Cycle 11 SCALING FACTOR

ISO programming

G72

Application

The control can increase or reduce the size of contours within an NC program. This enables you to program shrinkage and oversize allowances.

The scaling factor takes effect as soon as it has been defined in the NC program. It is also in effect in the Manual operating mode in the MDI application. The active scaling factor is shown in the additional status display.

The scaling factor has an effect on

  • all three coordinate axes at the same time
  • dimensions in cycles

Requirement

It is advisable to set the datum to an edge or a corner of the contour before enlarging or reducing the contour.

Enlargement: SCL greater than 1 (up to 99.999 999)

Reduction: SCL less than 1 (down to 0.000 001)

 
Tip

This cycle can be executed only in the FUNCTION MODE MILL machining mode.

Reset

Program Cycle 11 SCALING FACTOR again and specify a scaling factor of 1.

Cycle parameters

Help graphic

Parameter

Factor?

Enter the scaling factor SCL. The control multiplies the coordinates and radii with SCL.

Input: 0.000001...99.999999

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.

Example

11 CYCL DEF 11.0 SCALING FACTOR

12 CYCL DEF 11.1 SCL 0.75