Taking the tool offset into account in calculations with M144 (#9 / #4-01-1)
Application
The control uses M144 in subsequent traverse movements to compensate for tool offsets that result from inclined rotary axes.
You can use M144 (#50 / #4-03-1) for an inclined turning operation, for example.
HEIDENHAIN recommends using the more powerful function FUNCTION TCPM (#9 / #4-01-1) instead of M144.
Exceptions are, e.g.:
- RL or RR positioning blocks with tool radius compensation
- Positioning blocks with M91
- Positioning blocks with tool tip radius compensation SRK (#50 / #4-03-1)
Related topics
- Compensating for tool offset with FUNCTION TCPM
Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
- Inclined turning (#50 / #4-03-1)
Requirement
- Software option Adv. Function Set 2 (#9 / #4-01-1)
Description of function
Effect
M144 takes effect at the start of the block.
In order to reset M144, program M145.
Application example
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.
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.
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.
Notes
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.
- You can use M91 and M92 for positioning even when M144 is active.
- The functions M128 and FUNCTION TCPM are not permitted when M144 is active. The control will issue an error message if you try to active these functions.
- M144 does not work in connection with PLANE functions. If both functions are active, then the PLANE function is in effect.
Tilting the working plane with PLANE functions (#8 / #1-01-1)
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.
Notes on turning (#50 / #4-03-1)
- If the inclined axis is a tilting table, the control changes the orientation of the workpiece coordinate system W-CS versus the machine coordinate system M-CS.
If the tilted axis is a swivel head, the control changes the orientation of the tool coordinate system T-CS versus the machine coordinate system M-CS.
- After inclining a rotary axis, you possibly have to pre-position the turning tool in the Y coordinate and orient the position of the tool tip with Cycle 800 ADJUST XZ SYSTEM.