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
Bill Shields
Posts: 5271
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Wed Sep 19, 2018 6:24 am

motion repetition is not something supported by all software or controls.

User avatar
ctwo
Posts: 2730
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Thread Milling

Post by ctwo » Wed Sep 19, 2018 8:16 am

If I recall, I think I had to put the repetitious code in a subroutine and call that. Have to look it up. Mach was doing some strange things with cutter comp until I added a Y motion. I never tried that feature before so need to look into it. I might actually try cutting some threads before January now :D
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: 5271
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Wed Sep 19, 2018 10:43 am

SOME controls, when activating G41/G42 and going directly into a series of more than 2 arcs (as you are here) at a sharp included corner, 'loose track' of where they need to begin without having a Y component in the initiation line.

It is better (for the general control case), to initialize cutter comp on a short line, then have a small TANGENT ARC that joins the G41 line to the thread milling arc series...

If you do this, you will RARELY find a control that chokes on the code.

User avatar
ctwo
Posts: 2730
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Thread Milling

Post by ctwo » Wed Sep 19, 2018 2:34 pm

I could not figure it out because the tool would follow most of the initial small arc, but get closer to the edge and finally cross before it got to the large arc. Then, it fully reversed direction to pick up the large arc where it would cross at the left side...here is a figure I recreated from memory.

And not intending to derail the thread into a discussion about mach, but at least it's somewhat thread related. I figured I'd try to change the lead in and small arc to be tangent, so only 1/4 of a circle lead-in, especially since I'd expect my cutters to be closer to the hole diameter. Proposed paths shown in the figure, right side. My goal is to set up an Excel spreadsheet that takes the cutter diameter, hole diameter, and thread pitch and will produce the g-code. I could either rely on mach's cutter comp, or build it into my spreadsheet. My spreadsheet would produce a result as shown in the image. Mach will likely steer the cutter up (Y) from the lead in at the start to observe compensation on that path.
Attachments
mach3-g41-misfit.PNG
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: 5271
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Wed Sep 19, 2018 4:43 pm

This is a case of the control not knowing what to do with cutter comp as described earlier.

You might find it easier tp use G42 and put in a negative value for the offset. Some controls will handle it better.

Another way to handle this is to break it into quadrants..some controls handle the LOOK AHEAD better if you do.

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

Re: Thread Milling

Post by Geezer » Wed Sep 19, 2018 7:31 pm

This is just a sample, It works with my Mach3

%
O0
G17 G40 G80 G90
T1 M6
S2500 M3
G0 G90 G54 X0 Y0
G43 Z1. H1 M8
G0 Z-0.9833
G1 Z-1.0833 F30.
X0.0003
G41 X0.0002 D1
G3 X0.9496 Y-0.0287 I0.4747 J-0.0143 F21.509
Z-1. I-0.9496 J0.0287
Z-0.9167 I-0.9496 J0.0287
Z-0.8334 I-0.9496 J0.0287
Z-0.7501 I-0.9496 J0.0287
Z-0.6668 I-0.9496 J0.0287
Z-0.5835 I-0.9496 J0.0287
Z-0.5002 I-0.9496 J0.0287
Z-0.4169 I-0.9496 J0.0287
Z-0.3336 I-0.9496 J0.0287
Z-0.2503 I-0.9496 J0.0287
Z-0.167 I-0.9496 J0.0287
Z-0.0837 I-0.9496 J0.0287
Z-0.0004 I-0.9496 J0.0287
Z0.0829 I-0.9496 J0.0287
X0.95 Y0 Z0.0833 I-0.9496 J0.0287
X0.0002 I-0.4749 J0
G1 G40 X0.0003
G0 Z0
Z1.
M9
G28 G91 Z0
M30
%




CTWO
Verify.png

User avatar
Bill Shields
Posts: 5271
Joined: Fri Dec 21, 2007 4:57 am
Location: Somewhere in the World
Contact:

Re: Thread Milling

Post by Bill Shields » Wed Sep 19, 2018 8:56 pm

That's a good example of tangencies...but care that you wear offset cannot exceed 0.0001 -> which may not be enough

User avatar
neanderman
Posts: 709
Joined: Mon Jan 09, 2012 7:15 pm
Location: Cincinnati, Ohio, USA

Re: Thread Milling

Post by neanderman » Thu Sep 20, 2018 5:25 pm

A short video of this in use would be super cool. ;)
Ed

Le Blond Dual Drive
US-Burke Millrite MVI
Atlas 618
Files, snips and cold chisels

Proud denizen of the former "Machine Tool Capitol of the World"

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

Re: Thread Milling

Post by Geezer » Thu Sep 20, 2018 6:06 pm

I don’t have a video cutting the part.
Here’s the simulation and finished parts

https://www.youtube.com/watch?v=WWC3AjgiFd4

Leg Assy.JPG
Leg Assy.JPG (23.51 KiB) Viewed 1588 times
Upper mount.JPG
Upper mount.JPG (22.85 KiB) Viewed 1588 times
Foots.jpg

User avatar
GlennW
Posts: 6692
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Thread Milling

Post by GlennW » Wed Mar 06, 2019 6:27 pm

I'm liking thread milling a lot for stainless 1/8 NTP.
DSC01576.jpg
The next time I'm tinkering with it I'll shorten it up a thread or two and adjust the diameter accordingly.
Glenn

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

User avatar
Rich_Carlstedt
Posts: 1456
Joined: Sat Dec 21, 2002 12:16 am
Location: Green Bay Wisconsin USA

Re: Thread Milling

Post by Rich_Carlstedt » Sat Mar 16, 2019 10:58 pm

I have done many internal threads by milling .
I started in the early days by hand grinding a single flute carbide Router bit and putting a relieved 'V" in the bottom.
Worked fine, but now I buy single point thread cutters .
I like centering on the hole and going to the bottom first and doing a relief groove. Then I climb mill in the helix coming out of the hole.
This means I don't have to contend with swarf from the cut, and eliminates a possible crash because I went too deep.
Buying a commercial cutter means you can see your maximum depth and plan accordingly
Here is the type of cutter I am referring to.
https://www.mscdirect.com/product/details/05252036
The commercial (multi-thread endmill)) cutters or insert cutters are pretty pricey for me and these do a bang up job, plus they will do verry small holes, where as the inserts are at a disadvantage

Rich

User avatar
Rick
Posts: 435
Joined: Sat Jan 04, 2003 8:34 pm
Location: Stone Mountain, Ga.

Re: Thread Milling

Post by Rick » Mon Mar 18, 2019 10:46 am

I have done thread milling pretty much like Rich stated above. Done both with CAM (G-code) and by conversational programming on my Hurco which has a Helix feature.
Only difference than what Rich does is I use a single profile cutter in place of a single point cutter like he does.
https://www.mscdirect.com/product/details/57568883
Rick

“We make a living by what we get, but we make a life by what we give." Sir Winston Leonard Spencer Churchill (1874-1965)
"Peace is that brief glorious moment in history when everybody stands around reloading". Unknown
Murphy's Law: " If it can go wrong it will"
O-Tool's Corollary: "Murphy was entirely too optimistic"

Post Reply