Cycle 1274 OCM CIRCULAR SLOT (#167 / #1-02-1)

ISO programming

G1274

Application

Use figure cycle 1274 OCM CIRCULAR SLOT to program a circular slot. Optionally, you can program a tolerance for the slot width.

When using Cycle 1274, program the cycles in the following sequence:

  • Cycle 1274 OCM CIRCULAR SLOT
  • 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 1274 is DEF-active, which means that Cycle 1274 becomes active as soon as it has been defined in the NC program.
  • The machining data defined in Cycle 1274 are valid for the OCM machining cycles 272 to 274 and 277.

Notes on programming

  • This cycle requires pre-positioning, which depends on the setting in parameter Q367 REF. SLOT POSITION.
  • Make sure to define the angle between the starting point and the end point Q248 in such a way that the contour does not intersect itself. Otherwise, the control will display an error message.

Cycle parameters

Help graphic

Parameter

Q219 Width of slot?

Slot width

This value has an incremental effect. You can program a tolerance if needed.

Tolerances

Input: 0...99999.9999

Q375 Pitch circle diameter?

The pitch circle diameter is the center line path of the slot.

Input: 0...99999.9999

Q376 Starting angle?

Polar angle of starting point

This value has an absolute effect.

Input: –360.000...+360.000

Q248 Angular length?

The opening angle is the angle between the starting point and the end point of the circular slot. This value has an incremental effect.

Input: 0...360

Q378 Intermediate stepping angle?

Angle between two machining positions

The center of rotation is at the center of the slot. This parameter is effective when the number of machining operations is Q377>=2. This value has an incremental effect.

Input: –360.000...+360.000

Q377 Number of repetitions?

Number of machining operations on a pitch circle

Input: 1...99999

Q367 Ref. for slot pos. (0/1/2/3)?

Position of the figure relative to the position of the tool during the cycle call:

0: Tool position = center of the pitch circle

1: Tool position = center of the left figure arc

2: Tool position = figure center on center line

3: Tool position = center of the right figure arc

Input: 0, 1, 2, 3

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 1274 OCM CIRCULAR SLOT ~

Q219=+10

;SLOT WIDTH ~

Q375=+60

;PITCH CIRCLE DIAMETR ~

Q376=+0

;STARTING ANGLE ~

Q248=+60

;ANGULAR LENGTH ~

Q378=+90

;STEPPING ANGLE ~

Q377=+4

;NR OF REPETITIONS ~

Q367=+0

;REF. SLOT POSITION ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-20

;DEPTH ~

Q368=+0.1

;ALLOWANCE FOR SIDE ~

Q369=+0.1

;ALLOWANCE FOR FLOOR ~

Q260=+100

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR