Cycle 1271 OCM RECTANGLE (#167 / #1-02-1)

ISO programming

G1271

Application

Use the figure cycle 1271 OCM RECTANGLE to program a rectangle. You can use the figure to machine a pocket, an island, or a boundary by face milling. In addition, you can program tolerances for the lengths.

If you work with Cycle 1271, program the following:

  • Cycle 1271 OCM RECTANGLE
    • 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, if required OCM FINISHING FLOOR
  • Cycle 274, if required OCM FINISHING SIDE
  • Cycle 277, if required OCM CHAMFERING

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • Cycle 1271 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 1271 are valid for the OCM machining cycles 272 to 274 and 277.

Notes 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

Q218 First side length?

Length of the first side of the figure, parallel to the main axis. This value has an incremental effect. You can program a tolerance if needed.

Tolerances

Input: 0...99999.9999

Q219 Second side length?

Length of the second side of the figure, parallel to the secondary axis. This value has an incremental effect. You can program a tolerance if needed.

Tolerances

Input: 0...99999.9999

Q660 Type of corners?

Geometry of the corners:

0: Radius

1: Chamfer

2: Milling corners in the main and secondary axis directions

3: Milling corners in the main axis direction

4: Milling corners in the secondary axis direction

Input: 0, 1, 2, 3, 4

Q220 Corner radius?

Radius or chamfer of the corner of the figure

Input: 0...99999.9999

Q367 Position of pocket (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 = Lower left corner

2: Tool position = Lower right corner

3: Tool position = Upper right corner

4: Tool position = Upper left corner

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.

 
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 1271 OCM RECTANGLE ~

Q650=+1

;FIGURE TYPE ~

Q218=+60

;FIRST SIDE LENGTH ~

Q219=+40

;2ND SIDE LENGTH ~

Q660=+0

;CORNER TYPE ~

Q220=+0

;CORNER RADIUS ~

Q367=+0

;POCKET POSITION ~

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