Cycle 400 BASIC ROTATION (#17 / #1-05-1)

ISO programming

G400

Application

Touch probe cycle 400 determines a workpiece misalignment by measuring two points, which must lie on a straight line. With the basic rotation function, the control corrects the measured value.

 
Tip

Instead of Cycle 400 BASIC ROTATION, 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 performs the basic rotation it determined.

Notes

 
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 on programming

  • Before defining this cycle, you must have programmed a tool call to define the touch probe axis.

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 Measuring axis (1=1st / 2=2nd)?

Axis in the working plane in which the measurement will be performed:

1: Main axis = measuring axis

2: Secondary axis = measuring axis

Input: 1, 2

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

Q307 Preset value for rotation angle

If the misalignment is measured relative to any straight line other than the main axis, enter the angle of this reference line. For the basic rotation, the control will then calculate the difference between the value measured and the angle of the reference line. This value has an absolute effect.

Input: –360.000...+360.000

Q305 Preset number in table?

Specify the number of the row in the preset table in which the control will save the calculated basic rotation. If you enter Q305 = 0, the control automatically stores the calculated basic rotation in the ROT menu of the Manual Operation mode.

Input: 0...99999

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 400 BASIC ROTATION ~

Q263=+10

;1ST POINT 1ST AXIS ~

Q264=+3.5

;1ST POINT 2ND AXIS ~

Q265=+25

;2ND POINT 1ST AXIS ~

Q266=+2

;2ND PNT IN 2ND AXIS ~

Q272=+2

;MEASURING AXIS ~

Q267=+1

;TRAVERSE DIRECTION ~

Q261=-5

;MEASURING HEIGHT ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+20

;CLEARANCE HEIGHT ~

Q301=+0

;MOVE TO CLEARANCE ~

Q307=+0

;PRESET ROTATION ANG. ~

Q305=+0

;NUMBER IN TABLE