[Doubleddaved]

I'm going to try for the first time thread milling and I can use some help.
Haas vf-8/50 5/8-11 blind holes in 316 stainless have a 5 flute thread mill with a .470 diameter. and I need to tap .635 deep and I have a .531.tap drill hole. I would like to take this in 2 passes.
I've been reading the older posts and looking at some of the free software out there but I seem to get different programs and since this is new to me I don't want to take a chance.I have 540 holes to thread.
If someone can post the code that is just for the Haas control for this I can go from there for this and other sizes in the future.
Thanks for any and all help and I continue to read posts on this site daily,and continue to learn on this 1 year old Haas.

Dave

[JWK42]

This is the way we program thread mill threads. This is based on X0. Y0. being the center of the thread and is in absolute mode. You could use G52 to shift program zero and put the thread milling portion in a local sub and call it with M97 P?


%
O5555 (TEST THREAD MILL)
N30 ( WRITTEN 09-11-2009 07:43:45 )
N40 (MODIFIED 09-11-2009 07:50:17)
N50 #101=1 ( 11-TPI THREAD MILL )
N60 G17 G54 G90
N70 G40 G49 G80
( TOOL #1 IS A 11-TPI THREAD MILL )
N90 G53 G00 Z0.0 ( RESTART TOOL #1 HERE )
N100 G53 G00 X-20. Y0.
N110 T#101 M6
N120 S1500 M3
N130 G54 G00 G90 X0. Y0.
N140 G43 Z2. H#101 D#101 M8
( START .625 MAJOR DIA - 11 TPI THREAD HERE )
( PROGRAMMED WITH .470 DIAMETER END MILL )
( SET TOOL RADIUS OFFSET TO ZERO )
( USE MINUS RADIUS TO INCREASE SIZE )
N190 G00 X0. Y0.
N200 Z.2
N210 G01 Z-0.635 F50. M8
N220 G41 X.0156 Y0. F10.
N230 G03 X.0639 Z-0.6294 R.0241
N240 G03 I-.0639 Z-0.5385
N250 G03 X.0156 Z-0.5328 R.0241
N260 G40 G01 X0. Y0. F50.
N270 Z-0.635
N280 G41 X.0293 Y0. F10.
N290 G03 X.0775 Z-0.6209 R.0241
N300 G03 I-.0775 Z-0.5299
N310 G03 X.0293 Z-0.5158 R.0241
N320 G40 G01 X0. Y0. F50.
N330 G00 Z2.
N340 G53 G00 Z0. M9
(UNLOAD HERE)
N360 G53 G00 X-20. Y0.
N370 M30 (END OF MAIN PROGRAM)
%

[anemachinebc]

this is how i thread mill, its very easy once you get the hang of it, and it is very easy to modify. It also works good for doing round holes. Just ad a Z to the code and you can spiral down. Very easy to put in to subs as well

say your hole is at X 1.0 Y-1.0

Go the the hole

G00 X1. Y-1.
Z.1
G1 Z0.F10.
G91 (INCRAMENTAL)
G1 Z-.635 (FEED TOOL TO BOTTOM OF HOLE)
G1 G41 D1 X.0775 (MAJ DIA - TOOL DIA/2)
G3 I-.0775 Z.0909 L8 (Z = 1/11 PITCH)
G40 G1 X-.0775 (FEED BACK TO CENTER)
G90 (BACK TO ABSOLUTE)
G0 Z1.

[JWK42]

If you have macros here is an example of milling the holes in a pattern.
It uses G91 incremental to make the threading cuts and absolute to position to the next hole.
I have only tested this on our simulator so make chips very carefully.


%
O5555 (TEST THREAD MILL)
N30 ( WRITTEN 09-11-2009 07:43:45 )
N40 ( RETURNED 09-11-2009 07:50:17 )
N50 #101= 1 ( 11-TPI THREAD MILL )
N60 G17 G54 G90
N70 G40 G49 G80
( TOOL #1 IS A 11-TPI THREAD MILL )
N80 G53 G00 Z0. ( RESTART TOOL #1 HERE )
N90 G53 G00 X-20. Y0.
N100 T#101 M06
N110 S1500 M03
( START .625 MAJOR DIA - 11 TPI THREAD HERE )
( PROGRAMMED WITH .470 DIAMETER END MILL )
( SET TOOL RADIUS OFFSET TO ZERO )
( USE MINUS RADIUS TO INCREASE SIZE )
N120 #601= 1 ( START OF 1ST ROW IN X AXIS )
N130 #602= 1 ( START OF 1ST ROW IN Y AXIS )
N140 #603= 2 ( STEP OVER IN X BETWEEN HOLES )
N150 #604= 0 ( STEP OVER IN Y BETWEEN HOLES )
N160 #610= 5 ( NUMBER OF HOLES )
N170 #620= #610
N180 G54 G00 G90 X#601 Y#602
N190 G43 Z2. H#101 D#101 M08
N200 WH [ #610 GT 0 ] DO1
N111 M97 P370
N210 #610= [ #610 - 1 ]
N220 #601= [ #601 + #603 ] ( CHANGE X AXIS HOLE LOCATION )
N230 #602= [ #602 + #604 ] ( CHANGE Y AXIS HOLE LOCATION )
N250 END1
N260 #601= 1 ( START OF 2ND ROW IN X AXIS )
N270 #602= 4 ( START OF 2ND ROW IN Y AXIS )
N275 #610= #620
N280 WH [ #610 GT 0 ] DO1
N111 M97 P370
N290 #610= [ #610 - 1 ]
N300 #601= [ #601 + #603 ] ( CHANGE X AXIS HOLE LOCATION )
N310 #602= [ #602 + #604 ] ( CHANGE Y AXIS HOLE LOCATION )
N330 END1
N340 G53 G00 Z0. M09
(UNLOAD HERE)
N350 G53 G00 X-20. Y0.
N360 M30 (END OF MAIN PROGRAM)
N370 (THREAD MILL HERE )
N380 G54 G00 X#601 Y#602
N390 Z0.2
N400 G01 Z-0.635 F50. M08
N410 G91
N420 G41 X0.0156 Y0. F10.
N430 G03 X0.0482 Z0.0056 R0.0241
N440 G03 I-0.0639 Z0.0909
N450 G03 X-0.0482 Z0.0056 R0.0241
N460 G90
N470 G40 G01 X#601 Y#602 F50.
N480 Z-0.635
N490 G91
N500 G41 X0.0294 Y0. F10.
N510 G03 X0.0482 Z0.0056 R0.0241
N520 G03 I-0.0775 Z0.0909
N530 G03 X-0.0482 Z0.0056 R0.0241
N540 G90
N550 G40 G01 X#601 Y#602 F50.
N560 G00 Z2.
N570 M99
%

[Superman]

Seco tools have a thread milling program that allows you to cut and paste into a program

On the same page is other progams to download for "special toolpaths"

PS --- no cost

The link