Fundamentals

Application

The OCM cycles include highly efficient roughing or finishing cycles that ease the load on the tool. Using OCM cycles, the control automatically calculates complex movements for milling pockets and islands. Besides pockets and islands, you can also machine open pockets. When roughing, the control will maintain the specified tool angle precisely.

During programming, you can apply the optimal machining parameters from the OCM cutting data calculator directly on the control. The OCM cutting data calculator benefits from an integrated, comprehensive material database. You can adapt the automatically calculated cutting values with regard to the mechanical and thermal load on the tool and transfer them to the roughing cycle.

In order to machine standard shapes, OCM offers various geometric shapes that can then be used as pockets, islands, or boundaries for face milling in conjunction with other OCM cycles.

 
Tip

The OCM cycles are more powerful than Cycles 22 to 24.

Related topics

Overview of the OCM cycles (#167 / #1-02-1)

Fixed cycles

Cycle

Call

Further information

271

OCM CONTOUR DATA

  • Definition of the machining information for the contour or subprograms
  • Input of a bounding frame or block

DEF-active

272

OCM ROUGHING

  • Technology data for roughing contours
  • Use of the OCM cutting data calculator
  • Plunging behavior: vertical, helical, or reciprocating
  • Plunging strategy: selectable

CALL-active

273

OCM FINISHING FLOOR

  • Finishing with finishing allowance for the floor from Cycle 271
  • Machining strategy with constant tool angle or with path calculated as equidistant (equal distances)

CALL-active

274

OCM FINISHING SIDE

  • Finishing with side finishing allowance from Cycle 271

CALL-active

277

OCM CHAMFERING

  • Deburr the edges
  • Consideration of adjacent contours and walls

CALL-active

OCM: Geometric figures

Cycle

Call

Further information

1271

OCM RECTANGLE

  • Definition of a rectangle
  • Input of the side lengths
  • Definition of the corners

DEF-active

1272

OCM CIRCLE

  • Definition of a circle
  • Input of the circle diameter

DEF-active

1273

OCM SLOT / RIDGE

  • Definition of a groove or ridge
  • Input of the width and the length

DEF-active

1274

OCM CIRCULAR SLOT

  • Definition of a circular slot
  • Input of the width, the pitch circle, and the number of repeats

DEF-active

1278

OCM POLYGON

  • Definition of a polygon
  • Input of the reference circle
  • Definition of the corners

DEF-active

1281

OCM RECTANGLE BOUNDARY

  • Definition of a bounding rectangle

DEF-active

1282

OCM CIRCLE BOUNDARY

  • Definition of a bounding circle

DEF-active

Requirements

  • Software option Opt. Contour Milling (#167 / #1-02-1)
  • Refer to your machine manual. Read and note the functional description of the machine manufacturer. Follow the safety precautions.
  • OCM cycles conduct comprehensive and complex internal calculations as well as the resulting machining operations. For safety reasons, always verify the program graphically! This is a simple way to find out whether the program calculated by the control will provide the desired results.

Description of function

Program structure

Program structure: Machining with OCM cycles

The table below shows an example of what a program run with the OCM cycles might look like.

0 BEGIN OCM MM

...

12 CONTOUR DEF; Define contour call or figure cycles

...

13 CYCL DEF 271 OCM CONTOUR DATA; Only required for contour definitions

...

16 CYCL DEF 272 OCM ROUGHING

...

17 CYCL CALL

...

20 CYCL DEF 273 OCM FINISHING FLOOR

...

21 CYCL CALL

...

24 CYCL DEF 274 OCM FINISHING SIDE

...

25 CYCL CALL

...

35 CYCL DEF 277 OCM CHAMFERING

36 CYCL CALL

...

50 L Z+250 R0 FMAX M2

51 LBL 1

...

55 LBL 0

56 LBL 2

...

60 LBL 0

...

99 END PGM OCM MM

Contour definition

OCM figure cycles

The figure defined in an OCM figure cycle can be a pocket, an island, or a boundary. Use Cycles 128x for programming an island or an open pocket.

OCM cycles for figure definition

 
Tip

With a figure, you can redefine the OCM contour data and cancel the definition of a previously defined Cycle 271 OCM CONTOUR DATA or of a figure boundary.

Contour formula

Specify the contour with CONTOUR DEF / SEL CONTOUR or with the OCM figure cycles 127x.

Closed pockets can also be defined in Cycle 14.

The machining dimensions, such as milling depth, allowances, and clearance height, can be entered centrally in Cycle 271 OCM CONTOUR DATA or in the 127x figure cycles.

CONTOUR DEF / SEL CONTOUR:

In CONTOUR DEF / SEL CONTOUR, the first contour can be a pocket or a boundary. The next contours can be programmed as islands or pockets. To program open pockets, use a boundary and an island.

 
Tip

Programming notes:

  • Subsequently defined contours that are outside the first contour will not be considered.
  • The first depth of the subcontour is the cycle depth. This is the maximum depth for the programmed contour. Other subcontours cannot be deeper than the cycle depth Therefore, start programming the subcontour with the deepest pocket.

