Cylinder surface machining with CYLINDER SURFACE (#8 / #1-01-1)

Application

The CYLINDER SURFACE NC function allows you to machine the cylinder surface with various NC functions, for example OCM cycles (#167 / #1-02-1), pocket milling cycles or path functions.

Requirements

  • Machine with at least one rotary table axis
  • Rotary table axis as modulo axis

  • Software option Adv. Function Set 1 (#8 / #1-01-1)
  • The cylinder is set up centered and perpendicular on the rotary table
  • Workpiece preset in the center and on the surface of the cylinder

  • Milling operation FUNCTION MODE MILL
  • PARAX COMP DISPLAY NC function programmed with at least the main axes X, Y and Z
  • HEIDENHAIN recommends defining all of the available axes within the PARAX COMP DISPLAY function.

  • Tool call with tool axis Z
  • No active coordinate transformation such as TRANS ROTATION
  • Working plane for cylinder surface machining:
    • Cylinder axis parallel to a machine axis
    • Tool axis parallel to a machine axis and perpendicular above the cylinder axis
  •  
    Tip

    Machines with axes installed at a right angle or at 45 degrees meet these conditions after tilting the working plane, if required.

    Different kinematics possibly do not allow you to meet these conditions.

Description of function

Use the NC function CYLINDER SURFACE ON to activate cylinder surface machining. When the NC function CYLINDER SURFACE is active, the control displays an icon in the Positions workspace. This icon covers the icon for the PARAX COMP DISPLAY NC function.

The control deactivates cylinder surface machining in the following cases:

  • CYLINDER SURFACE OFF
  • M2 or M30
  • End of program END PGM
  • Cancellation of an NC program

You program the contour or machining cycles on the unrolled surface of the cylinder. The control transfers the programmed values to the cylinder surface. The control automatically calculates the feed rate of the rotary table axis based on the programmed feed rate and the cylinder diameter.

Use the X and Y coordinates to program the contour or machining cycles, independent of which rotary axes exist on your machine. The X coordinate describes the circumference of the cylinder and defines the position of the rotary table axis. The Y coordinate is on the cylinder axis. The Z axis serves as infeed axis.

The following table shows a possible sequence for cylinder surface machining:

Description

Help graphic

The workpiece preset is in the center and on the surface of the cylinder.

You tilt the working plane to the spatial angle SPB-90 and position the tool in the Y axis on the value 0. The working plane is tilted to the spatial angle SPB-90.

The tool is thus oriented perpendicularly above the cylinder axis. Due to the tilted working plane, the cylinder axis and the tool axis are each parallel to a machine axis.

You activate the NC function CYLINDER SURFACE.

The control automatically shifts the workpiece datum in the direction of the tool axis on the cylinder surface:

  • The X coordinate describes the circumference of the cylinder and defines the position of the rotary table axis
  • The Y coordinate is on the cylinder axis
  • The Z axis serves as infeed axis

You shift the workpiece datum in the direction Y-.

You program the contour on the unrolled surface of the cylinder.

The completed contour is transferred to the cylinder surface.

 
Tip

If the CYLINDER SURFACE NC function is active, the tool is positioned perpendicularly to the cylinder surface and as a result, the tool center is aligned with the cylinder center. If the X coordinate changes, the control moves the rotary table axis and not the tool.

This results in the following effects:

  • When using a contour definition with Y coordinates, the walls are not parallel to each other.
  • The bottom of a pocket, for example, can be uneven.
  • When you produce threads using thread milling cycles, the threads will be conical.
  • Only use tapping cycles for cylinder surface machining.

  • Tapping

If cylinder surface machining is active, do not use the following NC functions:

  • M91/M92
  • TOOL CALL
  • M140
  • M144 (#9 / #4-01-1)
  • POLARKIN
  • Tool radius compensation
  • 3D tool compensation (#9 / #4-01-1)
  • FUNCTION TCPM or M128 (#9 / #4-01-1)
  • Rotary axis movements
  • Tilting the working plane with PLANE functions
  • Switching the machining mode with FUNCTION MODE
  • Handwheel superimpositioning with M118 (#21 / #4-02-1)

Input

CYLINDER SURFACE ON

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.

11 CYLINDER SURFACE ON D99 X AS LIN

; Activate cylinder surface machining and define the cylinder size

To navigate to this function:

Insert NC function All functions Special functions Functions Cylinder kinematics CYLINDER SURFACE ON

The NC function includes the following syntax elements:

Syntax element

Meaning

CYLINDER SURFACE ON

Syntax initiator for activating cylinder surface machining

R or D

Radius or diameter of the cylinder

Number or numerical parameter

X AS

Axis of the unrolled surface of the cylinder

LIN or DEG

Indication of coordinates defining the unrolled surface of the cylinder as length or angle

DEG currently has no function

If DEG is selected, the control will display the error message Block format incorrect.

CYLINDER SURFACE OFF

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.

11 CYLINDER SURFACE OFF

; Deactivate cylinder surface machining

To navigate to this function:

Insert NC function All functions Special functions Functions Cylinder kinematics CYLINDER SURFACE OFF

The NC function includes the following syntax elements:

Syntax element

Meaning

CYLINDER SURFACE OFF

Syntax initiator for deactivating cylinder surface machining

Note

If a basic rotation around the cylinder axis is active, you always must tilt the working plane using, for example, PLANE SPATIAL SPA+0 SPB+0 SPC+0 before machining the cylinder surface.

