Thread milling ?

[Wal]

Hi all,

I'm also hoping to have a go at this - I had a play around with writing the G-Code for it earlier in an effort to better understand what's going on, I've got something that might work - I wouldn't mind a bit of a sanity check on my process, though...

For the sake of argument I'm going to be cutting an M4 thread. For the cutting tool I'm going to use an M4 tap ground down to a flat nose / single row of cutting teeth - I'll be using this tool for both the internal and external threads, but when cutting the external thread I'll adjust the radius to cut me a slightly deeper groove for a bit of clearance (...maybe I'm better off doing that on the internal thread..?)

These threads don't need to be ISO compliant, so long as they work together that'll be fine!

Here's the code I came up with for the external thread (probably ought to be a G17 in there..) along with a vid of Linux CNC running it:

%
G90 G21 G40 G49 M6 T1
G0 X0 Y0 Z5
G0 X-5
G1 Z0 F500
G1 X-3.571
G2 X0 Y-3.571 Z-3.5 I3.571 J0 P5 F500
G0 X-5
G0 Z5
G0 X0 Y0
M2
%

(The radius of the arc is 3.571 as that'll bury a 4mm tap 0.429mm (male thread height) into the 4mm stock to be threaded.



Does all of this look about right, or wishful thinking..? I guess I'll just have to give it a go..!

Wal.

[magicniner]

My CAM uses a radius lead-in to the starting point

[JohnHaine]

I suggest that you start with a bigger thread, seems to me that an M4 tap may be quite flimsy by the time you have ground off 2 or 3 of the rows of teeth. Also it won't give you much clearance in an M4 tapping hole. You do of course need to use a tap with the same pitch as the thread you want which is limiting. I was lucky using a modified tap as I wanted an M14 x 1 thread and had an M8 x 1 tap.

As for the code, I suggest you look at Richard's wizard that I linked to in an earlier post as an example for comparison.

[Wal]

Cheers guys.

Yep, going to try feeding in tangentially as opposed to crashing in to the side like that..!

Hi John - yeah, I've had a play with the Chestnut Pens app - very good it is too. I'm having a go from scratch as I'm a noob when it comes to G-Code and fancy getting my pea-brain around it a bit better. Seems to me that the main difference with how Richard's app works is that he uses full circles and increments the Z at each line, where I'm asking the machine (using 'P') to make a set number of circles while the Z moves as it's doing doing that.

Well, I've ground down a cheap M4 tap, gonna stop my procrastinations and give it a go on a bit of brass... I'm reasonably confident it won't work, but ya gotta start somewhere..!

Wal.

[JohnHaine]

Well I hope it goes OK - the worst can happen is you break a cheap tap, at least it won't be stuck in the hole! First time I tried I was amazed how easy it went, and thread fitted first time.

[Wal]

Well, I'm pleased to report that things went alright... I didn't video my mill doing the deed, so to speak, but the results are below - you can see how I modified the tap in the second clip. Turns out I didn't need to feed in tangentially, I'm coming in from above so it makes no real difference... It's a decent fit but was a little tight to begin with - nothing that running the nut over didn't sort, though.

I'm quite chuffed with the results here - but yeah, of course, it's a hack. CZ121 is forgiving and I wouldn't fancy the chances of this going as well on something harder..! Certainly gets me out of a hole for a little project I've got on the go at the moment.



Wal.

EDIT - in action:

[JohnHaine]

Nice!

[Clive S]

Wal Great job. who would have though it.