Simple contour formula

Fundamentals

Using simple contour formulas, you can easily combine up to nine subcontours (pockets or islands) to program a particular contour. The control calculates the complete contour from the selected subcontours.

Program structure: Machining with SL Cycles and simple contour formula

0 BEGIN CONTDEF MM

...

5 CONTOUR DEF

...

6 CYCL DEF 20 CONTOUR DATA

...

8 CYCL DEF 21 ROUGH-OUT

...

9 CYCL CALL

...

13 CYCL DEF 23 FLOOR FINISHING

...

14 CYCL CALL

...

16 CYCL DEF 24 SIDE FINISHING

...

17 CYCL CALL

...

50 L Z+250 R0 FMAX M2

51 END PGM CONTDEF MM

 
Tip

The memory capacity for programming an SL cycle (all contour description programs) is limited to 100 contours. The number of possible contour elements depends on the type of contour (inside or outside contour) and the number of contour descriptions. You can program up to 16384 contour elements.

Void areas

Using optional void areas V (void), you can exclude areas from machining. These areas can be, for example, contours in castings or areas machined in previous steps. You can define up to five void areas.

If you are using OCM cycles, the control will plunge vertically within void areas.

If you are using SL Cycles 22 to 24, the control will determine the plunging position, regardless of any defined void areas.

Run the simulation to verify proper behavior.

Properties of the subcontours

  • Do not program radius compensation.
  • The control ignores feed rates F and miscellaneous functions M.
  • 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.
  • Although the subprograms can contain coordinates in the spindle axis, such coordinates are ignored.
  • The working plane is defined in the first coordinate block of the subprogram.

Cycle properties

  • The control automatically positions the tool to the set-up clearance before a cycle.
  • Each level of infeed depth is milled without interruptions; 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 dimensions, such as milling depth, allowances, and clearance height, can be entered centrally in Cycle 20 CONTOUR DATA or 271 OCM CONTOUR DATA.

Entering a simple contour formula

You can use the selection possibility in the action bar or in the form to interlink various contours in a mathematical formula.

Proceed as follows:

  1. Select Insert NC function
  2. The control opens the Insert NC function window.
  3. Select CONTOUR DEF
  4. The control opens the dialog for entering the contour formula.
  5. Enter the first subcontour P1

  1. Select the P2 pocket or I2 island selection possibility
  2. Enter second subcontour
  3. If needed, enter the depth of the second subcontour.
  4. Carry on with the dialog as described above until you have entered all subcontours.
  5. Define void areas V as needed
  6.  
    Tip

    The depth of the void areas corresponds to the total depth that you define in the machining cycle.

You can enter contours in the following ways:

Possible setting

Function

File

  • Input
  • File selection

Define the name of the contour or select File Selection

QS

Define the number of a QS parameter

LBL

  • Number
  • Name
  • Parameter

Define the number, name or variable of a label

Example:

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

11 CONTOUR DEF P1 = LBL 1 I2 = LBL 2 DEPTH5 V1 = LBL 3

 
Tip

Programming notes:

  • The first depth of the subcontour is the cycle depth. This is the maximum depth for the programmed contour. Other subcontours cannot be deeper than the cycle depth Therefore, always start programming the subcontour with the deepest pocket.
  • If the contour is defined as an island, the control interprets the entered depth as the island height. The entered value (without an algebraic sign) then refers to the workpiece top surface!
  • If you enter a value of 0 for the depth, then the depth defined in Cycle 20 is in effect for pockets. For islands, this means that they extend up to the workpiece surface!
  • If the called file is located in the same directory as the file you are calling it from, you can also integrate the file name without the path.

Machining contours with SL or OCM cycles