Cycle 1278 OCM POLYGON (#167 / #1-02-1)

ISO programming

G1278

Application

Use figure cycle 1278 OCM POLYGON to program a polygon. You can use the figure to machine a pocket, an island, or a boundary by face milling. In addition, you can program a tolerance for the reference diameter.

If you work with Cycle 1278, program the following:

  • Cycle 1278 OCM POLYGON
    • 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 1278 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 1278 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

Q573 Inscr.circle/circumcircle (0/1)?

Define whether the dimension Q571 is referenced to the inscribed circle or the circumcircle:

0: Dimension is referenced to the inscribed circle

1: Dimension is referenced to the circumcircle

Input: 0, 1

Q571 Reference circle diameter?

Enter the diameter of the reference circle. Specify in parameter Q573 whether the diameter entered here is referenced to the inscribed circle or the circumcircle. You can program a tolerance if needed.

Tolerances

Input: 0...99999.9999

Q572 Number of corners?

Enter the number of corners of the polygon. The control will always distribute the corners evenly on the polygon.

Input: 3...30

Q660 Type of corners?

Geometry of the corners:

0: Radius

1: Chamfer

Input: 0, 1

Q220 Corner radius?

Radius or chamfer of the corner of the figure

Input: 0...99999.9999

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.

 
Tip

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.

Example

11 CYCL DEF 1278 OCM POLYGON ~

Q650=+0

;FIGURE TYPE ~

Q573=+0

;REFERENCE CIRCLE ~

Q571=+50

;REF-CIRCLE DIAMETER ~

Q572=+6

;NUMBER OF CORNERS ~

Q660=+0

;CORNER TYPE ~

Q220=+0

;CORNER RADIUS ~

Q224=+0

;ANGLE OF ROTATION ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-10

;DEPTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+50

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR