Water Industry Process Automation & Control Monthly - April 2024
MILL SPINDLE PROGRAMS
1. %
O00000
(** MILL CLASS WB 4/20/04 **)
(=================================)
O00001
(vv MILL WORKBOOK EXERCISES vv)
(=================================)
O01000
(vvvv WARMUP PROGRAMS 1000 vvv)
(=================================)
O01001
(5,000 Spindle Warmup program)
(This program should be run prior)
(to machine use if machine has)
(been idle for more than 4 days.)
(Cycle time is 20-minutes.)
(This program can be used daily)
(for spindle warm-up prior to high)
(speed spindle use.)
(Set override at 100 percent for)
(5,000 rpm machines.)
(9-22-99)
(---------------------------------)
S250 M03
G04 P200.
S500 M03
G04 P200.
S1250 M03
G04 P200.
S2500 M03
G04 P200.
S3750 M03
G04 P200.
S5000 M03
G04 P200.
M30
(=================================)
O01002
(7,500 Spindle Warmup program)
(This program should be run prior)
(to machine use if machine has)
(been idle for more than 4 days.)
(Cycle time is 20-minutes.)
(This program can be used daily)
(for spindle warm-up prior to high)
(speed spindle use.)
(Set override at 100 percent for)
(7,500 rpm machines.)
(9-22-99)
(---------------------------------)
2. S500 M03
G04 P200.
S1000 M03
G04 P200.
S2500 M03
G04 P200.
S5000 M03
G04 P200.
S7500 M03
G04 P200.
S10000 M03
G04 P200.
M30
(=================================)
O01003
(10,000 Spindle Warmup program)
(This program should be run prior)
(to machine use if machine has)
(been idle for more than 4 days.)
(Cycle time is 20-minutes.)
(This program can be used daily)
(for spindle warm-up prior to high)
(speed spindle use.)
(Set override at 100 percent for)
(10,000 rpm machines.)
(9-22-99)
(---------------------------------)
(10,000 Spindle Warmup program)
S500 M03
G04 P200.
S1000 M03
G04 P200.
S2500 M03
G04 P200.
S5000 M03
G04 P200.
S7500 M03
G04 P200.
S10000 M03
G04 P200.
M30
(=================================)
O01004
(15,000 Spindle Warmup program)
(This program should be run prior)
(to machine use if machine has)
(been idle for more than 4 days.)
(Cycle time is 20-minutes.)
(This program can be used daily)
(for spindle warm-up prior to high)
(speed spindle use.)
(Set override at 100 percent for)
3. (15,000 rpm machines.)
(9-22-99)
(---------------------------------)
(150 percent for)
(15,000 rpm machines.)
(9-22-99)
S750 M03
G04 P200.
S1500 M03
G04 P200.
S3750 M03
G04 P200.
S7500 M03
G04 P200.
S11250 M03
G04 P200.
S15000 M03
G04 P200.
M30
(=================================)
O01005
(30,000 Spindle Warmup program)
(This program should be run prior)
(to any 30,000 spindles operating)
(above 10,000 rpm. This will help)
(revent possible overheating of)
(the spindle due to settling of)
(lubrication. This 20 minute)
(warmup program will bring the)
(spindle up to speed slowly and)
(allow the spindle to thermally)
(stabalize. This program should)
(be used daily for spindle warmup)
(prior to high speed use.)
(ES0352 REV.E10/03)
(---------------------------------)
(30K Spindle Warmup program)
(20 Minutes)
S1500 M03
G04 P200.
S3000 M03
G04 P200.
S7500 M03
G04 P200.
S15000 M03
G04 P200.
S22500 M03
G04 P200.
S30000 M03
G04 P200.
M30
(=================================)
4. O02000
(vv MISC. INFORMATION 2000 vvv)
(=================================)
O02001
(Program Names listed here, in)
(the first two lines of a program)
(will show up next to the program)
(number in the LIST PROG. display)
(when entering text names between)
(parenthesis.)
(---------------------------------)
(Pressing SHIFT and then a letter)
(will output lower case text for)
(the letters beween parenthesis.)
