Cycle 1273 OCM SLOT / RIDGE (#167 / #1-02-1)
ISO programming
G1273
Application
Use figure cycle 1273 OCM SLOT / RIDGE to program a slot or a ridge. This figure cycle also allows you to program a boundary for face milling. In addition, you can program a tolerance for the width and the length.
If you work with Cycle 1273, program the following:
- Cycle 1273 OCM SLOT / RIDGE
- If you program an island (Q650=1), you need to define a boundary using Cycle 1281 OCM RECTANGLE BOUNDARY or 1282 OCM CIRCLE BOUNDARY. You define the boundary after the shape cycle.
- If necessary, Cycle 1281 OCM RECTANGLE BOUNDARY oder 1282 OCM CIRCLE BOUNDARY
- Cycle 272 OCM ROUGHING
- Cycle 273 OCM FINISHING FLOOR, if applicable
- Cycle 274 OCM FINISHING SIDE, if applicable
- Cycle 277 OCM CHAMFERING, if applicable
Notes
- This cycle can be executed only in the FUNCTION MODE MILL machining mode.
- Cycle 1273 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 1273 are valid for the OCM machining cycles 272 to 274 and 277.
Note on programming
- The cycle requires corresponding pre-positioning, depending on the setting in Q367.
- If you have roughed a figure or a contour before, program the number or the name of the rough-out tool in the cycle. If there was no initial roughing, you need to define Q438=0 ROUGH-OUT TOOL in the cycle parameter during the first roughing operation.
Cycle parameters
Help graphic | Parameter |
---|---|
Q650 Type of figure? Geometry of the figure: 0: Pocket 1: Island 2: Boundary for face milling Input: 0, 1, 2 | |
Q219 Width of slot? Width of the slot or ridge, parallel to the secondary axis of the working plane. This value has an incremental effect. You can program a tolerance if needed. Input: 0...99999.9999 | |
Q218 Length of slot? Length of the slot or ridge, parallel to the main axis of the working plane. This value has an incremental effect. You can program a tolerance if needed. Input: 0...99999.9999 | |
Q367 Position of slot (0/1/2/3/4)? Position of the figure relative to the position of the tool when the cycle is called: 0: Tool position = Center of figure 1: Tool position = Left end of figure 2: Tool position = Center of left figure arc 3: Tool position = Center of right figure arc 4: Tool position = Right end of figure Input: 0, 1, 2, 3, 4 | |
Q224 Angle of rotation? Angle by which the figure is rotated. The center of rotation is at the center of the figure. This value has an absolute effect. Input: –360.000...+360.000 | |
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 |
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 1273 OCM SLOT / RIDGE ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|