Blank form update in turning with FUNCTION TURNDATA BLANK (#50 / #4-03-1)
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.
Related topics
- Subprograms
- Turning mode: FUNCTION MODE TURN
- Defining a workpiece blank with BLK FORM for simulation
Requirements
- Software option Turning (#50 / #4-03-1)
- 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
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.
If the contour to be machined is larger than the workpiece blank, the control will display an error message.
Mill-turning cycles (#50 / #4-03-1)
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 string parameter
- Define the number of the subprogram in a numerical 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.
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 |
To navigate to this function:
Insert NC function All functions Special functions Turning functions Basic functions FUNCTION TURNDATA BLANK
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 Parameter | Number or name of the separate NC programor subprogram Number, text, or variable Selection by means of a selection window When File, QS, or LBL is selected |