Use LONGHOLE to machine long holes located on a circle. The longitudinal axis of the long holes is aligned radially.
In contrast to the slot, the width of the long hole is determined by the tool diameter. Internally in the cycle, an optimum traversing path of the tool is determined, ruling out unnecessary idle passes. If several depth infeeds are required to machine an slot, the infeed is carried out alternately at the end points. The path to be traversed along the longitudinal axis of the long hole will change its direction after each infeed. The cycle will search for the shortest path when changing to the next long hole.
NOTICE: The cycle requires a milling cutter with an “end tooth cutting across center” (DIN844).
Note: A tool compensation must be programmed before the cycle is called. Otherwise, the cycle is aborted and alarm 61000 “No tool compensation active” is output.
If mutual contour violations of the slots result from incorrect values of the parameters that determine the arrangement and the size of the slots, the cycle will not start the machining. The cycle is aborted and the error message 61104 “Contour violation of slots/long holes” is output.
During the cycle, the workpiece coordinate system is offset and rotated. The values in the workpiece coordinate system are shown on the actual value display such that the longitudinal axis of the long hole being machined is positioned on the first axis of the current machining plane.
After the cycle has been completed, the workpiece coordinate system is in the same position again as it was before the cycle was called.
|You may be interested also:|
|“Siemens CNC Milling | CYCLE90 | Thread Milling”|
Supported CNC Series
|Siemens CNC 802D, 810D, 840D, 840D sl, 840Di, 840Di sl series controllers.|
|LONGHOLE (RTP, RFP, SDIS, DP, DPR, NUM, LENG, CPA, CPO, RAD, STA1, INDA, FFD, FFP1, MID)|
|RTP = Retraction plane (absolute)|
|RFP = Reference plane (absolute)|
|SDIS = Safety clearance (enter without sign)|
|DP = Long hole depth (absolute)|
|DPR = Long hole depth relative to the reference plane (enter without sign)|
|NUM = Number of long holes|
|LENG = Length of long hole (enter without sign)|
|CPA = Center point of circle, abscissa (absolute)|
|CPO = Center point of circle, ordinate (absolute)|
|RAD = Radius of the circle (enter without sign)|
|STA1 = Starting angle|
|INDA = Incrementing angle|
|FFD = Feedrate for depth infeed|
|FFP1 = Feedrate for surface machining|
|MID = Maximum infeed depth for an infeed (enter without sign)|
LONGHOLE CNC Program Example – 1
With this program, you can machine 4 long holes with a length of 30 mm and a relative depth of 23 mm (difference between the reference plane and the long hole base), which are positioned on a circle with the center point Z45 Y40 and a radius of 20 mm in the Y plane (G19). The starting angle is 45 degrees, the incremental angle is 90 degrees. The maximum infeed depth is 6 mm, the safety clearance 1 mm.
N10 G19 G90 S600 M3 ; Specification of technology values
T10 D1 ;
N20 G0 Y50 Z25 X5 ; Approach starting position
N30 LONGHOLE (5, 0, 1, , 23, 4, 30, 40, 45, 20, 45, 90, 100 ,320, 6) ; Cycle call
N40 M30 ; Program end