(---------------------------------)
N1 (Operation information)
T1 M06 (Tool information...)
G90 G54 G00 X0.5 Y-0.5
(=================================)
O03000
(vvvv MISC. PROGRAMS 3000 vvvv)
(=================================)
O03001
(MDI Commands)
(Text 10/18/02)
(vvvvvvvvv TEXT vvvvvvvvv)
(---------------------------------)
(=================================)
N1 (Spindle On S500)
S500 M03
G04 P100.
M30
N2 (Spindle On S2000)
S2000 M03
M30
N3
M80 (DOOR OPEN)
M30
N4
M81 (DOOR CLOSE)
G04 P1.
M00
N9
T9 (CHIP FAN)
28. X-0.35
G80 G00 Z1. M09
G28 G91 Y0. M05
M00
T1 M06 (1/2 DIA. E.M.)
G90 G54 G00 X-0.35 Y-0.25
S1400 M03
G43 H01 Z0.1 M08
Z-0.25
G01 X-0.25 F12.
Y1.5
G02 X1.884 Y0.616 R-1.25
G01 X1.018 Y-0.25
X-0.35
G80 G00 Z1. M09
G28 G91 Y0. M05
M30
(=================================)
O90047
(P.47=G12/G13 One Pass I Only)
(FIRST G12/G13 EXAMPLE)
(*The first example will do the)
(G13 circular pocket with the same)
(feedrate in X,Y and Z axes.)
( The second example is the same)
(as the first example, except a Z)
(axis feed move down has been)
(added with a different feedrate)
(then what the X and Y axes are)
(doing in the G13 circular pocket.)
(SECOND G13 EXAMPLE below)
(Adds a Z move with a different)
(feed move down)
(---------------------------------)
(FIRST G12/G13 EXAMPLE)
(G12 ONE PASS USING I ONLY)
N11 (D01 DIA. OFFSET IS .500)
N12 T1 M06 (1/2 DIA. 2 FLT E.M.)
N13 G90 G54 G00 X2.5 Y2.5
N14 S1910 M03
N15 G43 H01 Z0.1 M08
N16 G13 Z-0.5 I0.5 D01 F12. (*)
N17 G00 Z1. M09
N18 G53 G49 Z0. M05
N19 M30
(---------------------------------)
(SECOND G12/G13 EXAMPLE)
(**This second example is the same)
(as the first example, except a Z)
(axis feed move down has been)
(added with a different feedrate)
(then what the X and Y axes are)
29. (doing in the G13 circular pocket)
(command.)
(---------------------------------)
(G12/G13 ONE PASS USING I ONLY)
N21 (D01 DIA. OFFSET IS .500)
N22 T1 M06 (1/2 DIA. 2FLT END MILL)
N23 G90 G54 G00 X2.5 Y2.5
N24 S1910 M03
N25 G43 H01 Z0.1 M08
N26 G01 Z-0.5 F30. (**)
N27 G13 Z-0.5 I0.5 D01 F12. (**)
N28 G00 Z1. M09
N29 G53 G49 Z0. M05
N30 M30
(=================================)
O90048
(P.48=G13 Multiple Pass I,K,Q)
(FIRST G13 EXAMPLE)
(*The first example will do the)
(G13 circular pocket with the same)
(feedrate in X,Y and Z axes.)
(The second example is the same)
(as the first example, except a Z)
(axis feed move down has been)
(added with a different feedrate)
(then what the X and Y axes are)
(doing in the G13 circular pocket.)
(SECOND G13 EXAMPLE below)
(Adds a Z move with a different)
(feed move down)
(---------------------------------)
(FIRST G13 EXAMPLE)
(G13 MULTIPLE PASS I,K & Q to do a)
(3.0 Dia.x.5 Deep circular pocket.)
N31 (D02 DIA. OFFSET IS .625)
N32 T2 M06 (5/8 DIA. 2 FLT E.M.)
