Cycle 3 MEASURING (#17 / #1-05-1)

ISO programming

NC syntax is available only in Klartext programming.

Application

Touch probe cycle 3 measures any position on the workpiece in a selectable probing direction. Unlike other touch probe cycles, Cycle 3 enables you to enter the measuring range SET UP and feed rate F directly. Also, the touch probe retracts by a definable value MB after determining the measured value.

Cycle sequence

  1. The touch probe moves from the current position at the specified feed rate in the defined probing direction. Use polar angles to define the probing direction in the cycle.
  2. After the control has saved the position, the touch probe stops. The control saves the X, Y, Z coordinates of the probe-tip center in three successive Q parameters. The control does not conduct any length or radius compensations. You define the number of the first result parameter in the cycle.
  3. Finally, the control retracts the touch probe by the value that you defined in parameter MB in the direction opposite to the probing direction.

Return parameters

Q parameter
number

Meaning

Q1*

First measured position in the X axis

Q2*

First measured position in the Y axis

Q3*

First measured position in the Z axis

Q4*

Result

  • 0: Valid probing result
  • -1: No touch point found, stylus not deflected
  • -2: Stylus already deflected at beginning of cycle

*The number of the Q parameter can deviate from this example. You define the number of the first result parameter in the cycle under 3.1. The further results are in the immediately following Q parameters.

Notes

 
Machine

The exact behavior of touch probe cycle 3 is defined by your machine manufacturer or a software manufacturer who uses it within specific touch probe cycles.

  • This cycle can be executed only in the FUNCTION MODE MILL and FUNCTION MODE TURN machining modes.
  • The DIST (maximum traverse to touch point) and F (probing feed rate) touch-probe data, which are effective in other touch probe cycles, do not apply in touch probe cycle 3.
  • Remember that the control always writes to four successive Q parameters.
  • If the control was not able to determine a valid touch point, the NC program is run without an error message. In this case the control assigns the value –1 to the fourth result parameter so that you can deal with the error yourself.
  • 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.
 
Tip

The FN 17: SYSWRITE ID990 NR6 function allows setting whether the cycle runs through the probe input X12 or X13.

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

Return parameters

Probing axis?

Enter the axis in whose direction the touch probe will move and confirm with the ENT key.

Input: X, Y, or Z

Probing angle?

This angle defines the probing direction. The angle refers to the probe axis. Confirm with the ENT key.

Input: -180...+180

Maximum measuring range?

Enter the maximum distance from the starting point by which the touch probe will move. Confirm with ENT.

Input: 0...999999999

Feed rate measurement

Enter the measuring feed rate in mm/min.

Input: 0...3000

Maximum retraction distance?

Traverse path in the direction opposite to the probing direction, after the stylus was deflected. The control returns the touch probe to a point no farther than the starting point, so that there can be no collision.

Input: 0...999999999

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

Define whether the probing direction and measurement result will be referenced to the current coordinate system (ACT, can be shifted or rotated) or the machine coordinate system (REF):

0: Perform the probing operation in the current system and save the measurement result in the ACT system

1: Perform the probing operation in the machine-based REF system. Save the measurement result in the REF system.

Input: 0, 1

Error mode? (0=OFF/1=ON)

Define whether the control will issue an error message if the stylus is deflected at cycle start. If mode 1 is selected, the control saves the value -2 in the 4th result parameter and continues the cycle:

0: Issue error message

1: Do not issue error message

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 3.0 MEASURING

12 TCH PROBE 3.1 Q1

13 TCH PROBE 3.2 X ANGLE:+15

14 TCH PROBE 3.3 ABST+10 F100 MB1 REFERENCE SYSTEM:0

15 TCH PROBE 3.4 ERRORMODE1