General information about touch probe cycles

Method of function

 
Machine
  • Refer to your machine manual.
  • The control must be specifically prepared by the machine manufacturer for the use of a 3D touch probe.
  • HEIDENHAIN guarantees the proper operation of the touch probe cycles only in conjunction with HEIDENHAIN touch probes.
  • If you are using a HEIDENHAIN touch probe with EnDat interface, then the software option Touch Probe Functions (#17 / #1-05-1) is automatically enabled.
  • The control’s full range of functions is available only if the Z tool axis is used.
  • Restricted use of the tool axes X and Y is possible when prepared and configured by the machine manufacturer.

The touch probe functions allow you to set presets on the workpiece, measure the workpiece, and determine and compensate for workpiece misalignment.

Whenever the control runs a touch probe cycle, the 3D touch probe approaches the workpiece parallel to the axis. This is also true during an active basic rotation or with a tilted working plane. The machine manufacturer will determine the probing feed rate in a machine parameter.

General information about touch probe cycles

When the probe stylus contacts the workpiece,

  • the 3D touch probe transmits a signal to the control: the coordinates of the probed position are stored,
  • the touch probe stops moving, and
  • returns to its starting position at rapid traverse.

If the stylus is not deflected within a defined distance, the control displays an error message (distance: DIST from touch probe table).

Working with an L-shaped stylus

In addition to a SIMPLE stylus, probing cycles 444 and 14xx also support the L-TYPE stylus, which is L-shaped. The L-shaped stylus must be calibrated prior to use.

HEIDENHAIN recommends calibrating the stylus with the following cycles:

Stylus orientation must be permitted via TRACK ON in the touch probe table. During the probing process, the control orients the L-shaped stylus to the given probing direction. If the probing direction is identical to the tool axis, then the control orients the touch probe to the calibration angle.

 
Tip
  • The control does not show the arm of the stylus in the simulation. The arm is the angled part of the L-shaped stylus.
  • The software option DCM (#40 / #5-03-1) does not monitor the L-shaped stylus.
  • In order to achieve maximum accuracy, the feed rate during calibration must be identical to the feed rate during probing.

Touch probe table tchprobe.tp (#17 / #1-05-1)

Notes

 
Notice
Danger of collision!
When running touch probe cycles 400 to 499, all cycles for coordinate transformation must be inactive. There is a danger of collision!
  1. The following cycles must not be activated before a touch probe cycle: Cycle 7 DATUM SHIFT, Cycle 8 MIRRORING, Cycle 10 ROTATION, Cycle 11 SCALING FACTOR, and Cycle 26 AXIS-SPECIFIC SCALING.
  2. Reset any coordinate transformations beforehand.

General information on the touch-probe table

In the touch probe table you define the set-up clearance, i.e., how far away from the defined touch point (or the one calculated by the cycle) the control will pre-position the touch probe. The smaller the value you enter, the more exactly you must define the touch point position. In many touch probe cycles, you can also define a set-up clearance that is added to the one from the touch probe table.

The following can be defined in the touch probe table:

  • Type of tool
  • Touch probe center offset
  • Spindle angle during calibration
  • Probing feed rate
  • Rapid traverse in probing cycle
  • Maximum measuring range
  • Set-up clearance
  • Feed rate for pre-positioning
  • Touch probe orientation
  • Serial number
  • Reaction in case of collision

Touch probe table tchprobe.tp (#17 / #1-05-1)

Touch probe cycles in the Manual Operation and Electronic Handwheel modes

Touch probe cycles for automatic operation

Besides the manual touch probe cycles, several cycles are available for a wide variety of applications in automatic operation:

  • Automatic measurement of workpiece misalignment
  • Automatic determination of the preset
  • Automatic workpiece inspection
  • Special functions
  • Touch probe calibration
  • Automatic kinematics measurement
  • Automatic tool measurement

Defining touch probe cycles

Like the most recent machining cycles, touch probe cycles with numbers greater than 400 use Q parameters as transfer parameters. Parameters with the same functionality, which the control requires in various cycles, always have the same number: For example, Q260 is always the clearance height, Q261 the measuring height, etc.

There are various ways to define the touch probe cycles. Touch probe cycles are programmed in the Programming mode of operation.

Defining cycles

 
Tip

For the various cycle parameters, the control provides selectable choices via the action bar or the form.

Executing touch probe cycles

All touch probe cycles are DEF-active. The control runs the cycle automatically as soon as it reads the cycle definition in the program run.

Notes

 
Notice
Danger of collision!
When running touch probe cycles 400 to 499, all cycles for coordinate transformation must be inactive. There is a danger of collision!
  1. The following cycles must not be activated before a touch probe cycle: Cycle 7 DATUM SHIFT, Cycle 8 MIRRORING, Cycle 10 ROTATION, Cycle 11 SCALING FACTOR, and Cycle 26 AXIS-SPECIFIC SCALING.
  2. Reset any coordinate transformations beforehand.
 
Notice
Danger of collision!
When touch probe cycles 444 and 14xx are executed, the following coordinate transformation must not be active: Cycle 8 MIRRORING, Cycle 11 SCALING FACTOR, Cycle 26 AXIS-SPECIFIC SCALING and TRANS MIRROR. There is a risk of collision.
  1. Reset any coordinate transformations before the cycle call.

Note regarding machine parameters

  • Depending on how the optional machine parameter chkTiltingAxes (no. 204600) is set, the control will check during probing whether the position of the rotary axes matches the tilting angles (3D-ROT). If that is not the case, the control displays an error message.

Notes in connection with programming and execution

  • Please note that the units of measure in the measuring log and in return parameters depend on the setting in the main program.
  • The touch probe cycles 40x to 43x will reset an active basic rotation at the beginning of the cycle.
  • The control interprets a basic transformation as a basic rotation, and an offset as a table rotation.
  • You can apply the inclined position as a workpiece rotation only if a table rotary axis exists on the machine and if its orientation is perpendicular to the workpiece coordinate system W-CS.
  • Comparison of offset and 3D basic rotation

Pre-positioning

Before each probing operation, the control pre-positions the touch probe.

Pre-positioning is done in the inverse probing direction.

The distance between the probing point and the pre-position results from the following values:

  • Ball-tip radius R
  • SET_UP from the touch-probe table
  • Q320 SET-UP CLEARANCE

Positioning logic

Touch-probe cycles with numbers from 400 through 499 or 1400 through 1499 pre-position the touch probe according to the following positioning logic:

Current position > Q260 CLEARANCE HEIGHT

  1. The control positions the touch probe at FMAX at the pre-position in the working plane.
  2. Pre-positioning

  3. Then, the control positions the touch probe at FMAX in the tool axis, directly at probing height.

Current position < Q260 CLEARANCE HEIGHT

  1. The control positions the touch probe at FMAX at Q260 CLEARANCE HEIGHT.
  2. The control positions the touch probe at FMAX to the pre-position in the working plane.
  3. Pre-positioning

  4. Then, the control positions the touch probe at FMAX in the tool axis, directly to the probing height.