N33 G90 G54 G00 X2.5 Y2.5
N34 S1500 M03
N35 G43 H02 Z0.1 M08
N36 G13 Z-0.5 I0.3 K1.5 Q0.3 D02 F9. (*)
N37 G00 Z1. M09
N38 G53 G49 Z0. M05
N39 M30
(---------------------------------)
(SECOND G13 EXAMPLE)
(**This second example is the same)
(as the first example, except a Z)
(axis feed move down has been)
(added with a different feedrate)
(then what the X and Y axes are)
(doing in the G13 circular pocket)
(command.)
30. (---------------------------------)
(G13 MULTIPLE PASS I,K & Q to do a)
(3.0 Dia.x.5 Deep circular pocket.)
N41 (D02 DIA. OFFSET IS .625)
N42 T2 M06 (5/8 DIA. 2 FLT E.M.)
N43 G90 G54 G00 X2.5 Y2.5
N44 S1500 M03
N45 G43 H02 Z0.1 M08
N46 G01 Z-0.5 F6. (*)
N47 G13 Z-0.5 I0.3 K1.5 Q0.3 D02 F9. (**)
N48 G00 Z1. M09
N49 G53 G49 Z0. M05
N50 M30
(=================================)
O90049
(P.49=G13 Multi Z Passes+G91)
(TO DEPTH USING G91 AND AN L LOOP)
(COUNT)
(Since the G91 incremental is)
(looped together within the G13)
(circular pocket command, you are)
(NOT able to separate the Z axis)
(feed from the X and Y axis feed,)
(unless you have a separate G12 or)
(G13 for each step down, with a Z)
(move at a different feedrate.)
( You may want to fast feed down)
(to the surface of where the)
(pocket starts on the part, to)
(begin incrementally stepping down)
(to the desired depth.)
(---------------------------------)
(G13 MULTIPLE Z PASSES)
N1 (D02 DIA. OFFSET IS .625)
N2 T2 M06 (5/8 DIA. 2 FLT END MILL)
N3 G90 G54 G00 X2.5 Y2.5
N4 S1500 M03
N5 G43 H02 Z0.1 M08
N6 G01 Z0. F30.
N7 G13 G91 Z-0.375 I0.325 K2. Q0.3 D02 L4 F12.
N8 G00 G90 Z1. M09
N9 G53 G49 Z0. M05
N10 M30
(=================================)
O90054
(P.54=G17 XY Circular Plane)
N1 T1 M06 (1/2 DIA. 2 FLT E.M.)
N2 G90 G54 G00 X4. Y3.25 S2600 M03
N3 G43 H01 Z0.1 M08
N4 G01 Z-0.5 F50.
N5 G17 G02 X5.25 Y2. R1.25 F10.
N6 G00 Z0.1
34. N7 G02 X-1.75 Y2. R0.25
N8 G01 X1.5
N9 G02 X2. Y1.5 R0.5
N10 G01 Y-1.
N11 X-0.75 Y-2.
N12 X-1.75
N13 G02 X-2. Y-1.75 R0.25
N14 G40 G01 X-2.35 Y-2.
N15 G41 G01 X-2. D01 F8.
N16 Y1.75
N17 G02 X-1.75 Y2. R0.25
N18 G01 X1.5
N19 G02 X2. Y1.5 R0.5
N20 G01 Y-1.
N21 X-0.75 Y-2.
N22 X-1.75
N23 G02 X-2. Y-1.75 R0.25
N24 G40 G01 X-2.35 Y-2.
N25 G00 Z1. M09
N26 G53 G49 Y0 Z0 M05
N27 M30
(=================================)
O90068
(P.68=Loop Single Helical Move)
(FIRST HELICAL EXAMPLE)
(Repeating a single helical move)
(10 times to do a 2.0-12UN thread.)
(Tool is positioned down inside)
(thread in the Z axis on line N5,)
(and then moved up with a positive)
(Z move in N7 for the helical move)
(to climb cut thread tool.)
(---------------------------------)
N1 T4 M06 (SINGLE POINT THRD. TOOL)
N2 G90 G54 G00 X1.6 Y-1.25
N3 S1500 M03
N4 G43 H04 Z0.1 M08
N5 G01 Z-0.8 F50.