Basic rotation and 3D basic rotation

Program structure for cylinder surface machining

Here you see a possible program structure for cylinder surface machining.

BLK FORM...

TOOL CALL...

If required, tilt the working plane

PLANE SPATIAL...

Pre-position above the cylinder axis

L X... Y+0 Z...

Activate cylinder surface machining

CYLINDER SURFACE ON...

Shift datum, if required

TRANS DATUM...

Machine cylinder surface

CYCL DEF 251 RECTANGULAR POCKET

; E.g., pocket milling cycle

CYCL CALL...

Reset datum shift

TRANS RESET

Deactivate cylinder surface machining

CYLINDER SURFACE OFF

If required, reset tilt angle and deactivate tilting of the working plane

PLANE RESET...

...

Example: Rectangular pocket with CYLINDER SURFACE

The following machining operations were already executed on the workpiece blank BLANK.STL:

  • Outside diameter as circular stud
  • Inside diameter as circular pocket
  • Chamfering at circular pocket and circular stud

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.

0 BEGIN PGM 1442806 MM

1 BLK FORM FILE "Blank.stl"

2 CALL LBL "RESET"

3 ;

4 * -

; Main program

5 FUNCTION PARAX COMP DISPLAY X Y Z

; Activate FUNCTION PARAX COMP DISPLAY

6 TOOL CALL "MILL_D10" Z S15000

7 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MB MAX FMAX

; Tilt the working plane

8 L X+0 Y+0 R0 FMAX M3

; Pre-position above the cylinder axis

9 ;

10 CYLINDER SURFACE ON D99 X AS LIN

; Activate cylinder surface machining

11 ;

12 TRANS DATUM AXIS Y-36

; Shift workpiece datum in direction Y-

13 CONTOUR DEF P1 = LBL "Pocket"

14 CYCL DEF 271 OCM CONTOUR DATA ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-10.5

;DEPTH ~

Q368=+0.2

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+10

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+0

;OPEN BOUNDARY

15 CYCL DEF 272 OCM ROUGHING ~

Q202=+10.5

;PLUNGING DEPTH ~

Q370=+0.608

;TOOL PATH OVERLAP ~

Q207=+5951

;FEED RATE MILLING ~

Q568=+0.6

;PLUNGING FACTOR ~

Q253=MAX

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=+0

;ROUGH-OUT TOOL ~

Q577=+0.2

;APPROACH RADIUS FACTOR ~

Q351=+1

;CLIMB OR UP-CUT ~

Q576=+15000

;SPINDLE SPEED ~

Q579=+1

;PLUNGING FACTOR S ~

Q575=+0

;INFEED STRATEGY

16 CYCL CALL

17 CYCL DEF 274 OCM FINISHING SIDE ~

Q338=+10.5

;INFEED FOR FINISHING ~

Q385=+2500

;FINISHING FEED RATE ~

Q253=MAX

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q351=+1

;CLIMB OR UP-CUT

18 CYCL CALL

19 TRANS RESET

; Reset datum shift

20 ;

21 CYLINDER SURFACE OFF

; Deactivate cylinder surface machining

22 ;

23 CALL LBL "RESET"

24 TOOL CALL "CHAMFERING_D10" Z S15000

25 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MB MAX FMAX

; Tilt the working plane

26 L X+0 Y+0 R0 FMAX M3

; Pre-position above the cylinder axis

27 ;

28 CYLINDER SURFACE ON D99 X AS LIN

; Activate cylinder surface machining

29 ;

30 TRANS DATUM AXIS Y-36

; Shift workpiece datum in direction Y-

31 CONTOUR DEF P1 = LBL "Pocket"

32 CYCL DEF 271 OCM CONTOUR DATA ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-10.5

;DEPTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+10

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+0

;OPEN BOUNDARY

33 CYCL DEF 277 OCM CHAMFERING ~

Q353=-2

;DEPTH OF TOOL TIP ~

Q359=+0.5

;CHAMFER WIDTH ~

Q207=+2000

;FEED RATE MILLING ~

Q253=MAX

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

QS438="MILL_D10"

;ROUGH-OUT TOOL ~

Q351=+1

;CLIMB OR UP-CUT ~

Q354=+0

;CHAMFER ANGLE ~

Q240=+1

;NUMBER OF CUTS

34 CYCL CALL

35 TRANS RESET

; Reset datum shift

36 ;

37 CYLINDER SURFACE OFF

; Deactivate cylinder surface machining

38 FUNCTION PARAX COMP OFF X Y Z

; Deactivate FUNCTION PARAX COMP

39 ;

40 CALL LBL "RESET"

41 M30

42 ;

43 * -

; Subprograms

44 LBL "Pocket"

45 L X+25 Y+31

46 L X+25 Y+5

47 L X-25 Y+5

48 L X-25 Y+31

49 L X+25 Y+31

50 LBL 0

51 ;

52 LBL "SAFE"

53 M140 MB+50

54 L Z+300 R0 FMAX M91

55 L X+400 Y-300 R0 FMAX M91

56 LBL 0

57 ;

58 LBL "RESET"

59 FUNCTION RESET TCPM

60 M140 MB+50

61 CALL LBL "SAFE"

62 TRANS DATUM RESET

63 PLANE RESET TURN FMAX

64 LBL 0

65 END PGM 1442806 MM

Definition

Modulo axis
Modulo axes are axes whose encoder only returns values between 0° and 359.9999°. If an axis is used as a spindle, then the machine manufacturer must configure this axis as a modulo axis.