Thread milling ?

[Leadhead]

John - Thanks for the info. I actually just bought similar from Banggood. (SNR0013M16 Lathe Turning Tool Holder with 10pcs 16IR AG60 Inserts) Suited my budget at £15.31 with ten inserts included. It will serve to cut my teeth on. Will report on the efficacy.
I use many of their lathe tools and inserts and have found them good value for money. Have cut Titanium for instance,(gently) to good effect. I have no connection with them, just sometimes like relatively good cheapo`s for rarely practiced applications .
Confess this is more an interest in "how to do it" than actual immediate need. May need some foam.

[JohnHaine]

I just started with a chunk of bms.

[JohnHaine]

Tap.



If using a tap I think you have to mill down from the top. With a single point tool you can climb mill from the bottom of the hole.

[Neale]

Out of curiosity, how do you measure the effective diameter of the boring tool used for thread milling? I assume that you need this parameter for the CAM tool you are using? I have one of those internal threading tools for use on the lathe but until - eventually - I get my CNC mill conversion done, it's all a bit academic for me...

[Leadhead]

I simply drill a hole in some MDF about the size of the cutter dia. Harden it with CA glue and finish bore it with the tool. Then measure the hole carefully. This gives me my offset.

[Leadhead]

Should have said to be careful with various tool tip radii. These will of course vary the cutting dia and thus the depth of the form when trying to match an existing thread. Imagine a huge tip radius verses a tiny one. The V form would cut in different places. Start small and creep up on it.

[JohnHaine]

Best if you download and look at the little app that Richard has on the Chestnut Pens website - that defines the dimensions that you need. I measured mine by clamping the tool in a vee block and careful use of a digital height gauge, it was very quick. The app is designed for metric threads so it calculates dimensions from the standard formulas - it would presumably work for UNF, but I don't think it would for imperial 55 degree forms.

[JohnHaine]

One of the benefits of using a TCT threading tool or a tap is that it already includes the flat or radius. I just used the app, chose my fit class, and it worked.

[Leadhead]

John - My caution above is born of trying to use standard 55 deg trapezoidal tips which do not always, of course, have a compatible tip radius. Tripped me up until the penny dropped, but close approximations can be found if you search. I have tried it on the CA hardened MDF only so far. But reproduced a heavy Whit. thread quite well,

[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.