N6 G41 X2.25 D04 F10.
N7 G91 G03 X0. Y0. I-1. J0. Z0.0833 F3. L10
N8 G90 G40 G01 X1.6 Y-1.25
N9 G00 Z0.1 M09
N10 G53 G49 Z0.
N11 M30
(---------------------------------)
(SECOND HELICAL EXAMPLE)
(*This second example is the same)
(as the first example, without)
(some of the letter commands in)
(line N7. These ending command)
(values where defined with a G91)
(incremental move that has the)
35. (ending point the same as the)
(start point. And if it starts and)
(ends at the same location in)
(either axis, you dont need to)
(list them again. And if either)
(I and J are zero, they dont need)
(to be entered in the program.)
(---------------------------------)
N1 T4 M06 (SINGLE POINT THRD. TOOL)
N2 G90 G54 G00 X1.6 Y-1.25
N3 S1500 M03
N4 G43 H04 Z0.1 M08
N5 G01 Z-0.8 F50.
N6 G41 X2.25 D04 F10.
N7 G91 G03 I-1. Z0.0833 F3. L10
N8 G90 G40 G01 X1.6 Y-1.25
N9 G00 Z0.1 M09
N10 G53 G49 Z0.
N11 M30
(=================================)
O90069
(P.69=Thread Hob Helical Move)
(FIRST HELICAL EXAMPLE)
(Doing a single helical move once,)
(with a thread hob, to do a)
(2.0-12UN thread.)
(Tool is positioned down inside)
(thread in the Z axis on line N5,)
(and then moved up with a positive)
(Z move in N7 for the helical move)
(to climb cut thread tool.)
(Below is a SECOND HELICAL EXAMPLE)
(---------------------------------)
N1 T3 M06 (3/4 DIA. THREAD MILL)
N2 G90 G54 G00 X1.25 Y-1.25
N3 S1500 M03
N4 G43 H03 Z0.1 M08
N5 G01 Z-1. F50.
N6 G41 X1.75 Y-1.75 D03
N7 G03 X2.25 Y-1.25 R0.5 F10.
N8 G03 X2.25 Y-1.25 I-1. J0. Z-0.9167 F12.
N9 G03 X1.75 Y-0.75 R0.5
N10 G40 G01 X1.25 Y-1.25
N11 G00 Z0.1 M09
N12 G53 G49 Z0.
N13 M30
(---------------------------------)
(SECOND HELICAL EXAMPLE)
(*This second example is the same)
(as the first example, without)
(some of the letter commands in)
(line N8. These commands where)
36. (the same as the commands in N7.)
(And if these command values are)
(the same, you dont need to list)
(them again. And if I and J are)
(zero, they dont need to be)
(entered in the program.)
(And G03 does not need to be in)
(lines N8 and N9 since the G03 in)
(line N7 is modal, though for)
(clarity its a good idea to list)
(all arcs with either G02 or G03.)
(---------------------------------)
N1 T3 M06 (3/4 DIA. THREAD MILL)
N2 G90 G54 G00 X1.25 Y-1.25
N3 S1500 M03
N4 G43 H03 Z0.1 M08
N5 G01 Z-1. F50.
N6 G41 X1.75 Y-1.75 D03
N7 G03 X2.25 Y-1.25 R0.5 F10.
N8 G03 I-1. Z-0.9167 F12.
N9 G03 X1.75 Y-0.75 R0.5
N10 G40 G01 X1.25 Y-1.25
N11 G00 Z0.1 M09
N12 G53 G49 Z0.
N13 M30
(=================================)
O90072
(P.72=G98/G99 Return Plane)
N1 T2 M06 (7/16 DIA. CARBIDE DRILL)
N2 G90 G54 G00 X1.5 Y-0.5
N3 S1200 M03
N4 G43 H02 Z1. M08
N5 G83 G99 Z-1.2 Q0.2 R0.1 F8.
