Cycle 4 MEASURING IN 3-D (#17 / #1-05-1)

ISO programming

NC syntax is available only in Klartext programming.

Application

Touch probe cycle 4 measures any position on the workpiece in the probing direction defined by a vector. Unlike other touch probe cycles, Cycle 4 enables you to enter the probing distance and probing feed rate directly. You can also define the distance by which the touch probe retracts after acquiring the probed value.

Cycle 4 is an auxiliary cycle that can be used for probing with any touch probe (TS or TT). The control does not provide a cycle for calibrating the TS touch probe in any probing direction.

Cycle sequence

  1. The control moves the touch probe from the current position at the entered feed rate in the defined probing direction. Define the probing direction in the cycle by using a vector (delta values in X, Y and Z).
  2. After the control has saved the position, the control stops the probe movement. The control saves the X, Y, Z coordinates of the probing position in three successive Q parameters. You define the number of the first parameter in the cycle. If you are using a TS touch probe, the probe result is corrected by the calibrated center offset.
  3. Finally, the control retracts the touch probe in the direction opposite to the direction of probing. You define the traverse distance in parameter MB—the touch probe is moved to a point no farther than the starting point.
 
Tip

Ensure during pre-positioning that the control moves the probe-tip center without compensation to the defined position.

Notes

 
Notice
Danger of collision!
If the control was not able to determine a valid touch point, the 4th result parameter will have the value –1. The control does not interrupt the program run! There is a danger of collision!
  1. Make sure that all touch points can be reached.
  • This cycle can be executed only in the FUNCTION MODE MILL and FUNCTION MODE TURN machining modes.
  • The control retracts the touch probe by at most the retraction distance MB, but not beyond the starting point of the measurement. This rules out any collision during retraction.
  • Remember that the control always writes to four successive Q parameters.

Cycle parameters

Help graphic

Parameter

Parameter number for result?

Enter the number of the Q parameter to which you want the control to assign the first measured coordinate (X). The Y and Z values, as well as the reaction, will be written to the immediately following Q parameters.

Input: 0...1999

Relative measuring path in X?

X component of the direction vector defining the direction in which the touch probe will move.

Input: –999999999...+999999999

Relative measuring path in Y?

Y component of the direction vector defining the direction in which the touch probe will move.

Input: –999999999...+999999999

Relative measuring path in Z?

Z component of the direction vector defining the direction in which the touch probe will move.

Input: –999999999...+999999999

Maximum measuring range?

Enter the maximum distance from the starting point by which the touch probe will move along the direction vector.

Input: –999999999...+999999999

Feed rate measurement

Enter the measuring feed rate in mm/min.

Input: 0...3000

Maximum retraction distance?

Traverse path in the direction opposite the probing direction, after the stylus was deflected.

Input: 0...999999999

Reference system? (0=ACT/1=REF)

Define whether the result of probing will be saved in the input coordinate system (ACT), or with respect to the machine coordinate system (REF):

0: Save the measurement result in the ACT system

1: Save the measurement result in the REF system

Input: 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.

 
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 4.0 MEASURING IN 3-D

12 TCH PROBE 4.1 Q1

13 TCH PROBE 4.2 IX-0.5 IY-1 IZ-1

14 TCH PROBE 4.3 ABST+45 F100 MB50 REFERENCE SYSTEM:0