Thread Milling

This forum is dedicated to those Hobbyists Interested in CNC machining in their home shops. (Digital Read Outs are also topical, as is CAD/CAM as it relates to CNC)

Moderator: Harold_V

User avatar
GlennW
Posts: 6656
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Thread Milling

Post by GlennW » Sat Aug 04, 2018 2:55 pm

I always wanted to give it a try.

I had a job that needed external 1/8" NTP threads on stainless.

I have a really nice taper attachment for my lathe that I have never installed, so I tried cutting the pipe threads using a Geometric Die Head and it worked, but the results were not as nice as I had hoped.

Soon after, I bought a thread milling cutter for 27 tpi pipe threads and never got around to tinkering with that either...

Today I figured I would give it a try, and after figuring out all of the specs that I needed using an Optical Comparator since I had no info on the cutter, and trying to remember how to run my CNC mill, the first attempt was actually successful. :shock:
DSC01189.JPG
DSC01188.jpg
The L1 gauge actually likes it!
DSC01190.jpg
This was on aluminum bar, but it's a pretty good start, so next I'll try the stainless and see how it works out.

I may shorten it up one thread and reduce the diameter accordingly, but for now, it's not a problem.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

Harold_V
Posts: 17189
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Thread Milling

Post by Harold_V » Sat Aug 04, 2018 3:51 pm

Nice, Glenn!
I've always been curious about thread milling, but have not had a reason to pursue the process.
The thread mill looks a lot like a tap. Do you see any significant differences between the two?

H
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
GlennW
Posts: 6656
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Thread Milling

Post by GlennW » Sat Aug 04, 2018 4:03 pm

For one, there is no helix to it, as I ran it at 3700 rpm and 20 ipm feed and it just ran a spiral pattern down the stock equal to the thread pitch per helical orbit as if it was a single V cutter.

It's also Carbide.

I programmed 11 orbits since I plan on using it for stainless. If I was only cutting aluminum I would drop it down to two threads from full depth and only make two orbits using the length of the cutter to cut all of the threads.

Not sure any of that makes sense, but I understood it!
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

User avatar
Bill Shields
Posts: 5163
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Sat Aug 04, 2018 5:25 pm

thread mills are not like taps...and cannot be used as such.

for small IDs they are quite the way to go..or in as in this case one mill can make any OD you want as long as the pitch is correct (assuming it is a multi-tooth mill).

Single tooth mills can make literally any pitch thread - as long as there is enough back clearance to handle the helix.

You should see one of these things making 2 mm ID threads in titanium...

Harold_V
Posts: 17189
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: Thread Milling

Post by Harold_V » Sun Aug 05, 2018 3:56 am

Thanks, guys. I'm woefully lacking in CNC operations, but eager to learn.

H
Wise people talk because they have something to say. Fools talk because they have to say something.

User avatar
Bill Shields
Posts: 5163
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Sun Aug 05, 2018 7:43 pm

getting the thread mill in / out is a challenge, especially with an ID thread.

If using a single point tool, typically you helical mill down to depth, the make at least one full 360 degree arc move, then move radially until the tool is clear and pull it out of the hole.

The same can be applied to an OD thread if the design allows.

if using a multi tip tool (as shown here), you have to always move helically while cutting stock...then move away from the part

User avatar
AndrewMawson
Posts: 286
Joined: Sat Jan 04, 2003 5:46 pm
Location: Battle, East Sussex

Re: Thread Milling

Post by AndrewMawson » Mon Sep 17, 2018 3:32 pm

The late (and sadly missed) John Stevenson once showed a way of mounting an individual cutter from a die head on a slotted arbor and using it to thread mill external threads.
Andrew Mawson
Battle, East Sussex, UK

User avatar
ctwo
Posts: 2720
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Thread Milling

Post by ctwo » Mon Sep 17, 2018 7:40 pm

Single point threading on the mill sounds interesting. I might see what mess I can produce, with nothing more than a bit of creativity and lots of time. Maybe by January...
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

Geezer
Posts: 22
Joined: Wed Dec 13, 2017 7:14 pm

Re: Thread Milling

Post by Geezer » Tue Sep 18, 2018 12:34 pm

Climb Mill,
Start OD thread at top
ID thread at bottom


Single Point.jpg

User avatar
ctwo
Posts: 2720
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Thread Milling

Post by ctwo » Tue Sep 18, 2018 4:47 pm

That's awesome! Thanks! I typed that out and put into my mill program and it looks like one thread - enter and exit from the bottom up. I did have a problem with the G41 line and will look into that, I had to comment it out. Also, it looks like an inside thread, which was more interesting to me.

(I'm using Mach3 and found: Compensation has been changed in mill. In mill you need to have a lead in and lead out > 1/2 tool diameter before and after g41 & g42)

And here is text:

%
O1000
(X0Y0 is at center of hole)
(Z0 is at the top of the part)
T1 M06
G00 G90 G54 X0
T1 M06
G00 G90 G54 X0 Y0 S2500 M03
G43 H01 Z.1 M08
G01 Z-1.083 F35
(G41 X0.275DI)
G3 X0.875 I0.3 F15
G91 G3 I-0.875 Z0.0833 L14
G90 G3 X0.275 I-0.300
G00 G90 Z1.0 M09
G1 G40 X0 Y0
G28 G91 Y0 Z0
M30
%
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
Bill Shields
Posts: 5163
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Tue Sep 18, 2018 6:40 pm

DI or D1?????

Cutter compensation can be either for wear or full radius offset.

If doing wear, then the lead-in / out can be quite a small number because it only handles the difference between the programmed and actual tool.

User avatar
ctwo
Posts: 2720
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Thread Milling

Post by ctwo » Wed Sep 19, 2018 3:22 am

Ha, yes, D1 seems to solve one error message. Maybe I don't understand it well enough, of course. Mach does not seem to repeat the arc in the program, but I recall the machine does.

%
O1000
(X0Y0 is at center of hole)
(Z0 is at the top of the part)
T1 M06
G00 G90 G54 X0 Y0 S2500 M03
G43 H01 Z0.1 M08
G01 Z-1.083 F100
G41 Y0.251 D1 F15
G1 X0.275 Y0
G3 X0.875 I0.3
G91 G3 I-0.875 Z0.0833 L14
G90 G3 X0.275 I-0.3
G00 G90 Z1.0 M09
G1 G40 X0 Y0
G28 G91 Y0 Z0
M30
%
Attachments
mach3-g41-tool-offset.PNG
mach3-g41-tool-offset.PNG (6.21 KiB) Viewed 803 times
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

Post Reply