Cycle 417 PRESET IN TS AXIS (#17 / #1-05-1)
ISO programming
G417
Application
Touch probe cycle 417 measures any coordinate in the touch probe axis and defines it as the preset. If desired, the control can also write the measured coordinates to a datum table or preset table.
Instead of Cycle 417 PRESET IN TS AXIS, HEIDENHAIN recommends using the more powerful Cycle 1400 POSITION PROBING.
Related topics
- Cycle 1400 POSITION PROBING
Cycle run
- Following the positioning logic, the control positions the touch probe to the programmed touch point 1. In this process, the control offsets the touch probe by the set-up clearance in the direction of the positive touch probe axis.
- Then the touch probe moves in its own axis to the coordinate entered as touch point 1 and measures the actual position with a simple probing movement.
- The control returns the touch probe to the clearance height.
- Depending on the cycle parameters Q303 and Q305, the control processes the determined preset, (see Fundamentals of touch probe cycles 408 to 419 for preset setting).
- Then the control saves the actual values in the Q parameters listed below.
Q parameter | Meaning |
---|---|
Q160 | Actual value of measured point |
Notes
- Do not activate the following cycles before the use of touch probe cycles:
- Cycle 7 DATUM SHIFT
- Cycle 8 MIRRORING
- Cycle 10 ROTATION
- Cycle 11 SCALING FACTOR
- Cycle 26 AXIS-SPECIFIC SCALING
- Reset any coordinate transformations beforehand.
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control sets the preset in this axis.
- The control will reset an active basic rotation at the beginning of the cycle.
Note on programming
- Before defining this cycle, you must have programmed a tool call to define the touch probe axis.
Cycle parameters
Help graphic | Parameter |
---|---|
Q263 1st measuring point in 1st axis? Coordinate of the first touch point in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q264 1st measuring point in 2nd axis? Coordinate of the first touch point in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q294 1st measuring point in 3rd axis? Coordinate of the first touch point in the touch probe axis. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q320 Set-up clearance? Additional distance between touch point and ball tip. Q320 is active in addition to the SET_UP column in the touch probe table. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q260 Clearance height? Coordinate in the tool axis at which no collision between touch probe and workpiece (fixtures) can occur. This value has an absolute effect. Input: –99999.9999...+99999.9999 or PREDEF | |
Q305 Number in table? Indicate the number of the row of the preset table or datum table, in which the control saves the coordinates. Depending on Q303, the control writes the entry to the preset table or datum table. If Q303 = 1, the control will write the data to the preset table. If Q303 = 0, the control will write the data to the datum table. The datum is not automatically activated. Input: 0...99999 | |
Q333 New preset in TS axis? Coordinate in the touch probe axis at which the control will set the preset. Default setting = 0. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q303 Meas. value transfer (0,1)? Define whether the calculated preset will be saved in the datum table or in the preset table: -1: Do not use. Is entered by the control when old NC programs are loaded see Application 0: Write the calculated preset to the active datum table. The reference system is the active workpiece coordinate system. 1: Write the calculated preset to the preset table. Input: -1, 0, +1 |
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 417 PRESET IN TS AXIS ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|