Cycle 277 OCM CHAMFERING (#167 / #1-02-1)

ISO programming

G277

Application

Cycle 277 OCM CHAMFERING enables you to deburr edges of complex contours that you roughed out using OCM cycles.

This cycle considers adjacent contours and boundaries that you called before with Cycle 271 OCM CONTOUR DATA or the 12xx standard geometric elements.

Requirements

Before the control can execute Cycle 277, you need to create the tool in the tool table using appropriate parameters:

  • L + DL: Overall length up to the theoretical tip
  • R + DR: Definition of the overall tool radius
  • T-ANGLE: Point angle of the tool

In addition, you need to program other cycles before programming the call of Cycle 277:

  • CONTOUR DEF / SEL CONTOUR, alternatively Cycle 14 CONTOUR
  • Cycle 271 OCM CONTOUR DATA or the 12xx standard geometric elements
  • Cycle 272 OCM ROUGHING, if applicable
  • Cycle 273 OCM FINISHING FLOOR, if applicable
  • Cycle 274 OCM FINISHING SIDE, if applicable

Cycle run

  1. The tool uses positioning logic to move to the starting point. This point is determined automatically based on the programmed contour.
  2. In the next step, the tool moves at FMAX to set-up clearance Q200.
  3. Then, the tool plunges vertically to Q353 DEPTH OF TOOL TIP.
  4. The tool approaches the contour in a tangential or vertical movement (depending on the available space).
  5. Depending on the definition in Q240 NUMBER OF CUTS, the tool approaches the first stepover or the entire chamfer width.
  6. For machining the chamfer, the tool uses the milling feed rate Q207.
  7. Then, the tool is retracted from the contour in a tangential or vertical movement (depending on the available space).
  8. If there are several contours, all of them will be machined. The tool is positioned at clearance height after each contour and then moves to the next starting point.
  9. Depending on the definition in Q240, the tool approaches the workpiece laterally; steps 5 to 8 are repeated until the entire programmed contour has been chamfered.
  10. Then, the tool moves at Q253 F PRE-POSITIONING to Q200 SET-UP CLEARANCE and then at FMAX to Q260 CLEARANCE HEIGHT.

Positioning logic in OCM cycles

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The control automatically calculates the starting point for chamfering. The starting point depends on the available space.
  • The control monitors the tool radius. Adjacent walls machined with Cycle 271 OCM CONTOUR DATA or with the 12xx figure cycles will remain intact.
  • The cycle monitors for damage to the contour floor from the tool tip. This tool tip results from the radius R, the radius of the tool tip R_TIP, and the point angle T-ANGLE.
  • Keep in mind that the active tool radius of the chamfering tool must be smaller than or equal to the radius of the rough-out tool. Otherwise, the control might not be able to completely chamfer all edges. The effective tool radius is the radius of the cutting length of the tool. This tool radius results from T-ANGLE and R_TIP from the tool table.
  • 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

  • If the roughing operations have not completely removed the material before chamfering, you need to define the last roughing tool in QS438 ROUGH-OUT TOOL, in order to prevent damage to the contour.
  • Procedure regarding residual material in inside corners

Note on programming

  • If the value of parameter Q353 DEPTH OF TOOL TIP is less than the value of parameter Q359 CHAMFER WIDTH, the control will display an error message.

Cycle parameters

Help graphic

Parameter

Q353 Depth of tool tip?

Distance between theoretical tool tip and workpiece surface coordinate. This value has an incremental effect.

Input: –999.9999...–0.0001

Q359 Width of chamfer (-/+)?

Width or depth of chamfer:

-: Depth of chamfer

+: Width of chamfer

This value has an incremental effect.

Input: –999.9999...+999.9999

Q207 Feed rate for milling?

Traversing speed of the tool in mm/min for milling

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

Q253 Feed rate for pre-positioning?

Traversing speed of the tool in mm/min for positioning

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

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

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

Q354 Angle of chamfer?

Angle of the chamfer

0: The chamfer angle is half the defined T-ANGLE from the tool table

> 0: The chamfer angle is compared to the value of T-ANGLE from the tool table. If these two values do not match, the control will display an error message.

Input: 0...89

Q240 Number of cuts? (optional)

Number of infeeds until the chamfer size is attained

The control retains the same depth for all infeeds and shifts the tool only laterally. The control divides the cuts in such a way that a constant chip cross section results over all infeeds.

1: Machining in one infeed

2-99: Machining in several infeeds

Input: 1...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 277 OCM CHAMFERING ~

Q353=-1

;DEPTH OF TOOL TIP ~

Q359=+0.2

;CHAMFER WIDTH ~

Q207=+500

;FEED RATE MILLING ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q351=+1

;CLIMB OR UP-CUT ~

Q354=+0

;CHAMFER ANGLE ~

Q240=+1

;NUMBER OF CUTS