Cycle 405 ROT IN C AXIS (#17 / #1-05-1)

ISO programming

G405

Application

With touch probe cycle 405, you can measure

  • the angular offset between the positive Y axis of the active coordinate system and the center line of a hole
  • the angular offset between the nominal position and the actual position of a hole center point

The control compensates for the determined angular offset by rotating the C axis. The workpiece can be clamped in any position on the rotary table, but the Y coordinate of the hole must be positive. If you measure the angular misalignment of the hole with touch probe axis Y (horizontal position of the hole), it may be necessary to execute the cycle more than once because the measuring strategy causes an inaccuracy of approx. 1% of the misalignment.

 
Tip

Instead of Cycle 405 ROT IN C AXIS, HEIDENHAIN recommends using the more powerful Cycle 1411 PROBING TWO CIRCLES.

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). The control derives the probing direction automatically from the programmed starting angle.
  4. Then, the touch probe moves along a circular arc, either at measuring height or at clearance height, to the next touch point 2 and probes again.
  5. The control positions the touch probe to touch point 3 and then to touch point 4 to probe two more times and then positions the touch probe on the calculated hole center.
  6. Finally, the control returns the touch probe to the clearance height and aligns the workpiece by rotating the rotary table. The control rotates the rotary table in such a way that the hole center, after compensation, lies in the direction of the positive Y axis or at the nominal position of the hole center point—both with a vertical and a horizontal touch probe axis. The measured angular offset is also available in the parameter Q150.

Notes

 
Notice
Danger of collision!
If the dimensions of the pocket and the set-up clearance do not permit pre-positioning in the proximity of the touch points, the control always starts probing from the center of the pocket. In this case, the touch probe does not return to the clearance height between the four measuring points. There is a risk of collision!
  1. The pocket/hole must be free of material on the inside
  2. To prevent a collision between the touch probe and the workpiece, enter a low estimate for the nominal diameter of the pocket (or hole).
 
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.

Notes on programming

  • The smaller the stepping angle, the less accurately the control can calculate the circle center point. Minimum input value: 5°.

Cycle parameters

Help graphic

Parameter

Q321 Center in 1st axis?

Center of the hole in the main axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q322 Center in 2nd axis?

Center of the hole in the secondary axis of the working plane. If you program Q322 = 0, the control aligns the hole center point with the positive Y axis. If you program Q322 not equal to 0, then the control aligns the hole center point with the nominal position (angle resulting from the position of the hole center). This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q262 Nominal diameter?

Approximate diameter of the circular pocket (or hole). Enter a value that is more likely to be too small than too large.

Input: 0...99999.9999

Q325 Starting angle?

Angle between the main axis of the working plane and the first touch point. This value has an absolute effect.

Input: –360.000...+360.000

Q247 Intermediate stepping angle?

Angle between two measuring points. The algebraic sign of the stepping angle determines the direction of rotation (negative = clockwise) in which the touch probe moves to the next measuring point. If you wish to probe a circular arc instead of a complete circle, then program the stepping angle to be less than 90°. This value has an incremental effect.

Input: –120...+120

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

Q337 Set to zero after alignment?

0: Set the display of the C axis to 0 and write to C_Offset of the active row of the datum table

> 0: Write the measured angular offset to the datum table. Row number = value in Q337. If a C-axis shift is entered in the datum table, the control adds the measured angular offset with the correct sign, positive or negative.

Input: 0...2999

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 405 ROT IN C AXIS ~

Q321=+50

;CENTER IN 1ST AXIS ~

Q322=+50

;CENTER IN 2ND AXIS ~

Q262=+10

;NOMINAL DIAMETER ~

Q325=+0

;STARTING ANGLE ~

Q247=+90

;STEPPING ANGLE ~

Q261=-5

;MEASURING HEIGHT ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+20

;CLEARANCE HEIGHT ~

Q301=+0

;MOVE TO CLEARANCE ~

Q337=+0

;SET TO ZERO