OCM cycles

OCM cycles

General information

 
Machine

Refer to your machine manual.

Your machine manufacturer enables this function.

Using OCM cycles (Optimized Contour Milling), you can combine subcontours to form complex contours. These cycles provide more functionality than Cycles 22 to 24. The OCM cycles feature the following additional functions:

  • When roughing, the control will maintain the specified tool angle precisely
  • Besides pockets, you can also machine islands and open pockets
 
Tip
  • Programming and operating notes:
  • You can program up to 16 384 contour elements in one OCM cycle.
  • 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 of finding out whether the program calculated by the control will provide the desired results.

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°.

Contour

Specify the contour with CONTOUR DEF / SEL CONTOUR or with the OCM shape 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.

Proceed as follows:

  1. Program CONTOUR DEF
  2. Define the first contour as a pocket and the second one as an island
  3. Define Cycle 271 OCM CONTOUR DATA
  4. Program cycle parameter Q569 = 1
  5. The control will interpret the first contour as an open boundary instead of a pocket. Thus, the open boundary and the island programmed subsequently are combined to form an open pocket.
  6. Define Cycle 272 OCM ROUGHING
 
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.

OCM figure cycles:

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

Proceed as follows:

  1. Program a figure using cycles 127x
  2. If the first figure will be an island or an open pocket, make sure to program boundary cycle 128x.
  3. Define Cycle 272 OCM ROUGHING

OCM cycles for pattern definition

Program structure: Machining with OCM cycles

0 BEGIN OCM MM

...

12 CONTOUR DEF

...

13 CYCL DEF 271 OCM CONTOUR DATA

...

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

...

50 L Z+250 R0 FMAX M2

51 LBL 1

...

55 LBL 0

56 LBL 2

...

60 LBL 0

...

99 END PGM OCM MM

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
Innenecke_Tasche
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 takes into account 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

Chamfering

  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

Positioning logic in OCM cycles

  1. The current tool position is above the clearance height:
  2. The control moves the tool to the starting point in the working plane at rapid traverse.
  3. At FMAX, the tool moves to Q260 CLEARANCE HEIGHT and then to Q200 SET-UP CLEARANCE
  4. The control then positions the tool to the starting point in the tool axis at Q253 F PRE-POSITIONING.
  1. The current tool position is below the clearance height:
  2. The control moves the tool to Q260 CLEARANCE HEIGHT at rapid traverse.
  3. At FMAX, the tool moves to the starting point in the working plane and then to Q200 SET-UP CLEARANCE
  4. The control then positions the tool to the starting point in the tool axis at Q253 F PRE-POSITIONING
 
Tip
  • Programming and operating notes:
  • The control takes Q260 CLEARANCE HEIGHT from Cycle 271 OCM CONTOUR DATA or from the figure cycles.
  • Q260 CLEARANCE HEIGHT is effective only if the clearance height position is above the set-up clearance.