Cycle 274 OCM FINISHING SIDE (#167 / #1-02-1)

ISO programming

G274

Application

With Cycle 274 OCM FINISHING SIDE, you can program finishing with the side finishing allowance programmed in Cycle 271. You can run this cycle in climb or up-cut milling.

Cycle 274 can also be used for contour milling.

Proceed as follows:

  1. Define the contour to be milled as a single island (without pocket boundary)
  2. Enter the finishing allowance (Q368) in Cycle 271 to be greater than the sum of the finishing allowance Q14 + radius of the tool being used

Requirements

Before programming the call of Cycle 274, you need to program further cycles:

  • CONTOUR DEF / SEL CONTOUR, alternatively Cycle 14 CONTOUR
  • Cycle 271 OCM CONTOUR DATA
  • Cycle 272 OCM ROUGHING, if applicable
  • Cycle 273 OCM FINISHING FLOOR, if applicable

Cycle run

  1. The tool uses positioning logic to move to the starting point
  2. The control positions the tool above the workpiece surface to the starting point for the approach position. This position in the plane results from a tangential arc on which the control moves the tool when approaching the contour
  3. Positioning logic in OCM cycles

  4. The control then moves the tool to the first plunging depth using the feed rate for plunging
  5. The tool approaches and moves along the contour helically on a tangential arc until the entire contour is finished. Each subcontour is finished separately
  6. Finally, the tool moves with Q253 F PRE-POSITIONING to Q200 SET-UP CLEARANCE and then at FMAX to Q260 CLEARANCE HEIGHT

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The control automatically calculates the starting point for finishing. The starting point depends on the available space in the contour and the allowance programmed in Cycle 271.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.
  • The cycle considers the miscellaneous functions M109 and M110. During the inside and outside machining of circular arcs the control keeps the feed rate constant at the cutting edge for inside and outside radii.
  • Adapting the feed rate for circular paths with M109

Note on programming

  • The finishing allowance for the side Q14 is left over after finishing. It must be smaller than the allowance in Cycle 271.

Cycle parameters

Help graphic

Parameter

Q338 Infeed for finishing?

Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect.

0: Finishing in one infeed

Input: 0...99999.9999

Q385 Finishing feed rate?

Traversing speed of the tool in mm/min for side finishing

Input: 0...99999.999 or FAUTO, FU, FZ

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min for approaching the starting position. This feed rate will be used below the coordinate surface, but outside the defined material.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q200 Set-up clearance?

Distance between lower edge of tool and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q14 Finishing allowance for side?

The finishing allowance for the side Q14 is left over after finishing. This allowance must be smaller than the allowance in Cycle 271. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q438 or QS438 Number/name of rough-out tool?

Number or name of the tool that was used by the control to rough out the contour pocket. You can transfer the coarse roughing tool directly from the tool table via the action bar. In addition, you can enter the tool name via the Name in the action bar. The control automatically inserts the closing quotation mark when you exit the input field.

-1: The control assumes that the tool last used is the rough-out tool (default behavior).

Input: –1...+32767.9 or max. 255 characters

Q351 Direction? Climb=+1, Up-cut=-1

Type of milling operation. The direction of spindle rotation is taken into account.

+1 = climb milling

–1 = up-cut milling

PREDEF: The control uses the value of a GLOBAL DEF block

(If you enter 0, climb milling is performed)

Input: -1, 0, +1 or PREDEF

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 274 OCM FINISHING SIDE ~

Q338=+0

;INFEED FOR FINISHING ~

Q385=+500

;FINISHING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q351=+1

;CLIMB OR UP-CUT