Fundamentals

Application

SL Cycles enable you to form complex contours by combining up to twelve subcontours (pockets or islands). You define the individual subcontours in subprograms. The control calculates the entire contour from the list of subcontours (subprogram numbers) you have specified in Cycle 14 CONTOUR.

 
Tip

Instead of SL cycles, HEIDENHAIN recommends using the more powerful software option Opt. Contour Milling (#167 / #1-02-1).

Related topics

Description of function

Characteristics of the subprograms

  • Closed contour without approach and departure movements
  • Coordinate transformations are permitted; if they are programmed within the subcontours, they are also effective in the following subprograms, but they need not be reset after the cycle call.
  • The control recognizes a pocket if the tool path lies inside the contour, for example if you machine the contour clockwise with radius compensation RR
  • The control recognizes an island if the tool path lies outside the contour, for example if you machine the contour clockwise with radius compensation RL
  • The subprograms must not contain spindle axis coordinates.
  • Always program both axes in the first NC block of the subprogram
  • If you use Q parameters, then only perform the calculations and assignments within the affected contour subprograms
  • Without machining cycles, feed rates, and M functions

Cycle properties

  • The control automatically positions the tool to the set-up clearance before each cycle. You must move the tool to a safe position before the cycle call
  • Each level of infeed depth is milled without interruptions since the cutter traverses around islands instead of over them
  • The radius of inside corners can be programmed—the tool will not stop, dwell marks are avoided (this applies to the outermost path of roughing or side finishing operations)
  • The contour is approached on a tangential arc for side finishing
  • For floor finishing, the tool again approaches the workpiece on a tangential arc (for spindle axis Z, for example, the arc is in the Z/X plane)
  • The contour is machined throughout in either climb or up-cut milling

The machining data, such as milling depth, allowances, and set-up clearance can be entered centrally in Cycle 20 CONTOUR DATA.

Program structure: Machining with SL Cycles

0 BEGIN SL 2 MM

...

12 CYCL DEF 14 CONTOUR

...

13 CYCL DEF 20 CONTOUR DATA

...

16 CYCL DEF 21 PILOT DRILLING

...

17 CYCL CALL

...

22 CYCL DEF 23 FLOOR FINISHING

...

23 CYCL CALL

...

26 CYCL DEF 24 SIDE FINISHING

...

27 CYCL CALL

...

50 L Z+250 R0 FMAX M2

51 LBL 1

...

55 LBL 0

56 LBL 2

...

60 LBL 0

...

99 END PGM SL2 MM

Notes

  • The memory capacity for programming an SL cycle is limited. You can program up to 16384 contour elements in one SL cycle.
  • SL Cycles conduct comprehensive and complex internal calculations as well as the resulting machining operations. For safety reasons, always use the simulation to verify your program before running it. This is a simple way of finding out whether the program calculated by the control will provide the desired results.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.