Threading and Tapping
Thread Milling Macros
Dear Readers,
A Haas distributor recently sent us this handy macro program, which can be used to thread mill just about any size thread with any size tool. We liked it, so we decided to pass it on to you.
%
O0001
...
G00 G40 G54 X0 Y0
T1 M06
S1000 M03
G90 G43 H01 Z0.5 M08
G65 P1234 D1.98 C0.5 E0.0556 Z-0.75 F15. M2
G65 P1234 D2.0 C0.5 E0.0556 Z-0.75 F15. M2
G00 Z1.
M05
...
M30
O01234
(MACRO - ID RIGHT HAND STRAIGHT)
(THREAD MILLING WITH MULTI-POINT)
(TOOL)
(C=#3 CUTTER DIA)
(D=#7 PASS DIA)
(E=#8 LEAD)
(Z=#26 Z DEPTH)
(M=#13 Z LEAD UP LOOPS)
G103 P1 (HALT LOOK AHEAD)
(BLANK LINE)
(BLANK LINE)
IF [#13 EQ #0] THEN #13=1
G01 Z[#26]F20. (FEED TO BOTTOM)
#32=[#7-#3]/2 (CALC CUTTER PATH)
#9=[#9*[#32/[#7/2]]] (CALC FEED RATE CENTER OF CUTTER)
G03 X#32 I[#32/2]J0 F#9 (APPROACH)
WHILE [#30 LT #13] DO1
#30 = #30 + 1
G03 I[-#32]J0 Z[#26+[#8 * #30]]
(THREAD MILL UP)
END1
G03 X0 I[-#32/2]J0 (ESCAPE)
G103 (RESUME LOOK AHEAD)
M99
%
Sincerely, Haas Applications