Cycle 1400 POSITION PROBING

Application

Touch probe cycle 1400 measures any position in a selectable axis. You can apply the result to the active row of the preset table.

If you program Cycle 1493 EXTRUSION PROBING before this cycle, you can repeat probing points in a given direction over a specified distance.

Cycle 1493 EXTRUSION PROBING

Cycle sequence

cyc1400
  1. Following the positioning logic, the control positions the touch probe at rapid traverse (value from the FMAX column) to the programmed touch point 1. The control takes into account the set-up clearance Q320 during pre-positioning.
  2. Positioning logic

  3. Then the touch probe moves to the entered measuring height and measures the actual position with a single probing movement.
  4. The control returns the touch probe to the clearance height.
  5. The control saves the measured position in the following Q parameters. If Q1120 = 1, then the control writes the measured position to the active row of the preset table.
  6. Fundamentals of touch probe cycles 14xx for presetting

Q parameter
number

Meaning

Q950 to Q952

Measured position 1 in the main axis, secondary axis, and tool axis

Q980 to Q982

Measured deviations of touch point 1

Q183

  • Workpiece status
  • –1 = Not defined
  • 0 = Good
  • 1 = Rework
  • 2 = Scrap

Q970

If you have programmed Cycle 1493 EXTRUSION PROBING:

Mean value of all deviations from the ideal line of the second touch point

Notes

 
Notice
Danger of collision!
When running touch probe cycles 444 and 14xx, no coordinate transformations must be active (e.g., Cycles 8 MIRRORING, 11 SCALING FACTOR, 26 AXIS-SPECIFIC SCALING, TRANS MIRROR).
  1. Reset any coordinate transformations before the cycle call.
  • This cycle can only be executed in the FUNCTION MODE MILL machining mode.

Cycle parameters

Help graphic

Parameter

cyc1400_1

Q1100 1st noml. position of ref. axis?

Absolute nominal position of the first touch point in the main axis of the working plane

Input: –99999.9999...+99999.9999 or optionally ?, -, +, @

?: Semiautomatic mode, Semi-automatic mode

-, +: Evaluation of the tolerance, Evaluation of tolerances

@: Transferring the actual position, Transferring the actual position

Q1101 1st noml. position of minor axis?

Absolute nominal position of the first touch point in the secondary axis of the working plane

Input: –99999.9999...+9999.9999 or optional input (see Q1100)

Q1102 1st nominal position tool axis?

Absolute nominal position of the first touch point in the tool axis

Input: –99999.9999...+9999.9999 or optional input (see Q1100)

cyc1400_2

cyc1400_3

Q372 Probe direction (–3 to +3)?

Axis defining the direction of probing. With the algebraic sign, you define the positive or negative direction of traverse of the probing axis.

Input: –3, -2, -1, +1, +2, +3

Q320 Set-up clearance?

Additional distance between touch point and ball tip. Q320 is 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. The value has an absolute effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q1125 Traverse to clearance height?

Positioning behavior between the touch points:

–1: Do not move to clearance height.

0, 1, 2: Move to clearance height before and after the touch point. Pre-positioning occurs at FMAX_PROBE.

Input: –1, 0, +1, +2

Q309 Reaction to tolerance error?

Reaction when tolerance is exceeded:

0: Do not interrupt program run when tolerance is exceeded. The control does not open a window with the results.

1: Interrupt program run when tolerance is exceeded. The control opens a window with the results.

2: The control opens a window with the results if the actual position is in the scrap range. Program run is interrupted. The control does not open a window with the results if rework is necessary.

Input: 0, 1, 2

Q1120 Transfer position?

Define which touch point will be used to correct the active preset:

0: No correction

1: Correction based on the 1st touch point

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 1400 POSITION PROBING ~

Q1100=+25

;1ST POINT REF AXIS ~

Q1101=+25

;1ST POINT MINOR AXIS ~

Q1102=-5

;1ST POINT TOOL AXIS ~

Q372=+0

;PROBING DIRECTION ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+50

;CLEARANCE HEIGHT ~

Q1125=+1

;CLEAR. HEIGHT MODE ~

Q309=+0

;ERROR REACTION ~

Q1120=+0

;TRANSER POSITION