Cycle 412 PRESET INSIDE CIRCLE (#17 / #1-05-1)

ISO programming

G412

Application

Touch probe cycle 412 finds the center of a circular pocket (hole) and defines this position as the preset. If desired, the control can also write the center point coordinates to a datum table or the preset table.

 
Tip

Instead of Cycle 412 PRESET INSIDE CIRCLE, HEIDENHAIN recommends using the more powerful Cycle 1401 CIRCLE 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). 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.
  6. The control returns the touch probe to the clearance height.
  7. Depending on the cycle parameters Q303 and Q305, the control processes the determined preset, (see Fundamentals of touch probe cycles 408 to 419 for preset setting).
  8. Then the control saves the actual values in the Q parameters listed below.
  9. If desired, the control subsequently determines the preset in the touch probe axis in a separate probing operation.

Q parameter
number

Meaning

Q151

Actual value of center in reference axis

Q152

Actual value of center in minor axis

Q153

Actual value of diameter

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.
 
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).
  • 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 Q247, the less accurately the control can calculate the preset. Minimum input value: 5°
 
Tip

Program the stepping angle to be less than 90°.

Cycle parameters

Help graphic

Parameter

Q321 Center in 1st axis?

Center of the pocket 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 pocket in the secondary axis of the working plane. If you program Q322 = 0, the control aligns the hole center point to the positive Y axis. If you program Q322 not equal to 0, then the control aligns the hole center point to the nominal position. 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

Q305 Number in table?

Enter the row number from the preset table / datum table in which the control saves the center coordinates. Depending on Q303, the control writes the entry to the preset table or datum table.

If Q303=1, the control will write the data to the preset table.

If Q303=0, then the control describes the datum table. The datum is not automatically activated.

Saving the calculated preset

Input: 0...99999

Q331 New preset in reference axis?

Coordinate in the main axis at which the control will set the calculated pocket center. Default setting = 0. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q332 New preset in minor axis?

Coordinate in the secondary axis at which the control will set the calculated pocket center. Default setting = 0. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q303 Meas. value transfer (0,1)? (optional)

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

-1: Do not use. Is entered by the control when old NC programs are loaded see Application

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

1: Write the calculated preset to the preset table.

Input: -1, 0, +1

Q381 Probe in TS axis? (0/1) (optional)

Define whether the control will also set the preset in the touch probe axis:

0: Do not set the preset in the touch probe axis

1: Set the preset in the touch probe axis

Input: 0, 1

Q382 Probe TS axis: Coord. 1st axis? (optional)

Coordinate of the touch point in the main axis of the working plane; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q383 Probe TS axis: Coord. 2nd axis? (optional)

Coordinate of the touch point in the secondary axis of the working plane; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q384 Probe TS axis: Coord. 3rd axis? (optional)

Coordinate of the touch point in the touch probe axis; the preset will be set at this point in the touch probe axis. Only effective if Q381 = 1. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q333 New preset in TS axis? (optional)

Coordinate in the touch probe axis at which the control will set the preset. Default setting = 0. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q423 No. probe points in plane (4/3)? (optional)

Define whether the control will use three or four touch points to measure the circle:

3: Use three measuring points

4: Use four measuring points (default setting)

Input: 3, 4

Q365 Type of traverse? Line=0/arc=1 (optional)

Specify the path function to be used by the tool for moving between the measuring points if "traverse to clearance height" (Q301 = 1) is active.

0: Move in a straight line between machining operations

1: Move along a circular arc on the pitch circle diameter between machining operations

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 412 PRESET INSIDE CIRCLE ~

Q321=+50

;CENTER IN 1ST AXIS ~

Q322=+50

;CENTER IN 2ND AXIS ~

Q262=+75

;NOMINAL DIAMETER ~

Q325=+0

;STARTING ANGLE ~

Q247=+60

;STEPPING ANGLE ~

Q261=-5

;MEASURING HEIGHT ~

Q320=+0

;SET-UP CLEARANCE ~

Q260=+20

;CLEARANCE HEIGHT ~

Q301=+0

;MOVE TO CLEARANCE ~

Q305=+12

;NUMBER IN TABLE ~

Q331=+0

;PRESET ~

Q332=+0

;PRESET ~

Q303=+1

;MEAS. VALUE TRANSFER ~

Q381=+1

;PROBE IN TS AXIS ~

Q382=+85

;1ST CO. FOR TS AXIS ~

Q383=+50

;2ND CO. FOR TS AXIS ~

Q384=+0

;3RD CO. FOR TS AXIS ~

Q333=+1

;PRESET ~

Q423=+4

;NO. OF PROBE POINTS ~

Q365=+1

;TYPE OF TRAVERSE