Cycle 401 ROT OF 2 HOLES (#17 / #1-05-1)

ISO programming

G401

Application

Touch probe cycle 401 measures the center points of two holes. The control then calculates the angle between the main axis of the working plane and the line connecting the hole center points. With the basic rotation function, the control compensates for the calculated value. As an alternative, you can also compensate for the determined misalignment by rotating the rotary table.

 
Tip

Instead of Cycle 401 ROT OF 2 HOLES, HEIDENHAIN recommends using the more powerful Cycle 1411 PROBING TWO CIRCLES.

Cycle run

  1. The control positions the touch probe at the entered center of the first hole 1, using positioning logic.
  2. Positioning logic

  3. Then the probe moves to the entered measuring height and probes four points to determine the first hole center point.
  4. The touch probe returns to the clearance height and then to the position entered as center of the second hole 2.
  5. The control moves the touch probe to the entered measuring height and probes four points to determine the second hole center point.
  6. Then the control returns the touch probe to the clearance height and performs the calculated basic rotation.

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.
  • If you want to compensate for the misalignment by rotating the rotary table, the control will automatically use the following rotary axes:
    • C for tool axis Z
    • B for tool axis Y
    • A for tool axis X

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

Q268 1st hole: center in 1st axis?

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

Input: –99999.9999...+9999.9999

Q269 1st hole: center in 2nd axis?

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

Input: –99999.9999...+99999.9999

Q270 2nd hole: center in 1st axis?

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

Input: –99999.9999...+99999.9999

Q271 2nd hole: center in 2nd axis?

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

Input: –99999.9999...+99999.9999

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

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

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 Number in table?

Enter the number of a row in the preset table. The control will make the corresponding entry in the following row:

Q305 = 0: The rotary axis will be zeroed in row 0 of the preset table. The control will make an entry in the OFFSET column. (Example: For tool axis Z, the entry is made in C_OFFS). 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: The rotary axis will be zeroed in the preset table row specified here. The control will make an entry in the corresponding OFFSET column of the preset table. (Example: For tool axis Z, the entry is made in C_OFFS).

Q305 depends on the following parameters:

  • Q337 = 0 and, at the same time, Q402 = 0: A basic rotation will be set in the row specified in Q305. (Example: For tool axis Z, the basic rotation is entered in the SPC column).
  • Q337 = 0 and, at the same time, Q402 = 1: The parameter Q305 is not effective.
  • Q337 = 1: The parameter Q305 has the effect described above.

Input: 0...99999

Q402 Basic rotation/alignment (0/1)

Define whether the control will set the determined misalignment as a basic rotation or will compensate for it by rotating the rotary table:

0: Set basic rotation: The control saves the basic rotation (example: for tool axis Z, the control uses column SPC)

1: Rotate the rotary table: An entry will be made in the corresponding Offset column of the preset table (example: for tool axis Z, the control uses the C_OFFS column); in addition, the corresponding axis will be rotated

Input: 0, 1

Q337 Set to zero after alignment?

Define whether the control will set the position display of the corresponding rotary axis to 0 after the alignment:

0: The position display is not set to 0 after the alignment

1: After the alignment, the position display is set to 0, provided you have defined Q402 = 1

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 401 ROT OF 2 HOLES ~

Q268=-37

;1ST CENTER 1ST AXIS ~

Q269=+12

;1ST CENTER 2ND AXIS ~

Q270=+75

;2ND CENTER 1ST AXIS ~

Q271=+20

;2ND CENTER 2ND AXIS ~

Q261=-5

;MEASURING HEIGHT ~

Q260=+20

;CLEARANCE HEIGHT ~

Q307=+0

;PRESET ROTATION ANG. ~

Q305=+0

;NUMBER IN TABLE ~

Q402=+0

;COMPENSATION ~

Q337=+0

;SET TO ZERO