5 teeth not one so feed rate can be 5x greater than a chopped about tap

[John HaineParticipant @johnhaine32865]

<p style=”text-align: left;”>I used a standard 8mm shank insert threading tool from JB, feeding from the bottom.  Where have you seen cutters for a few quid please Jason?</p>

[JasonBModerator @jasonb]

Mr Ali will send then express delivery for less than one crispy one.

I have one from APT which was about £30 will fit into a 5mm hole so can do M6 or larger this is it in action

 

[NealebParticipant @nealeb]

…and the single-ring thread mills will cover a range of pitches, unlike the three-ring cutters which are for one single pitch. But the latter do create a fully-formed thread, of course. The single-ring are the equivalent of single-point cutting a thread in a lathe – crests are not dealt with correctly.

I bought a single-ring cutter when I needed to make a left-hand M10 external thread. I first had to make an internal thread to use as a gauge but both threads went well. The biggest issue was calculating thread depth to cut (using F360) to allow for the fact that the cutter tip was presumably sized for the thread at one extreme of its range (the finest thread?) and not the thread I was cutting. Did a couple of trial pieces in scrap first and it all came out well.

I have seen a suggestion that one reason for thread-milling internal threads rather than tapping is that in a complex and expensive workpiece, a broken thread mill is easily retrieved when a broken tap might be a real issue.

[John HaineParticipant @johnhaine32865]

Also I guess a thread mill will work in a CNC mill without rigid tapping, which needs spindle sync; and is probably faster since the cutter can run at a high speed not related to the Z feed rate.

[Martin ConnellyParticipant @martinconnelly55370]

…and with CNC thread milling you (normally, for a right hand thread) go from the bottom of a hole to the top so the chips fall down and away from the cutter. It is also better for fully formed threads further down a blind hole than can be achieved with standard taps.

You can also make the groove for a Helicoil without having the special Helicoil tap.

Martin C

[John HaineParticipant @johnhaine32865]

And for a LH thread too surely?  Though you would not then be climb milling but the opposite.

[HuubParticipant @huub]

I just started thread milling on the CNC router.  I use FreeCad where you can select an internal or external thread size and it shows the min and max diameter that can be used to mill the inner or outer to the appropriate size.

I made a few thread mills using a steel bar and soft soldered a HSS tool bit on the end. Ground the tip to the required 60° (metric) and it works pretty well.
A lathe inner threading tool holder SNR0010K11 holds an IR11 insert. The tool holder shaft is 10 mm in diameter and can be shortened to fit the CNC. The minimal bore diameter should be 13 mm. I measured the “center height” and found it to be 0.05 mm (0.002″) of center. That is more than adequate to mill decent threads.

For really small threads, you can grind a steel nail ( 2 mm shaft, 4 mm head), one of the projects on my list.

Chinese web shops sell thread mills for a few €. These are good enough to try thread milling.

 

 

[Author]

Posts