Cycle 271 OCM CONTOUR DATA (#167 / #1-02-1)
ISO programming
G271
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- Cycle 271 is DEF-active, which means that it becomes active as soon as it is defined in the NC program.
- The machining data entered in Cycle 271 are valid for Cycles 272 to 274.
Cycle parameters
Help graphic | Parameter |
---|---|
Q203 Workpiece surface coordinate? Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect. Input: –99999.9999...+99999.9999 | |
Q201 Depth? Distance between the workpiece surface and the contour floor. This value has an incremental effect. Input: –99999.9999...+0 | |
Q368 Finishing allowance for side? Finishing allowance in the machining plane which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q369 Finishing allowance for floor? Finishing allowance in depth which remains after roughing. This value has an incremental effect. Input: 0...99999.9999 | |
Q260 Clearance height? Position in the tool axis at which no collision can occur with the workpiece. The control approaches this position for intermediate positions and when retracting at the end of the cycle. This value has an absolute effect. Input: –99999.9999...+99999.9999 or PREDEF | |
Q578 Radius factor on inside corners? The tool radius multiplied with Q578 INSIDE CORNER FACTOR results in the smallest tool center point path. This prevents smaller inside radii at the contour, as resulting from the tool radius plus the product of tool radius and Q578 INSIDE CORNER FACTOR. Input: 0.05...0.99 | |
Q569 Is the first pocket a boundary? Define the boundary: 0: The first contour in CONTOUR DEF is interpreted as a pocket. 1: The first contour in CONTOUR DEF is interpreted as an open boundary. The following contour must be an island 2: The first contour in CONTOUR DEF is interpreted as a "bounding block." The following contour must be a pocket 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 CYCL DEF 271 OCM CONTOUR DATA ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
|