Cycle 420 MEASURE ANGLE (#17 / #1-05-1)
ISO programming
G420
Application
Related topics
- Cycle 1410 PROBING ON EDGE
Cycle run
- The control positions the touch probe to the pre-position of the first touch point 1, using positioning logic.
- Next, the touch probe moves to the entered measuring height and probes the first touch point at the probing feed rate (F column).
- The touch probe then moves to the next touch point 2 and probes again.
- The control returns the touch probe to the clearance height and saves the measured angle in the following Q parameter:
Q parameter | Meaning |
---|---|
Q150 | The measured angle is referenced to the main axis of the working plane. |
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- If touch probe axis = measuring axis, you can measure the angle in the direction of the A axis or B axis:
- If you want to measure the angle in the direction of the A axis, set Q263 equal to Q265 and Q264 unequal to Q266.
- If you want to measure the angle in the direction of the B axis, set Q263 not equal to Q265 and Q264 equal to Q266.
- 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 |
---|---|
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 | |
Q265 2nd measuring point in 1st axis? Coordinate of the second touch point in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q266 2nd measuring point in 2nd axis? Coordinate of the second touch point in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
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 | |
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 measuring point and ball tip. The touch probe movement will start with an offset of the sum of Q320, SET_UP, and the ball-tip radius, even when probing in the tool axis direction. 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 | |
Q281 Measuring log (0/1/2)? Define whether the control will create a measuring log: 1: Create a measuring log: The control will save the log file named TCHPR420.TXT in the folder that also contains the associated NC program. 2: Interrupt program run and display the measuring log on the control screen (you can later resume the NC program run with NC Start) Input: 0, 1, 2 |
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 420 MEASURE ANGLE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|