Cycle 430 MEAS. BOLT HOLE CIRC (#17 / #1-05-1)
ISO programming
G430
Application
Cycle run
- The control positions the touch probe at the entered center of the first hole 1, using positioning logic.
- Then the probe moves to the entered measuring height and probes four points to determine the first hole center point.
- The touch probe returns to the clearance height and then to the position entered as center of the second hole 2.
- The control moves the touch probe to the entered measuring height and probes four points to determine the second hole center point.
- The touch probe returns to the clearance height and then to the position entered as center of the third hole 3.
- The control moves the touch probe to the entered measuring height and probes four points to determine the third hole center point.
- 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 | 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 |
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.
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.
11 TCH PROBE 430 MEAS. BOLT HOLE CIRC ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|