ISO programming
G427
G427
Touch probe cycle 427 measures a coordinate in a selectable axis and saves the value in a Q parameter. 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 |
---|---|
Q160 | Measured coordinate |
Help graphic | Parameter |
---|---|
Q263 1st measuring point in 1st axis? Coordinate of the first touch point in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q264 1st measuring point in 2nd axis? Coordinate of the first touch point 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 | |
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 | |
Q272 Meas. axis (1/2/3, 1=ref. axis)? Axis in which the measurement will be made: 1: Main axis = measuring axis 2: Secondary axis = measuring axis 3: Touch probe axis = measuring axis Input: 1, 2, 3 | |
Q267 Trav. direction 1 (+1=+ / -1=-)? Direction in which the touch probe will approach the workpiece: –1: Negative traverse direction +1: Positive traverse direction Input: –1, +1 | |
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 | |
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 TCHPR427.TXT in the folder that also contains the associated NC program. 2: Interrupt the program run and display the measuring log on the control screen.Resume the NC program run with NC Start. Input: 0, 1, 2 | |
Q288 Maximum limit of size? Maximum permissible value Input: –99999.9999...+99999.9999 | |
Q289 Minimum limit of size? Minimum permissible value Input: –99999.9999...+99999.9999 | |
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 | |
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 427 MEASURE COORDINATE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|