N6 X0.5 Y-0.75
N7 Y-2.25
N8 G98 X1.5 Y-2.5
N9 G99 X3.5 R-0.4
N10 X4.5 Y-2.25
N11 Y-0.75
N12 X3.5 Y-0.5
N13 G80 G00 Z1. M09
N14 G53 G49 Z0. M05
N15 M30
(=================================)
O90073
(P.73=G81 Drilling Cycle)
N1 T1 M06 (1/2 DIA. DRILL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H01 Z1. M08
N5 G81 G99 Z-0.625 R0.1 F10.
N6 X1.5 Y1.5
37. N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90074
(P.74=G82 Drill*Dwell Cycle)
(The P command in a G82 is used to)
(dwell at the end of drill cycle)
(---------------------------------)
N1 T1 M06 (1/2 DIA. C,BORE TOOL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H01 Z1. M08
N5 G82 G99 Z-0.625 P1.5 R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90076
(P.76=G83 Deep Drill with Q)
(The P command can be used to)
(dwell at the end of the Z depth)
(on a G83 drill cycle.)
(---------------------------------)
N1 T3 M06 (1/2 DIA. x 2.5 L. DRILL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H03 Z1. M08
N5 G83 G99 Z-2.125 Q0.5 R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90077
(P.77=G83 Deep Drill with IJK)
(The P command can be used to)
(dwell at the end of the Z depth)
(on a G83 drill cycle.)
(---------------------------------)
N1 T3 M06 (1/2 DIA. x 2.5 L. DRILL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H03 Z1. M08
N5 G83 G99 Z-2.125 I0.5 J0.1 K0.2 R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
38. O90080
(P.80=G84 R.H. Tapping Cycle)
(You dont need to start the)
(sindle with an M03 for a tap)
(thats using a G84 because this)
(G84 cycle will turn the spindle)
(on for you.)
(---------------------------------)
N1 T4 M06 (7/16-14 TAP)
N2 G90 G54 G00 X0.75 Y0.75
N3 S450 (The G84 Turns on spindle)
N4 G43 H04 Z1. M08
N5 G84 G99 Z-0.65 R0.1 J3 F32.1429
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90081
(P.81=G85 Bore In-Bore Out)
(G85 Bores in to Z depth, then)
(bores out)
(---------------------------------)
(P.83 BORE IN BORE OUT CYCLE G85)
N1 T5 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H05 Z1. M08
N5 G85 G99 Z-0.55 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90082
(P.82=G86 Bore-Stop-Rapid Out)
(G86 Bores in to Z depth, spindle)
(stops, and then rapids out.)
(---------------------------------)
N1 T6 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H06 Z1. M08
N5 G86 G99 Z-0.55 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90083
39. (P.83=G87 Bore-Manual Retract)
(G87 Bores in to Z depth, spindle)
(stops, handwheel out.)
(---------------------------------)
N1 T7 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H07 Z1. M08
N5 G87 G99 Z-0.55 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90084
(P.84=G88 Bore-Dwell-Manual)
(G87 Bores in to Z depth, dwell,)
(spindle stops, handwheel out.)
(---------------------------------)
N1 T8 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H08 Z1. M08
N5 G88 G99 Z-0.55 P0.5 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90085
(P.85=G89 Bore-Dwell-Bore Out)
(G89 Bores in to Z depth, dwell,)
(bores out.)
(---------------------------------)
N1 T9 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H09 Z1. M08
N5 G89 G99 Z-0.55 P0.5 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90089
(P.89=G73 HS Peck Drill with Q)
(The P command can be used to)
(dwell at the end of the Z depth)
(on a G73 drill cycle.)
(---------------------------------)
N1 T3 M06 (1/2 DIA. x 2.5 L. DRILL)
40. N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H03 Z1. M08
N5 G73 G99 Z-2.125 Q0.1 R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90090
(P.90=G73 HS Peck Drill IJK)
(The P command can be used to)
(dwell at the end of the Z depth)
(on a G73 drill cycle.)
(---------------------------------)
N1 T3 M06 (1/2 DIA. x 2.5 L. DRILL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H03 Z1. M08
N5 G73 G99 Z-2.125 I0.5 J0.1 K0.2 R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90091
(P.91=G73 HS Peck Drill KQ)
(The P command can be used to)
(dwell at the end of the Z depth)
(on a G73 drill cycle.)
