The document contains the main program and subprograms for a CNC milling machine. It describes: 1. The main program calls several subprograms to perform operations like contouring, pocketing, circular pocketing, slot milling, and tapping holes. 2. The subprograms contain G-code instructions for specific milling operations like contouring an area, milling a pocket, or drilling holes in a pattern. 3. The main program executes the subprograms in sequence to machine features of a workpiece, using different tools for operations like end milling, drilling, and tapping. It provides information on tools, feedrates, and coordinates for each operation.

1. 1 – 6
Solution of Page 49
Fanuc 21 Controller

2. 2 – 6
Main Program
O0001 ( EXERCISE P49 )
( MAIN PROGRAM )
( O2..CONTOUR SUBPROG. )
( O3..POCKET SUBPROG. )
( O4..CIRCULAR POCKET SUBPROG. )
( O5..SLOT SUBPROG. )
( O6..TAPPED HOKLES SUBPROG. )
( CONTROLLER FANUC )
( MACHINE PC MILL 105 )
( PROGRAMMED BY ENG. AMIR TAWFIC )
( DATE:20-10-2016 )
( W.P 120 X 120 X 30 )
( T1..SHELL END MILL @40 MM )
( T2..SLOT END MILL @10 MM )
( T3..DOVETAIL CR 8, CL 4 MM )
( T4..NC SPOT DRILL @10 MM )
( T5..TWIST DRILL @5 MM )
( T6..TAP M6X1 )
N5 G90 G17 G21 G40 G49 G50 G80
N10 G54
N15 T1 M6 ( SHELL ENDMILL @40)
N20 G97 S1000 G94 F100 M3 M8
N25 G0 X18 Y-22
N30 G43 H1 Z0
N35 G1 Y142
N40 G91 G0 X38
N45 G90 G1 Y-22
N50 G91 G0 X38
N55 G90 G1 Y142
N60 G0 Z3
N65 X-50 Y-50
N70 Z0
N75 G41 H11
N80 M98 P50002
N85 G0 X-50
N90 G40 Y-50
N95 Z30
N100 T2 M6 ( SLOT ENDMILL @10)
N105 S1500 F150 M3 M8
N110 X20 Y85
Subprogram
O0002 ( SP O1 )
N5 G91 Z-2
N10 G90 G1 X10
N15 Y110
N20 X110
N25 Y10
N30 X-40
N35 Y-40
N40 M99
1
2

3. 3 – 6
Main Program
N115 G43 H2 Z3
N125 M98 P30003
N130 G90 G0 Z3
N135 X85 Y92.5
N140 G1 Z0
N145 M98 P30004
N150 G90 G0 Z2
N155 G68 X100 Y20 R160
N160 G0 X100 Y20
N165 M98 P20005
N170 G90 G0 Z30
N175 T3 M6 ( DOVETAIL )
N176 M3 M8
N180 X100 Y20
N185 G43 H3 G0 Z0
N190 G1 Z-2
N195 G91 X40
N200 G90 G69 G0 Z3
N205 G0 X85 Y92.5
N210 Z-1
N215 G91 G1 X-8.5
N220 G2 X0 Y0 I8.5 J0
N225 G90 G0 Z1
N230 X-50 Y-50
N235 G41 H13 ( H13 = 4 MM )
N240 M98 P2
N245 G0 X-50
N250 G40 Y-50
N255 Z3
N260 X20 Y85
N165 Z0
N270 M98 P3
N275 G90 G0 Z30
N280 T4 M6 ( NC SPOTDRILL @10 )
N285 S200 F200 M3 M8
N290 X10 Y50
N295 G43 H4 Z3
N300 G81 G91 X10 Z-4.125 K4
N305 G80 X10 Y10
N310 G81 X-10 Z-4.125 K4
Subprogram
O0003 ( SP O1 )
N5 G1 G91 Z-2
N10 Y15
N15 X20
N20 Y-15
N25 X-20
N30 Y8
N35 X11
N45 X-11 Y-8
N50 M99
Subprogram
O0004 ( SP O1 )
N5 G91 G1 Z-2
N10 X-7.5
N15 G2 X0 Y0 I7.5 H0
N20 G1 X7.5
N25 M99
Subprogram
O0005 ( SP O1 )
N10 G91 G1 Z-2
N15 X40
N20 Z-2
N25 X-40
N30 M99Recall Pocket
subprogram. and Execute
it one time
For chamfer
Recall Contour
Subprogram and
Execute it one time
for chamfer
3

4. 4 – 6
Main Program
N315 G80 X-10 Y10
N320 G81 X10 Z-4.125 K4
N325 G90 X20 Y30 Z-1.625
N330 M98 P6
N335 G0 Z30
N340 T5 M6 ( TWIST DRILL @5)
N345 M3 M8
N350 X10 Y50
N355 G43 H5 Z3
N360 G73 G91 Z-13 Q3 X10 K4
N365 G80 X10 Y10
N370 G73 Q3 X-10 K4
N375 G80 X-10 Y10
N380 G73 Q3 X10 K4
N385 G80 G90
N390 X20 Y30
N395 G83 Q3 Z-20 G98 R1
N400 M98 P6
N405 G0 Z30
N410 T6 M6 ( TAP M6 )
N415 S100 G95 F1 M3 M8
N420 X20 Y30
N425 G43 H6 Z3
N430 G84 Z-15 R1
N435 M98 P6
N440 G28 G91 Z0 M5 M9
N445 G28 X0 Y0
N450 M30
Subprogram
O0006 ( SP O1 )
N5 X30 Y20
N10 X40 Y30
N15 G52 X85 Y60 G16
N20 X15 Y0
N25 Y60
N30 Y120
N35 Y180
N40 Y-120
N45 Y-60
N50 G80 G15 G52 X0 Y0
N55 M99

5. 5 – 6
 By Replace the three doted boxes with the following boxes
 Software Setting
Other Solution
N65 X-22 Y-22
N70 Z0
N75 M98 P50008
1
O0002 ( SP O1 )
N5 G91 Z-2
N6 G90 G41 H11 G1 X10 Y10
N15 Y110
N20 X110
N25 Y10
N30 X-22
N35 G40 G0 Y-22 G50
N40 M99
2
N230 G51 X60 Y60 I680 J680
N235 X-22 Y-22
N240 M98 P8
3

6. 6 – 6
To Download files, go to Link Below
https://drive.google.com/drive/folders/0BwjrFT2DRuSXaWZOT2tPSmU3cFk?usp=sharing