ISO programming
G422
G422
Touch probe cycle 422 measures the center point and diameter of a circular stud. 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.
Q parameter | Meaning |
---|---|
Q151 | Actual value of center in reference axis |
Q152 | Actual value of center in minor axis |
Q153 | Actual value of diameter |
Q161 | Deviation at center of reference axis |
Q162 | Deviation at center of minor axis |
Q163 | Deviation from diameter |
Help graphic | Parameter |
---|---|
Q273 Center in 1st axis (nom. value)? Center of the stud 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)? Center of the stud 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 stud. 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 machining direction (negative = clockwise). 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)? Specify how the touch probe moves between measuring points: 0: Move at measuring height between measuring points 1: Move at clearance height between measuring points Input: 0, 1 | |
Q277 Maximum limit of size for stud? Maximum permissible diameter for the stud. Input: 0...99999.9999 | |
Q278 Minimum limit of size for stud? Minimum permissible diameter for the stud. 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 TCHPR422.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: Tool number in tool table TOOL.T Input: 0...99999.9 or max. 255 characters | |
Q423 No. probe points in plane (4/3)? 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 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 | |
Q498 Reverse tool (0=no/1=yes)? Only relevant if you have entered a turning tool in parameter Q330 before. For proper monitoring of the turning tool, the control requires the exact machining situation. Therefore, enter the following: 1: Turning tool is mirrored (rotated by 180°) by, for example, Cycle 800 and parameter Reverse the tool Q498 = 1 0: Turning tool corresponds to the description in the turning tool table (toolturn.trn); no modification by, for example , Cycle 800 and parameter Reverse the tool Q498 = 0 Input: 0, 1 | |
Q531 Angle of incidence? Only relevant if you have entered a turning tool in parameter Q330 before. Enter the angle of incidence (inclination angle) between turning tool and workpiece during machining (e.g., from Cycle 800, Angle of incidence? Q531). Input: -180...+180 |
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.
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 422 MEAS. CIRCLE OUTSIDE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|