Cycle 431 MEASURE PLANE (#17 / #1-05-1)
ISO programming
G431
Application
Related topics
- Cycle 1420 PROBING IN PLANE
Cycle run
- The control positions the touch probe to the programmed touch point 1, using positioning logic and measures the first plane point there. The control offsets the touch probe by the set-up clearance in the direction opposite to the direction of probing.
- The touch probe returns to the clearance height and then moves in the working plane to touch point 2 and measures the actual value of the second touch point in the plane.
- The touch probe returns to the clearance height and then moves in the working plane to touch point 3 and measures the actual value of the third touch point in the plane.
- Finally the control returns the touch probe to the clearance height and saves the measured angle values in the following Q parameters:
Q parameter | Meaning |
---|---|
Q158 | Projection angle of the A axis |
Q159 | Projection angle of the B axis |
Q170 | Spatial angle A |
Q171 | Spatial angle B |
Q172 | Spatial angle C |
Q173 to Q175 | Measured values in the touch probe axis (first to third measurement) |
Notes
- Make sure to program SYM (SEQ) + or SYM (SEQ) -
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- The control can calculate the angle values only if the three measuring points are not positioned on a straight line.
- The control will reset an active basic rotation at the beginning of the cycle.
Notes on programming
- Before defining this cycle, you must have programmed a tool call to define the touch probe axis.
- The spatial angles that are needed for the Tilt working plane function are saved in parameters Q170 to Q172. With the first two measuring points, you also specify the direction of the main axis when tilting the working plane.
- The third measuring point determines the direction of the tool axis. Define the third measuring point in the direction of the positive Y axis to ensure that the position of the tool axis in a clockwise coordinate system is correct.
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 | |
Q294 1st measuring point in 3rd axis? Coordinate of the first touch point in the touch probe axis. 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 | |
Q295 2nd measuring point in 3rd axis? Coordinate of the second touch point in the touch probe axis. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q296 3rd measuring point in 1st axis? Coordinate of the third touch point in the main axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q297 3rd measuring point in 2nd axis? Coordinate of the third touch point in the secondary axis of the working plane. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q298 3rd measuring point in 3rd axis? Coordinate of the third touch point in the touch probe axis. 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 | |
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 TCHPR431.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 |
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 431 MEASURE PLANE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|