Blank form update in turning mode with FUNCTION TURNDATA BLANK (option 50)

Application

Using the blank form update feature, the control detects the already machined areas and adapts all approach and departure paths to the specific, current machining situation. Thus, air cuts are avoided and the machining time is significantly reduced.

You define the workpiece blank for blank form update in a subprogram or separate NC program.

640_turn_006

Requirements

  • Combined milling/turning (software option 50)
  • FUNCTION MODE TURN must be active
  • Blank form update is only possible with cycle machining in turning mode.

  • Closed blank contour for blank form updating
  • The starting and end positions must be identical. The workpiece blank corresponds to the cross-section of a rotationally symmetrical body.

Description of function

640_turn_005

With TURNDATA BLANK you call a contour description used by the control as an updated workpiece blank.

You can define the workpiece blank in a subprogram within the NC program or as a separate NC program.

Blank form update is only active in conjunction with roughing cycles. In finishing cycles the control always machines the entire contour, for example so that the contour does not have any offset.

Cycles for milling and turning

  • There are various ways for selecting files or subprograms:
  • Enter the file path
  • Enter the number or name of the subprogram
  • Select the file or subprogram by means of a selection window
  • Define the file path or name of the subprogram in a QS parameter
  • Define the number of the subprogram in a Q, QL or QR parameter

Use FUNCTION TURNDATA BLANK OFF to deactivate blank form update.

Input

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.

1 FUNCTION TURNDATA BLANK LBL "BLANK"

; Blank form update with a workpiece blank from the subprogram "BLANK"

* - ...

11 LBL "BLANK"

; Subprogram start

12 L X+0 Z+0

; Beginning of contour

13 L X+50

; Coordinates in positive direction of main axis

14 L Z+50

15 L X+30

16 L Z+70

17 L X+0

18 L Z+0

; End of contour

19 LBL 0

; End of subprogram

The NC function includes the following syntax elements:

Syntax element

Meaning

FUNCTION TURNDATA BLANK

Syntax initiator for blank form update in turning mode

OFF, File, QS or LBL

Deactivate blank form update, blank contour as separate NC program, or call as subprogram

Number, Name or QS

Number or name of the separate NC programor subprogram

Fixed or variable number or name

If File, QS or LBL is selected