0  BEGIN PGM 5025_EN MM 
1  ;Program for using a form cutter 
2  ;to deburr a hole on the cylinder surface 
3  ;that was drilled perpendicular 
4  ;to the cylinder axis.
5  ;It is machined in the three linear axes 
6  ;without tilting the working plane.
7  ;First you have to define 
8  ;all required parameters.
9  ;Then you make a program section 
10 ;consisting of tool call, positioning 
11 ;and a machining cycle around the hole.
12 ;In this program section you define 
13 ;all parameters because the parameters 
14 ;already programmed are effective 
15 ;only for deburring.
16 ;After the hole operation, you define 
17 ;the tool to be used for deburring.
18 ;Then the control calculates the coordinates 
19 ;for the single axis and moves the tool to it.
20 ;The control then calculates 
21 ;the next respective point 
22 ;with its X, Y and Z coordinates 
23 ;and moves the tool to it.
24 ;This is repeated until
25 ;it returns to the starting point.
26 ;In the parameter PITCH you define the number 
27 ;of point in which the machining is divided.
28 ;Important! The control calculates
29 ;the path contour for the tool center.
30 ;With the parameter 
31 ;OFFSET OF TOOL CENTER TO RADIUS (Q7), 
32 ;you define how far the tool center 
33 ;is led away from the hole’s edge.
34 ;Watch for the algebraic sign: 
35 ;a positive value 
36 ;makes the tool-center path greater 
37 ;than the radius, negative value 
38 ;makes it smaller.
39 ;
40 ;Parameter entry
41 FN 0: Q3 =+100 ;RADIUS OF CYLINDER
42 FN 0: Q4 =+100 ;PITCH
43 FN 0: Q5 =+3 ;ENTER A POSITIVE DEPTH
44 FN 0: Q1 =+0 ;CENTER OF HOLE IN X
45 FN 0: Q6 =+60 ;RADIUS OF HOLE
46 FN 0: Q7 =-0.5 ;OFFSET OF TOOL CENTER TO RADIUS
47 FN 0: Q10 =+20 ;SAFETY CLEARANCE
48 FN 0: Q11 =+1000 ;FEED RATE FOR PECKING
49 FN 0: Q12 =+2000 ;FEED RATE FOR MILLING
50 ;End of parameter input
51 ;
52 BLK FORM CYLINDER X RQ3 L200 DIST+100
53 ;
54 ;Shift the datum to the hole center 
55 ;and cylinder surface
56 CYCL DEF 7.0 DATUM SHIFT
57 CYCL DEF 7.1  X+Q1
58 CYCL DEF 7.2  Z+Q3
59 ;
60 ;Tool call for the hole
61 TOOL CALL 8 Z S3000 F800
62 ;
63 L  Z+100 R0 FMAX M3 ;Move to clearance height
64 L  X+0  Y+0 R0 FMAX ;Move to the hole center
65 L  Z+Q10 R0 FMAX ;Move to set-up clearance
66 FN 3: Q80 =+Q6 * +2 ;Calculation of hole diameter
67 ;Cycle for drilling
68 CYCL DEF 252 CIRCULAR POCKET ~
    Q215=+0    ;MACHINING OPERATION ~
    Q223=+Q80  ;CIRCLE DIAMETER ~
    Q368=+0    ;ALLOWANCE FOR SIDE ~
    Q207= AUTO ;FEED RATE FOR MILLNG ~
    Q351=+1    ;CLIMB OR UP-CUT ~
    Q201=-100  ;DEPTH ~
    Q202=+10   ;PLUNGING DEPTH ~
    Q369=+0    ;ALLOWANCE FOR FLOOR ~
    Q206=+300  ;FEED RATE FOR PLNGNG ~
    Q338=+0    ;INFEED FOR FINISHING ~
    Q200=+2    ;SET-UP CLEARANCE ~
    Q203=+0    ;SURFACE COORDINATE ~
    Q204=+50   ;2ND SET-UP CLEARANCE ~
    Q370=+1    ;TOOL PATH OVERLAP ~
    Q366=+1    ;PLUNGE ~
    Q385=+500  ;FINISHING FEED RATE
69 M99
70 L  Z+100 R0 FMAX ;Retract
71 ;
72 ;Tool call for deburring
73 TOOL CALL 170 Z S12000
74 ;
75 L  Z+100 R0 FMAX M3 ;Move to clearance height
76 CALL LBL 1 ;Call the machining operation
77 ;
78 ;Retract and end program
79 L  Z+100 R0 FMAX M30
80 ;
81 ;Subprogram for machining
82 LBL 1
83 FN 0: Q23 =+Q5 ;First depth equals nominal depth
84 FN 0: Q24 =+0 ;Counter
85 FN 1: Q26 =+Q6 + +Q7 ;Accounting for cutter offset
86 FN 0: Q27 =+0 ;Starting angle
87 FN 4: Q37 =+360 DIV +Q4 ;Stepping angle
88 CALL LBL 10 ;Call of calculations
89 L  X+Q21  Y+Q22 FMAX ;Approach first position
90 L  Z+Q10 R0 FMAX ;Move to set-up clearance
91 L  Z-Q23 FQ11 ;Move to milling depth
92 LBL 2 ;Repetitions
93 FN 1: Q24 =+Q24 + +1 ;Update the counter
94 FN 1: Q27 =+Q27 + +Q37 ;Update the angle
95 CALL LBL 10 ;Call of calculations
96 L  X+Q21  Y+Q22  Z-Q23 FQ12 ;Move to new position
97 FN 12: IF +Q24 LT +Q4 GOTO LBL 2 ;Compare whether number of repetitions reached
98 LBL 0
99 LBL 10 ;Calculations
100 Q21 = Q26 * COS Q27 ;New X position
101 Q22 = Q26 * SIN Q27 ;New Y position
102 Q23 = Q3 - ( SQRT ( Q3 * Q3 - Q22 * Q22 ) ) + Q5 ;New Z position
103 LBL 0
104 END PGM 5025_EN MM