Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | GEAR HOBBING (Cycle 880, DIN/ISO: G880)

Cycle parameters

Q215 Machining operation (0/1/2/3)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing to finished dimension
3: Only finishing to oversize
Q540 Module?: Define the gear: Module of the
gear wheel. Input range 0 to 99.9999
Q541 Number of teeth?: Define the gear: Number
of teeth. Input range 0 to 99999
Q542 Outside diameter?: Define the gear:
Outside diameter of the finished part. Input range
0 to 99999.9999
Q543 Trough-to-tip clearance?: Define the gear:
Distance between the tip circle of the gear to be
cut and the root circle of the mating gear. Input
range 0 to 9.9999
Q544 Angle of inclination?: Define the gear:
Angle by which helical teeth are inclined relative to
the direction of the axis. (For straight-cut gears this
angle is 0°.) Input range -45 to +45
Q545 Tool lead angle?: Define the tool: Angle of
the tooth sides of the gear hob. Enter this value in
decimal notation. (Example: 0°47'=0.7833) Input
range : –60.0000 to +60.0000
Q546 Reverse tool rotation direction?: Define
the tool: Direction of spindle rotation of the gear
hob:
3: Tool turns to the right (M3)
4: Tool turns to the left (M4)
Q547 Angle offset of tool spindle?: Angle by
which the TNC rotates the workpiece at the
beginning of the cycle. Input range -180.0000 to
+180.0000
Q550 Machining side (0=pos./1=neg.)?: Define
the side on which the machining operation is to be
performed.
0: Positive machining side
1: Negative machining side
HEIDENHAIN | User's manual for cycle programming | 10/2017
NC blocks
63 CYCL DEF 880 GEAR HOBBING
Q215=0 ;MACHINING OPERATION
Q540=0 ;MODULE
Q541=0 ;NUMBER OF TEETH
Q542=0 ;OUTSIDE DIAMETER
Q543=0.167;TROUGH-TIP CLEARANCE
Q544=0 ;ANGLE OF INCLINATION
Q545=0 ;TOOL LEAD ANGLE
Q546=3 ;CHANGE TOOL DIRECTN.
Q547=0 ;ANG. OFFSET, SPINDLE
Q550=1 ;MACHINING SIDE
Q533=0 ;PREFERRED DIRECTION
Q530=2 ;INCLINED MACHINING
Q253=750 ;F PRE-POSITIONING
Q260=100 ;CLEARANCE HEIGHT
Q553=10 ;TOOL LENGTH OFFSET
Q551=0 ;STARTING POINT IN Z
Q552=-10 ;END POINT IN Z
Q463=1 ;MAX. CUTTING DEPTH
Q460=2 ;SAFETY CLEARANCE
Q488=0.3 ;PLUNGING FEED RATE
Q478=0.3 ;ROUGHING FEED RATE
Q483=0.4 ;OVERSIZE FOR DIAMETER
Q505=0.2 ;FINISHING FEED RATE
12
479