What's new
What's new

Thread Milling Help Needed

athack

Stainless
Joined
Nov 2, 2009
Location
Michigan USA
Hello,

Trying to mill an internal M16-1.0 left hand thread. The hole is blind and is .236" deep. Need to thread as close to the shoulder as possible. I have never thread milled before and the manual is not helping.

Please if someone could post the code to do this I would be most appreciative.

Thanks Athack
 
Is it .236 deep to the shoulder or to the drill point? Do you have a single tooth threadmill or one with multiple tooth? What's the OD of the cutter? I'll give it shot and post the code if you get me this info!! You said left hand thread right?

HTH
 
Last edited:
Is it .236 deep to the shoulder or to the drill point? Do you have a single tooth threadmill or one with multiple tooth? What's the OD of the cutter? I'll give it shot and post the code if you get me this info!! You said left hand thread right?

HTH

HTH,

Thank you... the depth is .236 to a shoulder. Multi tooth mill and the OD is .370. Yes the thread is lefthand.

Thanks a ton.

Athack
 
Here you go:

O0000( T )

(PROGRAM NOTES)
(X = 0 AT )
(Y = 0 AT )
(Z = 0 AT )
(NOTES : )

(TOOLS LIST)
( T1 | .370 DIAM X 1 MM PITCH THREAD MILL | H1 | D1 | WEAR COMP | TOOL DIA. - .37 )

G20
G0 G17 G40 G49 G80 G90
( .370 DIAM X 1 MM PITCH THREAD MILL | TOOL - 1 | DIA. OFF. - 1 | LEN. - 1 | TOOL DIA. - .37 )
( THREAD 16 X 1.00 ID LEFT HAND THREAD )
T1 M6
G0 G90 G54 X0. Y0. S1200 M3
G43 H1 Z1.
M8
Z.1
G1 Z-.23 F50.
G42 D1 Y.05 F10.
G2 X.0375 Y.0625 Z-.2272 I.0375 J-.05
X.1 Y0. Z-.2202 I0. J-.0625
X0. Y-.1 Z-.2104 I-.1 J0.
X-.1 Y0. Z-.2005 I0. J.1
X0. Y.1 Z-.1906 I.1 J0.
X.1 Y0. Z-.1808 I0. J-.1
X.0375 Y-.0625 Z-.1738 I-.0625 J0.
X0. Y-.05 Z-.1709 I0. J.0625
G1 G40 Y0.
Z-.23 F50.
G42 D1 Y.075 F10.
G2 X.04 Y.085 Z-.2277 I.04 J-.075
X.125 Y0. Z-.2202 I0. J-.085
X0. Y-.125 Z-.2104 I-.125 J0.
X-.125 Y0. Z-.2005 I0. J.125
X0. Y.125 Z-.1906 I.125 J0.
X.125 Y0. Z-.1808 I0. J-.125
X.04 Y-.085 Z-.1733 I-.085 J0.
X0. Y-.075 Z-.1709 I0. J.085
G1 G40 Y0.
Z-.23 F50.
G42 D1 Y.0775 F10.
G2 X.0402 Y.0873 Z-.2277 I.0402 J-.0775
X.1275 Y0. Z-.2202 I0. J-.0873
X0. Y-.1275 Z-.2104 I-.1275 J0.
X-.1275 Y0. Z-.2005 I0. J.1275
X0. Y.1275 Z-.1906 I.1275 J0.
X.1275 Y0. Z-.1808 I0. J-.1275
X.0402 Y-.0873 Z-.1732 I-.0873 J0.
X0. Y-.0775 Z-.1709 I0. J.0873
G1 G40 Y0.
Z-.23 F50.
G42 D1 Y.08 F10.
G2 X.0404 Y.0896 Z-.2278 I.0404 J-.08
X.13 Y0. Z-.2202 I0. J-.0896
X0. Y-.13 Z-.2104 I-.13 J0.
X-.13 Y0. Z-.2005 I0. J.13
X0. Y.13 Z-.1906 I.13 J0.
X.13 Y0. Z-.1808 I0. J-.13
X.0404 Y-.0896 Z-.1732 I-.0896 J0.
X0. Y-.08 Z-.1709 I0. J.0896
G1 G40 Y0.
Z-.23 F50.
G42 D1 Y.08 F10.
G2 X.0404 Y.0896 Z-.2278 I.0404 J-.08
X.13 Y0. Z-.2202 I0. J-.0896
X0. Y-.13 Z-.2104 I-.13 J0.
X-.13 Y0. Z-.2005 I0. J.13
X0. Y.13 Z-.1906 I.13 J0.
X.13 Y0. Z-.1808 I0. J-.13
X.0404 Y-.0896 Z-.1732 I-.0896 J0.
X0. Y-.08 Z-.1709 I0. J.0896
G1 G40 Y0.
G0 Z.1
Z1.
M5
G91 G28 Z0. M9
G28 Y0.
M30

This is for a M16 x 1.0 Left hand Id thread, positioned at X0., Y0. it makes 2 rough passes @ .03 per side ea, 2 semifinish @ .005 and 1 spring pass, just in case lol! Since this thread is positioned at origin, you should be fine but adding/subtracting your hole position's for it on X & Y accordingly. Or just send them back :)

HTH.
 
