Thread Mills     Centers     Form Tools     Custom Manufacturing     Home
Other Tools     Thread Mill data     Dealers' and Industry Links     Contact us

Thread Milling Formulas

Finding Programmed Diameter Feed Rate O/D Finding Programmed Diameter Feed Rate I/D Ramping In 90 Degrees Ramping In 180 Degrees Internal threadmilling macro for Fanuc™ 0M controls Technical and Customer Support

Programmed Diameter Feed Rate O/D

When thread milling, your linear feed must be converted to circular feed

Schmarje Tool Co. 06/10/98 M. Berry

TO TOP

Programmed Diameter Feed Rate I/D

When thread milling, your linear feed must be converted to circular feed

Schmarje Tool Co. 06/10/98 M. Berry

TO TOP

Schmarje Tool Co. Drw. No. 03-117A M. Berry

TO TOP

Schmarje Tool Co. Drw. No. 03-247A M. Berry

TO TOP

Internal threadmilling macro for Fanuc™ 0M controls
By Kelly D. Grills, KDG-Engineering

This macro works with both single point and multi tooth cutters.

My goal was to eliminate the calculations required for our operators to perform thread milling, thus providing increased productivity.

The macro basically does a radial lead in move, helical movement to machine the thread, and a radial lead out.  I typically utilize a modal macro call (G66), which causes the macro to be executed as any standard drill cycle.

Download the macro here

The parameters needed by the macro are:
P9020   the macro's name
D   major diameter
F   feed rate
H   CRC register
R   number of revolutions of the tool path
        For single point tools, the number of threads to mill
        For multi-pitch tools, normally 1
T   pitch
Z   depth (length of thread)

A typical call (1/4-20 Thread) would look as follows:
(MODAL-MACRO-CALL)
G66P9020D.25F10.H11.R1.T.05Z-.25
()
(LOCATIONS-TO-MACHINE)
X1.Y1.
X-1.
Y-1.
X1.
()
(CANCEL-MODAL-MACRO)
G67

The macro itself:
O9020
(FANUC-0M-CONTROLLER)
(INTERNAL-THREAD-MILLING)
(CALLED-AS-FOLLOWS)
(G66P9020D.25F10.H11.R1.T.05Z-.25)
(D-MAJOR-DIA)
(F-FEED-RATE)
(H-CRC-REGISTER)
(R-REVOLUTIONS)
(T-PITCH)
(Z-DEPTH)
()
(VALIDATE-INPUT)
IF[#7EQ#0]GOTO7(MAJOR-DIA)
IF[#9EQ#0]GOTO9(FEED-RATE)
IF[#11EQ#0]GOTO11(CRC-REGISTER)
IF[#18EQ#0]GOTO18(REVOLUTIONS)
IF[#20EQ#0]GOTO20(PITCH)
IF[#26EQ#0]GOTO26(Z-DEPTH)
()
(CALCULATE-AND-VALIDATE-LEAD-RADIUS)
#23=[[[[#7/2]-#[2000+#11]]/2]+#[2000+#11]]
IF[#23LT#[2000+#11]]GOTO23
()
(SAVE-SYSTEM-VARS)
#1=#5003(PRESENT-Z-POSITION)
#2=#4003(POSITIONING-MODE)
()
(RAPID-TO-DEPTH)
G0G90Z#26
()
(RAMP-IN)
G1G17G41G91X[[#7/2]-#23]Y-#23H#11F#9
G3X#23Y#23R#23
()
(HELICAL-MOVE)
#3=0
WHILE[#3LT#18]DO1
I-[#7/2]Z#20
#3=#3+1
END1
()
(RAMP-OUT)
X-#23Y#23R#23
G1G40X-[[#7/2]-#23]Y-#23
()
(RAPID-TO-SAVED-Z-POSITION)
G0G90Z#1
()
(RESTORE-POSITIONING-MODE)
IF[#2EQ90]GOTO99
G91
GOTO99
()
(ALARM-MESSAGES)
GOTO99
N7#3000=7(INVALID MAJOR DIA, D VALUE)
GOTO99
N9#3000=9(INVALID FEED RATE, F VALUE)
GOTO99
N11#3000=11(INVALID REGISTER, H VALUE)
GOTO99
N18#3000=18(INVALID REVOLUTIONS, R VALUE)
GOTO99
N20#3000=20(INVALID PITCH, T VALUE)
GOTO99
N23#3000=23(TOOL DIA TO LARGE)
GOTO99
N26#3000=26(INVALID DEPTH, Z VALUE)
()
(PROGRAM-END)
N99M99

Our thanks to the author for permission to make this macro available to you!

Kelly D. Grills
KDG-Engineering
CAD / CAM / CIM / CNC Consulting

TO TOP

Technical and Customer Support Ask for Rich Kerr 1-800-235-TOOL   (1-800-235-8665) or directly via e-mail, fax: 1-319-263-5346, mail:    Schmarje Tool Company P.O. Box 16 MUSCATINE, IA 52761