The Home Machinist!

I have watched several videos on threading on a CNC mill. Looks easy enough. There must be a simple G76 type code for it. I have the CNC mill but not the lathe. Anyone done it? If so how?

John B.

P.S. I forgot I use MachIII and a cheap mill.

_________________
http://www.ngshay.com/
Shay drawings and castings

I have a 1/8 NPT thread mill I have not yet used, but I programmed X,Y Z coordinates to the location, then then a couple of G2 X,Y,Z helix moves to follow the pitch. I have also programmed a single disc thread mill to run in a tapered spiral for milling tapered pipe threads, but it takes a bit of code to do that and is a single pass deal.

Don't have a Canned Cycle for it, as I don't have a synchronous spindle.

For tapping I use G84 with a floating tap holder.

Industrial controller, Not mach 3.

I'm having to scratch my brain a bit as I haven't even powered up the CNC mills yet this year...

_________________
Glenn

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

Never actually tried it but I had a co-worker tell me how he did it. Use a G02 to make a circle. At the same time have "Z" advance downward an amount equal to the pitch of the thread. Then repeat but increase "Z" to the next thread. A 3 axis machine running a 3 axis program should do it.

For a thread cutting tool he used a boring bar fashioned into the shape of a toolbit for threading. Then mounted the boring bar into a boring head. He increased the thread size by adjusting the boring head then ran the same program again. Remember to move the cutting tool toward the center of the hole before withdrawing the tool.

I did not see it but I heard it worked great.
Jim

_________________
Tool & Die Maker/Electrician, Retired 2007

So much to learn and so little time.

www.outbackmachineshop.com

The makers of thread mills often have sample programs for using them on their websites. Google is your friend!

cheers,
Michael

Thread milling is a way of life with our machines and small threads (think 1.5 mm internal threads in titanium - and forget taps).

Thread milling is not typically done with a canned cycle (there are probably exceptions). I seem to remember that the old FADAL control had something that did threads. The SIEMENS control also does straight and taper threads if your control has CYCLE90 active. (it is in the 840D version).

If the control supports HELICAL motion, then it is done that was as G2 / G3 XYZ..where for a Z oriented tool, the Z value is whatever % of the pitch needs to be moved during the arc (typically 1/4 or 1/2 or even a full pitch for 360 arc).

HOWEVER:

Caution as FANUC controls do not support use of -R values with helical moves of 180 degrees or larger, so if you are programming this, you must program with IJK instead...and HELICAL motion is an extra $$ option on FANUC controls.

Also, there are issues with cutter compensation (G41/G42) and helical motion for some versios of firmware, so I don't usually recommend using G41/G42 with helical motion unless you KNOW you control does it properly.

If you are programming a PIPE thread, then (again unless you control has a cycle), and have a single-point tool, you need to program it as a bunch of little 3D lines and forget arcs since you cannot change the radius of an arc 'on the fly'. I have (occasionally), taken a pipe thread and broken the arcs into 1/4s or 1/8s and programmed increasing / decreasing arc radius arcs, thereby 'simultating' a continuously changing radius thread - without complaint. It makes the program a lot shorter but requires a lot of tricky math because the center of each arc segment must be shifted to similate the decreasing radius from start to finish.

Alternately, if you have a tapered thread mill, and the horsepower to drive it, you can make a complete thread in one rotation, allowing the taper of the tool to create the taper of the thread.

i had to thread the end of some 8" dia aluminum housings with an external 4 pitch thread, or .250 lead, an inch long. my lathe control only supports g32 with the thread tool always remaining in the center of the thread groove, this can (does) result in chatter problems that worsen the deeper you get. i had never thread milled, but over to the 3 axis cnc knee mill i went, to figure it out. disregarding thread depth issues to keep it simpler, figuring an 8 dia circle, it worked like this:

8" circle, so radius is 4"

cutter (a 60 deg 4 dia 36 tooth sidemill on a stub arbor) so cutter rad is 2"

circle i need to swing is 6" rad (part rad plus cutter rad). i need to be off the part and feed into it, also wanted to start my cut above the part, so it all blended nicely on the end pc the part. i chose to start 1 full thread lead above the part as not to hit anything. the essential moves look like this (balance of comments will be in caps so i can use the cap lock key) (ALL TEXT IN PARENTHESIS ARE NOTES AND COMMENTS):

G0 X7 Y0 Z2 (RAPID TO 2" ABOVE PART AND OFF THE RH SIDE)
G0 X6.3 Y0 Z.25 (ANOTHER SAFE RAPID MOVE TO GET ME CLOSER)
G1 X6 Y0 (FEED TO DIA)
G2 X6 Y0 Z0 I-6 J0 (MILL A CIRCLE WITH A CONSTANT .25 Z PLUNGE) ( SEE I AND J COMMENT BELOW)
G2 X6 Y0 Z-.25 I-6 J0 (MILL THE 1ST THREAD)
G2 X6 Y0 Z-.5 I-6 J0
G2 X6 Y0 Z-.75 I-6 J0
G2 X6 Y0 Z-1 I-6 J0
G0 X7 (CLEAR THE PC)
G0 X10 Z4 (RAPID MAKE SOME ROOM TO REMOVE THE PART)

(I AND J ARE THE DISTANCE AND DIRECTION FROM WHERE YOU ARE TO THE CIRCLE CENTER, IF IT MAKES NO SENSE, TIME TO LEARN IT, ITS IMPORTANT)

THIS IS SPELLED OUT MOVE BY MOVE, A LOT OF CODE, MUCH OF THIS INFO IS MODAL AND REMAINS REMEMBERED, THE SAME UNLESS CHANGED. CLEANED UP FOR SAVING MEMORY, IT LOOKS LIKE THIS:

G0 X7 Y0 Z2
X6.3 Z.25
G1 X6
G2 Z0 I-6 J0
Z-.25
Z-.5
Z-.75
Z-1
G0 X7
X10 Z4

lots of room for improvement, but it gets it done. easy to make the 1st part a lil over pitch, then make adjustments. the customer provided a gage to fit to, but had to send a couple back, these were replacement parts for 50 yr old machines, and the old machines werent exactly the same. thank God they were at least the same pitch, and it was easy to pick up the returned parts and skin off a few more thousandths.

ea part took about 30 minutes, i was able to do other things while they were running.

my day job is on a big 4 axis hor work center, we mill most any thread over an inch dia or so. i like it. go gage getting a bit snug? cutter comp a couple tenths, back to perfect threads.

hope this helps!

(edited much later...I values wrong, shortened "cleaned up" version....errors likely induced by newcastle ale...)

.

Thanks for the input.

I found the threading wizzard that comes with Mach III.
Use a single point thread milling cutter. It works slick.

John B.

_________________
http://www.ngshay.com/
Shay drawings and castings