Cycle 1 POLAR PRESET (#17 / #1-05-1)

ISO programming

NC syntax is available only in Klartext programming.

Application

Touch probe cycle 1 measures any position on the workpiece in any probing direction.

Cycle sequence

  1. In a 3D movement, the touch probe moves at rapid traverse (value from the FMAX column) to the pre-position 1 programmed in the cycle.
  2. Next, the touch probe performs probing at the probing feed rate (F column). During probing, the control moves the touch probe simultaneously in two axes (depending on the probing angle). Use polar angles to define the probing direction in the cycle.
  3. After the control has saved the position, the touch probe returns to the starting point. The control stores the coordinates of the position of the touch probe at the time of the triggering signal in parameters Q115 to Q119.

Notes

 
Notice
Danger of collision!
The control moves the touch probe in a 3D movement at rapid traverse to the pre-position programmed in the cycle. Depending on the previous position of the tool, there is danger of collision!
  1. Pre-position to a position where there is no danger of collision when the programmed pre-positioning point is approached
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The probing axis defined in the cycle specifies the probing plane:
    Probing axis X: X/Y plane
    Probing axis Y: Y/Z plane
    Probing axis Z: Z/X plane

Cycle parameters

Help graphic

Parameter

Probing axis?

Enter the probing axis with the axis key or the alphabetic keyboard. Confirm with the ENT key.

Input: X, Y, or Z

Probing angle?

Angle measured from the probing axis in which the touch probe will move.

Input: -180...+180

Position value?

Use the axis keys or the alphabetic keyboard to enter all coordinates for pre-positioning of the touch probe.

Input: –999999999...+999999999

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 TCH PROBE 1.0 POLAR PRESET

12 TCH PROBE 1.1 X ANGLE:+30

13 TCH PROBE 1.2 X+0 Y+10 Z+3