Cycle 403 ROT IN ROTARY AXIS (#17 / #1-05-1)

ISO programming

G403

Application

Touch probe cycle 403 determines a workpiece misalignment by measuring two points, which must lie on a straight line. The control compensates for the determined misalignment by rotating the A, B, or C axis. The workpiece can be clamped in any position on the rotary table.

 
Tip

Instead of Cycle 403 ROT IN ROTARY AXIS, HEIDENHAIN recommends using the more powerful cycles below:

  • 1410 PROBING ON EDGE
  • 1412 INCLINED EDGE PROBING

Cycle run

  1. The control positions the touch probe to the pre-position of the first touch point 1, using positioning logic.
  2. Positioning logic

  3. Next, the touch probe moves to the entered measuring height and probes the first touch point at the probing feed rate (F column).
  4. The touch probe then moves to the next touch point 2 and probes again.
  5. The control returns the touch probe to the clearance height and rotates the rotary axis, which was defined in the cycle, by the measured value. Optionally, you can specify whether the control is to set the determined rotation angle to 0 in the preset table or in the datum table.

Notes

 
Notice
Danger of collision!
If the control positions the rotary axis automatically, a collision might occur.
  1. Pay attention to possible collisions between the tool and any elements attached to the table
  2. Use a sufficient clearance height so that no collisions can occur
 
Notice
Danger of collision!
If you set parameter Q312 Axis for compensating movement? to 0, then the cycle will automatically determine the rotary axis to be aligned (recommended setting). When doing so, it determines an angle that depends on the sequence of the touch points. The measured angle goes from the first to the second touch point. If you select the A, B or C axis as compensation axis in parameter Q312, the cycle determines the angle, regardless of the sequence of the touch points. The calculated angle is in the range of –90° to +90°. There is a risk of collision!
  1. After alignment, check the position of the rotary axis.
 
Notice
Danger of collision!
During execution of touch probe cycles 400 to 499, all coordinate transformation cycles must be inactive. Otherwise, there is a danger of collision!
  1. 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
  2. Reset any coordinate transformations beforehand.
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The control will reset an active basic rotation at the beginning of the cycle.

Note regarding machine parameters

  • In the optional machine parameter trackAsync (no. 122503), the machine manufacturer defines whether the control orients the spindle for probing during prepositioning. The setting takes effect only if the control uses the active kinematics to determine the rotary axis to be aligned (Q312=0).

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

Q265 2nd measuring point in 1st axis?

Coordinate of the second touch point in the main axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q266 2nd measuring point in 2nd axis?

Coordinate of the second touch point in the secondary axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q272 Meas. axis (1/2/3, 1=ref. axis)?

Axis in which the measurement will be made:

1: Main axis = measuring axis

2: Secondary axis = measuring axis

3: Touch probe axis = measuring axis

Input: 1, 2, 3

Q267 Trav. direction 1 (+1=+ / -1=-)?

Direction in which the touch probe will approach the workpiece:

–1: Negative traverse direction

+1: Positive traverse direction

Input: –1, +1

Q261 Measuring height in probe axis?

Coordinate of the ball tip center in the touch probe axis in which the measurement will be performed. 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

Q301 Move to clearance height (0/1)?

Define how the touch probe will move between the measuring points:

0: Move to measuring height between measuring points

1: Move to clearance height between measuring points

Input: 0, 1

Q312 Axis for compensating movement?

Define the rotary axis in which the control will compensate for the measured misalignment:

0: Automatic mode – the control uses the active kinematics to determine the rotary axis to be aligned. In Automatic mode the first rotary axis of the table (as viewed from the workpiece) is used as compensation axis. This is the recommended setting!

4: Compensate for misalignment with rotary axis A

5: Compensate for misalignment with rotary axis B

6: Compensate for misalignment with rotary axis C

Input: 0, 4, 5, 6

Q337 Set to zero after alignment?

Define whether the control will set the angle of the aligned rotary axis to 0 in the preset table or in the datum table after the alignment.

0: Do not set the angle of the rotary axis to 0 in the table after the alignment

1: Set the angle of the rotary axis to 0 in the table after the alignment

Input: 0, 1

Q305 Number in table?

Specify the number of the row in the preset table in which the control will enter the basic rotation.

Q305 = 0: The rotary axis is zeroed in row number 0 of the preset table. The control will make an entry in the OFFSET column. In addition, all other values (X, Y, Z, etc.) of the currently active preset will be transferred to row 0 of the preset table. In addition, the control activates the preset from row 0.

Q305 > 0: Specify the number of the row in the preset table in which the control will zero the rotary axis. The control will make an entry in the OFFSET column of the preset table.

Q305 depends on the following parameters:

  • Q337 = 0: Parameter Q305 is not effective
  • Q337 = 1: Parameter Q305 has the effect described above
  • Q312 = 0: Parameter Q305 has the effect described above
  • Q312 > 0: The entry in Q305 is ignored. The control will make an entry in the OFFSET column, in the row of the preset table that was active when the cycle was called.

Input: 0...99999

Q303 Meas. value transfer (0,1)?

Define whether the calculated preset will be saved in the datum table or in the preset table:

0: Write the calculated preset to the active datum table as a datum shift. The reference system is the active workpiece coordinate system.

1: Write the calculated preset to the preset table.

Input: 0, 1

Q380 Ref. angle in ref. axis?

Angle to which the control will align the probed straight line. Only effective if the rotary axis is in automatic mode or if C is selected (Q312 = 0 or 6).

Input: 0...360

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 403 ROT IN ROTARY AXIS ~

Q263=+0

;1ST POINT 1ST AXIS ~

Q264=+0

;1ST POINT 2ND AXIS ~

Q265=+20

;2ND PNT IN 1ST AXIS ~

Q266=+30

;2ND POINT 2ND AXIS ~

Q272=+1

;MEASURING AXIS ~

Q267=-1

;TRAVERSE DIRECTION ~

Q261=-5

;MEASURING HEIGHT ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+20

;CLEARANCE HEIGHT ~

Q301=+0

;MOVE TO CLEARANCE ~

Q312=+0

;COMPENSATION AXIS ~

Q337=+0

;SET TO ZERO ~

Q305=+1

;NUMBER IN TABLE ~

Q303=+1

;MEAS. VALUE TRANSFER ~

Q380=+90

;REFERENCE ANGLE