With the T NC function, you call a tool in the NC program.
T corresponds to the TOOL CALL Klartext syntax.
With G17, G18, and G19, you define the tool axis.
With the T NC function, you call a tool in the NC program.
T corresponds to the TOOL CALL Klartext syntax.
With G17, G18, and G19, you define the tool axis.
The spindle speed S is defined as spindle revolutions per minute (rpm).
Alternatively, the constant cutting speed VC in meters per minute (m/min) can be defined.
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.
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.
N110 T1 G17 S( VC = 200 ) | ; Tool call with constant cutting speed |
The feed rate for linear axes is defined in millimeters per minute (mm/min).
In inch programs, the feed rate must be defined in 1/10 inch/min.
The feed rate for rotary axes is defined in degrees per minute (°/min).
The feed rate can be defined with an accuracy of three decimal places.
With the G99 NC function, you can define the dimensions/allowance of a tool.
Refer to your machine manual.
A tool definition created with G99 is a machine-dependent function.
HEIDENHAIN recommends using tool management for the definition of tools instead of G99!
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.
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.
110 G99 T3 L+10 R+5 | ; Define tool |
G99 corresponds to the TOOL DEF Klartext syntax.
When you use the G51 NC function, the control prepares a tool in the magazine, thus reducing the tool-change time.
Refer to your machine manual.
A tool pre-selection defined with G99 is a machine-dependent function.
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.
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.
110 G51 T3 | ; Tool pre-selection |
G51 corresponds to the TOOL DEF Klartext syntax.