Cycle 271 OCM CONTOUR DATA (option 167)

ISO programming

G271

Application

Use Cycle 271 OCM CONTOUR DATA to program machining data for the contour or the subprograms describing the subcontours. In addition, Cycle 271 enables you to define an open boundary for a pocket.

Notes

  • This cycle can only be executed 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

cyc271_1

cyc271_2

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 working plane. This value has an incremental effect.

Input: 0...99999.9999

Q369 Finishing allowance for floor?

Finishing allowance for the floor. This value has an incremental effect.

Input: 0...99999.9999

Q260 Clearance height?

Coordinate in the tool axis in which no collision with the workpiece can occur (for intermediary positioning and retraction 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 inside radii of the contour are calculated based on the tool radius plus the product of the tool radius times Q578.

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.

 
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 271 OCM CONTOUR DATA ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-20

;DEPTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+100

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+0

;OPEN BOUNDARY