Cycle 430 MEAS. BOLT HOLE CIRC (#17 / #1-05-1)

ISO programming

G430

Application

Touch probe cycle 430 finds the center and diameter of a bolt hole circle by probing three holes. If you define the corresponding tolerance values in the cycle, the control makes a nominal-to-actual value comparison and saves the deviation values in Q parameters.

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. The touch probe returns to the clearance height and then to the position entered as center of the third hole 3.
  7. The control moves the touch probe to the entered measuring height and probes four points to determine the third hole center point.
  8. Finally, the control returns the touch probe to the clearance height and saves the actual values and deviations in the following Q parameters:

Q parameter
number

Meaning

Q151

Actual value of center in reference axis

Q152

Actual value of center in minor axis

Q153

Actual value of bolt hole circle diameter

Q161

Deviation at center of reference axis

Q162

Deviation at center of minor axis

Q163

Deviation of bolt circle diameter

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • Cycle 430 only monitors for tool breakage; there is no automatic tool compensation.
  • 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

Q273 Center in 1st axis (nom. value)?

Bolt hole circle center (nominal value) in the main axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q274 Center in 2nd axis (nom. value)?

Bolt hole circle center (nominal value) in the secondary axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q262 Nominal diameter?

Enter the diameter of the hole.

Input: 0...99999.9999

Q291 Polar coord. angle of 1st hole?

Polar coordinate angle of the first hole center in the working plane. This value has an absolute effect.

Input: –360.000...+360.000

Q292 Polar coord. angle of 2nd hole?

Polar coordinate angle of the second hole center in the working plane. This value has an absolute effect.

Input: –360.000...+360.000

Q293 Polar coord. angle of 3rd hole?

Polar coordinate angle of the third hole center in the working plane. This value has an absolute effect.

Input: –360.000...+360.000

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

Q288 Maximum limit of size?

Maximum permissible diameter of bolt hole circle

Input: 0...99999.9999

Q289 Minimum limit of size?

Minimum permissible diameter of bolt hole circle

Input: 0...99999.9999

Q279 Tolerance for center 1st axis?

Permissible position deviation in the main axis of the working plane.

Input: 0...99999.9999

Q280 Tolerance for center 2nd axis?

Permissible position deviation in the secondary axis of the working plane.

Input: 0...99999.9999

Q281 Measuring log (0/1/2)?

Define whether the control will create a measuring log:

0: Do not create a measuring log

1: Create a measuring log: The control will save the log file named TCHPR430.TXT in the folder that also contains the associated NC program

2: Interrupt program run and display the measuring log on the control screen. Resume the NC program run with NC Start.

Input: 0, 1, 2

Q309 PGM stop if tolerance exceeded?

Define whether in the event of a violation of tolerance limits the control will interrupt program run and output an error message:

0: Do not interrupt program run; no error message

1: Interrupt program run and output an error message

Input: 0, 1

Q330 Tool for monitoring?

Define whether the control should perform tool monitoring:

0: Monitoring not active

> 0: Number or name of the tool used for machining. Via selection in the action bar, you have the option of applying a tool directly from the tool table.

Input: 0...99999.9 or max. 255 characters

Tool monitoring

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 430 MEAS. BOLT HOLE CIRC ~

Q273=+50

;CENTER IN 1ST AXIS ~

Q274=+50

;CENTER IN 2ND AXIS ~

Q262=+80

;NOMINAL DIAMETER ~

Q291=+0

;ANGLE OF 1ST HOLE ~

Q292=+90

;ANGLE OF 2ND HOLE ~

Q293=+180

;ANGLE OF 3RD HOLE ~

Q261=-5

;MEASURING HEIGHT ~

Q260=+10

;CLEARANCE HEIGHT ~

Q288=+80.1

;MAXIMUM LIMIT ~

Q289=+79.9

;MINIMUM LIMIT ~

Q279=+0.15

;TOLERANCE 1ST CENTER ~

Q280=+0.15

;TOLERANCE 2ND CENTER ~

Q281=+1

;MEASURING LOG ~

Q309=+0

;PGM STOP TOLERANCE ~

Q330=+0

;TOOL