The control uses M144 in subsequent traverse movements to compensate for tool offsets that result from inclined rotary axes.
Instead of M144, HEIDENHAIN recommends using the more powerful function FUNCTION TCPM (option 9).
The control uses M144 in subsequent traverse movements to compensate for tool offsets that result from inclined rotary axes.
Instead of M144, HEIDENHAIN recommends using the more powerful function FUNCTION TCPM (option 9).
Compensating for the tool angle of inclination with FUNCTION TCPM (option 9)
M144 takes effect at the start of the block.
In order to reset M144, program M145.
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.
11 M144 | ; Activate tool compensation |
12 L A-40 F500 | ; Position the A axis |
13 L X+0 Y+0 R0 FMAX | ; Position the X and Y axes |
With M144 the control takes the position of the rotary axes into account in the subsequent positioning blocks.
In NC block 12 the control positions the rotary axis A, resulting in an offset between the tool tip and the workpiece. The control compensates for this offset mathematically.
In the next NC block the control positions the X and Y axes. When M144 is active, the control compensates for the position of the rotary axis A during this movement.
Without M144 the control does not take the offset into account, and the machining operation is performed with this offset.
Refer to your machine manual.
When working with angle heads, keep in mind that the machine geometry is defined by the machine manufacturer in a kinematics description. If you use an angle head during machining, then you must select the correct kinematics description.
Miscellaneous functions for coordinate entries
Tilting the working plane with PLANE functions (option 8)
With M144 the control moves according to the workpiece coordinate system W-CS.
If you activate PLANE functions, the control moves according to the working plane coordinate system WPL-CS.
If the inclined axis is a swivel head, the control does not orient the W-CS.