Programming instructions

NC Programming 17VRS Tool Corrections
5-39
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Tool Length Correction, Cancel 'G47'
The function G47 is used to cancel an already active tool length correc-
tion. When movements are being performed in the direction of the tool, all
position data relates to the position of spindle nose.
If an active tool length correction (G48 or G49) is canceled with G47, a
programmed move in the direction of the existing main axes is expected.
Moves which do not involve the removal of material from the workpiece, a
tool change for example, are generally performed without tool length cor-
rection.
•
Depending on the settings in the process parameter Bxx.038, G47
may be the power-on default, G47 remains modally active until it is
canceled by G48 or G49.
•
After the controller is turned on, after an NC-program is loaded, after a
BST, RET, M02, M30, or Control Reset, G47 is set automatically de-
pending on the setting in the process parameter Bxx.038.
Tool Length Correction, Positive 'G48'
After tool length correction has been activated by a G48, the CNC com-
pensates the tool lengths entered in the magazine list in the positive axis
direction beginning with the next programmed move in the direction of the
existing main axes.
•
Depending on the settings in the process parameter Bxx.038, G48
may be the power-on default. G48 remains modally active until it is
canceled by G47 or G49.
•
After the controller is turned on, after an NC-program is loaded, after a
BST, RET, M02, M30, or Control Reset, G48 is set automatically de-
pending on the setting in the process parameter Bxx.038.
Tool Length Correction, Negative 'G49'
After tool length correction has been activated by a G49, the CNC com-
pensates the tool lengths entered in the magazine list in the negative axis
direction beginning with the next programmed move in the direction of the
existing main axes.
•
G49 remains modally active until it is canceled by G47 or G49, or until
it is automatically reset at the program end (RET) or by BST.
5.7 Read/Write Tool Data from the NC Program 'TLD'
The TLD command (tool data) can be used to read the tool data from the
NC-program and to write them, however some restrictions apply to writing.
TLD([0..6],[1],[1..9999999],[1...999],[0..9],[1..35],[1..32])
Status
Data Element
Edge
Location / Index no.
Storage [0..2] / tool number
Addressing
Process
TLD([0..6],[0], [0..2] ,[1...999],[0..9],[1..35],[1..32])
PA
S/T L/D E D S
Syntax