Related topics

Contact angle

When roughing, the control will retain the tool angle precisely. The tool angle can be defined implicitly by specifying an overlap factor. The maximum overlap factor is 1.99; this corresponds to an angle of nearly 180°.

Positioning logic in OCM cycles

The current tool position is above the clearance height:

  1. The control moves the tool to the starting point in the working plane at rapid traverse.
  2. The tool moves at FMAX to Q260 CLEARANCE HEIGHT and then to Q200 SET-UP CLEARANCE
  3. The control then positions the tool to the starting point in the tool axis at Q253 F PRE-POSITIONING.

The current tool position is below the clearance height:

  1. The control moves the tool to Q260 CLEARANCE HEIGHT at rapid traverse.
  2. At FMAX, the tool moves to the starting point in the working plane and then to Q200 SET-UP CLEARANCE
  3. The control then positions the tool to the starting point in the tool axis at Q253 F PRE-POSITIONING
 
Tip

Programming and operating notes:

  • Q260 The control uses the CLEARANCE HEIGHT from Cycle 271 OCM CONTOUR DATA or from the figure cycles.
  • Q260 CLEARANCE HEIGHT is effective only when the position of the safe height is above the safety distance.

Removing residual material

When roughing, these cycles allow you to use larger tools for the first roughing passes and then smaller tools to remove the residual material. During finishing the control will take into account the material roughed out, thus preventing the finishing tool from being overloaded.

Example: Open pocket and fine roughing with OCM cycles

 
Tip
  • If residual material remains in the inside corners after roughing, then use a smaller rough-out tool or define an additional roughing operation with a smaller tool.
  • If the inside corners cannot be roughed out completely, the control may damage the contour during chamfering. In order to prevent damage to the contour, follow the procedure described below.

Procedure regarding residual material in inside corners

The example describes the inside machining of a contour by using several tools with radii greater than the programmed contour. Although the radius of the tools used becomes smaller, residual material remains in the inside corners after roughing. The control takes this residual material into account during the subsequent finishing and chamfering operations.

In the example, you use the following tools:

  • MILL_D20_ROUGH, Ø 20 mm
  • MILL_D10_ROUGH, Ø 10 mm
  • MILL_D6_FINISH, Ø 6 mm
  • NC_DEBURRING_D6, Ø 6 mm
Inside corner with a radius of 4 mm in this example

Roughing

  1. Rough the contour with the tool MILL_D20_ROUGH
  2. The control considers the Q parameter Q578 INSIDE CORNER FACTOR, resulting in inside radii of 12 mm during initial roughing.

...

12 TOOL CALL Z "MILL_D20_ROUGH"

...

15 CYCL DEF 271 OCM CONTOUR DATA

...

     Q578 = 0.2 ;INSIDE CORNER FACTOR

...

Resulting inside radius =

RT+ (Q578 * RT)

10 + (0.2 *10) = 12

16 CYCL DEF 272 OCM ROUGHING

...

  1. Then rough the contour with the smaller tool MILL_D10_ROUGH
  2. The control takes into account the Q parameter Q578 INSIDE CORNER FACTOR, resulting in inside radii of 6 mm during initial roughing.

...

20 TOOL CALL Z "MILL_D10_ROUGH"

...

22 CYCL DEF 271 OCM CONTOUR DATA

...

     Q578 = 0.2 ;INSIDE CORNER FACTOR     

...

Resulting inside radius =

RT+ (Q578 * RT)

5 + (0.2 *5) = 6

23 CYCL DEF 272 OCM ROUGHING

...

     Q438 = -1 ;ROUGH-OUT TOOL     

...

-1: The control assumes that the tool last used is the rough-out tool

Finishing

  1. Finish the contour with the tool MILL_D6_FINISH
  2. This finishing tool would allow inside radii of 3.6 mm. This means that the finishing tool would be capable of machining the defined inside radii of 4 mm. However, the control takes into account the residual material of the rough-out tool MILL_D10_ROUGH. The control machines the contour with the previous roughing tool's inside radii of 6 mm. Thus, the finishing cutter will be protected from overload.

...

27 TOOL CALL Z "MILL_D6_FINISH"

...

29 CYCL DEF 271 OCM CONTOUR DATA

...

     Q578 = 0.2 ;INSIDE CORNER FACTOR

...

Resulting inside radius =

RT+ (Q578 * RT)

3 + (0.2 *3) = 3.6

30 CYCL DEF 274 OCM FINISHING SIDE

...

     Q438 = -1 ;ROUGH-OUT TOOL

...

-1: The control assumes that the tool last used is the rough-out tool

  1. Chamfering the contour: When defining the cycle, you must define the last rough-out tool of the roughing operation.
  2.  
    Tip

    If you use the finishing tool as a roughing tool, the control will damage the contour. In this case, the control assumes that the finishing cutter machined the contour with inside radii of 3.6 mm. However, the finishing cutter has limited the inside radii to 6 mm based on the previous roughing operation.

...

33 TOOL CALL Z "NC_DEBURRING_D6"

...

35 CYCL DEF 277 OCM CHAMFERING

...

     QS438 = "MILL_D10_ROUGH" ;ROUGH-OUT TOOL

...

Rough-out tool of the last roughing operation