Cycle 1 POLAR PRESET (#17 / #1-05-1)
ISO programming
NC syntax is available only in Klartext programming.
Application
Cycle sequence
- 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.
- 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.
- 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
- 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.
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 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 |