Thank you...when I go to run the program I get alarm "369 TOOL TOO BIG"...any ideas?

Thanks Athack
 
Last edited:
to be honest, I don't know, What machine is this going in to? My sample code was for a Haas/Fanuc controller. Another idea that comes to mind is, Are you working on Metric or is it just for this thread, I guess you have realized my program sample is all on imperial units.

Let me know what else I can do.

Edit, do you have any values entered on your tool diameter offsets, as if you were using control cutter comp? Leave them both on zero and try it again, JUST REMEMBER TO RUN IT UP ABOVE THE PART FIRST..

HTH
 
HTH,

Thanks a ton...I set diameter offset to zero and it worked. Thread was too small, adjusted the offset and bang right on. What did you use to generate the code? Again thanks a ton you're a life saver, well a production saver anyway.

Athack
 
Not a problem, we do quite a bit of threadmilling here so I'm used to program them. I used Mastercam but I believe any other CadCam package would do it. I remember using a Macro for this on one of the shops I worked before. Also I believe you can go to some threadmill supplier's sites and download some Excel files that would give you the code you need.

Sorry I can't be much of help, I know for sure one of the distributors showed it to me once but I don't recall the brand it was.

By the way, HTH = Hope That Helps
 
What an awsome post!

Within a couple hours this was figured ou!

The thread just caught my eye as we are getting more and more into thread milling with real large threads or what we just learned to do thread mill in 55rc steel.
 
Hello,

Trying to mill an internal M16-1.0 left hand thread. The hole is blind and is .236" deep. Need to thread as close to the shoulder as possible. I have never thread milled before and the manual is not helping.

Please if someone could post the code to do this I would be most appreciative.

Thanks Athack


Your first and primary question was how to get close to the shoulder. That is maybe the easiest part. Move into the hole the desired distance/depth with your cutter. You sound like you have the same cutter that I usually use, four point carbide single point tool that is about .375 wide. So go into you hole the .236 distance or minus a few for safety, like .230, then mill up and out not down and in. That way you have the maximum depth and you do not have to worry about hitting the bottom.

As far as the code, with the Haas you can do it with just a few lines. Use a circular move out to the start and then a single line of code for the thread milling. The example below is not for you thread, just an example.

G00 X0. Y0. (go to whatever location)
G01 Z-1.083 F10.(move into your hole the depth you wish)
G41 X.275 D01(move to invoke cutter comp)
G3 X.275 I.3 F15.(small circular move into the material, could be a straight line if you wanted)
G3 G91 I.875 Z.0833 L14(puts mill into incremental mode, mills thread with 14 loops each moving up pitch distance of the thread to clear the hole)
G90 G3 X.275 I-.3(back into absolute mode and circular move out of material)
G00 G40 X0. Y0.(back to start and cancel cutter comp.)

If you can mill in one pass, you are done. If you need more just repeat with different I values etc..

Just food for thought.

Mike
 
Hello,

Trying to mill an internal M16-1.0 left hand thread. The hole is blind and is .236" deep. Need to thread as close to the shoulder as possible. I have never thread milled before and the manual is not helping.

Please if someone could post the code to do this I would be most appreciative.

Thanks Athack

Here's another solution helical interpolating through 360 deg, rather than quadrants as in the Mastercam example of Post #4

G00 X0.0000 Y0.0000
G43 Z0.500 H01
G01 Z-0.230 F50.0
G01 G42 X0.2017 Y0.2017 D01 F8.0
G02 X0.3150 Y0.0000 I-0.1230 J-0.2017 Z-0.2236
G02 X0.3150 Y0.0000 I-0.3150 J0.0000 Z-0.1842
G02 X0.2017 Y-0.2017 I-0.2362 J0.0000 Z-0.1778
G40 G01 X0.0000 Y0.0000
G00 Z0.500

The disadvantage in starting at the bottom of the hole with a LH thread, is that you will be conventional milling rather than climb milling. If you can be sure of evacuating the Swarf from the hole during cutting, you could start the distance of the ramp in and out of the thread, plus one thread lead from the bottom of the hole and helical interpolate in a Counter Clockwise direction. In this case you would use Cutter Radius Compensation to the Left and the cutting method will be climb milling.

If you don't have a CAM system, thread milling programs using the Helical Interpolation function of the machine, are fairly easy to create manually. The only real calculations made are to find the ramp in and out locations, where simple Trigonometry is used.

Regards,

Bill
 








 
Back
Top