(---------------------------------)
N1 T3 M06 (1/2 DIA. x 2.5 L. DRILL)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H03 Z1. M08
N5 G73 G99 Z-2.125 Q0.2 K1. R0.1 F10.
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90092
(P.92=G74 L.H. Tapping Cycle)
(You dont need to start the)
(sindle with an M03 for a tap)
(thats using a G74 because this)
(G74 cycle will turn the spindle)
(on for you.)
(---------------------------------)
N1 T4 M06 (1/2-20 L.H. TAP)
N2 G90 G54 G00 X0.75 Y0.75
41. N3 S450 (The G74 Turns on spindle)
N4 G43 H04 Z1. M08
N5 G74 G99 Z-0.65 R0.1 J5 F22.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(=================================)
O90093
(P.93=G76 Bore-Stop-Shift-Rapid)
(FIRST G76 Example = N1)
(SECOND G76 Example = N21)
(G76 Bores in to Z depth, spindle)
(stops, shifts off the amount of)
(Q in the X or Y direction either)
(+ or - as selected in setting 27,)
(and then rapids out.)
(BE SURE tool tip is positioned)
(accordingly with the position of)
(the spindle when it orientates.)
(Below is a SECOND G76 EXAMPLE)
(---------------------------------)
(FIRST G76 Example = N1)
N1 T6 M06 (BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H06 Z1. M08
N5 G76 G99 Z-0.55 Q0.01 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(---------------------------------)
(SECOND G76 Example = N21)
(*This second G76 example is the)
(same as the first example, except)
(the shift amount can be defined)
(with the I and J commands. I is)
(to shift the X axis, and J shifts)
(the Y axis in the +/- direction.)
(---------------------------------)
N21 T6 M06 (BORING BAR)
N22 G90 G54 G00 X0.75 Y0.75
N23 S1451 M03
N24 G43 H06 Z1. M08
N25 G76 G99 Z-0.55 P0.5 I-0.01 R0.1 F4.5
N26 X1.5 Y1.5
N27 G80 G00 Z1. M09
N28 G53 G49 Z0. M05
N29 M30
(=================================)
42. O90094
(P.94=G77 BackBore)
(FIRST G76 Example = N1)
(SECOND G76 Example = N21)
(G77 Above a part, stops spindle,)
(orientates, shifts off center,)
(rapids in to the R plane, shifts)
(back to center, turns on spindle,)
(feeds up to Z depth to produce)
(back counterbore, stops spindle,)
(shifts off, and rapids out.)
( G77 shifts off the amount of)
(Q in the X or Y direction either)
(+ or - as selected in setting 27.)
(BE SURE tool tip is positioned)
(accordingly with the positioning)
(of spindle when it orientates.)
(---------------------------------)
(FIRST G77 Example = N1)
N1 T7 M06 (BACK BORING BAR)
N2 G90 G54 G00 X0.75 Y0.75
N3 S1451 M03
N4 G43 H07 Z1. M08
N5 G77 G99 Z-0.55 Q0.06 R0.1 F4.5
N6 X1.5 Y1.5
N7 G80 G00 Z1. M09
N8 G53 G49 Z0. M05
N9 M30
(---------------------------------)
(SECOND G77 Example = N21)
(This second G77 example is the)
(same as the first example, except)
(the shift amount can be defined)
(with the I and J commands. I is )
(to shift the X axis, and J shifts)
(the Y axis in the +/- direction.)
(---------------------------------)
N21 T7 M06 (BORING BAR)
N22 G90 G54 G00 X0.75 Y0.75
N23 S1451 M03
N24 G43 H07 Z1. M08
N25 G77 G99 Z-0.55 I-0.06 R0.1 F4.5
N26 X1.5 Y1.5
N27 G80 G00 Z1. M09
N28 G53 G49 Z0. M05
N29 M30
(=================================)
O90096
(P.96=G70 Bolt Hole Circle)
(I=The BHC radius)
(J=Starting angle from 3*oClock)
(L=Number of holes)