Compensating the tool angle of inclination automatically with M128 (#9 / #4-01-1)
Application
If the position of a controlled rotary axis changes in the NC program, then the control uses M128 during the tilting procedure to automatically compensate for the tool inclination with a compensating movement of the linear axes. That way the position of the tool tip relative to the workpiece surface remains unchanged (TCPM).
Instead of M128, HEIDENHAIN recommends using the more powerful function FUNCTION TCPM.
Related topics
- Compensating for tool offset with FUNCTION TCPM
Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
Requirements
- Machine with rotary axes
- Kinematics description
- Machine
Refer to your machine manual.
The machine manufacturer creates the kinematics description of the machine.
- Software option Adv. Function Set 2 (#9 / #4-01-1)
Description of function
Effect
M128 takes effect at the start of the block.
You can reset M128 with the following functions:
- M129
- FUNCTION RESET TCPM
- In the Program Run operating mode, select a different NC program
M128 is also in effect in the Manual operating mode and remains active even after a change in the operating mode.
Application example
Behavior without M128 | Behavior with M128 |
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 L X+100 B-30 F800 M128 F1000 | ; Move with automatic compensation of the motion in the rotary axis |
In this NC block the control activates M128 with the feed rate for the compensating movement. The control then simultaneously moves the tool in the X axis and in the B axis.
In order to keep the position of the tool tip constant relative to the workpiece while inclining the rotary axis, the control uses the linear axes to perform a continuous compensating movement. In this example the control performs the compensating movement in the X and Z axes.
Without M128 an offset of the tool tip relative to the nominal position results as soon as the inclination angle of the tool changes. The control does not compensate for this offset. If you do not take this deviation into account in the NC program, the machining operation will not be performed correctly or a collision will occur.
The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message. Note that the compensating movement is performed in up to three linear axes.
Input
If you define M128, the control continues the dialog and prompts you for the feed rate F. The defined value limits the feed rate of the linear axis during the compensating movement.
Inclined machining with open-loop rotary axes
With open-loop rotary axes, also known as counter axes, you can also perform inclined machining in combination with M128.
For inclined machining operations with open-loop rotary axes, proceed as follows:
|
As long as M128 is active, the control monitors the actual positions of the open-loop rotary axes. If the actual position deviates from the value that is defined by the machine manufacturer, then the control issues an error message and interrupts program run.
Notes
- Make sure to retract the tool before changing the position of the rotary axis
- Use the Simulation mode to test the NC program before execution
- Slowly prove-out the NC program
3D tool compensation during peripheral milling (#9 / #4-01-1)
- The feed rate for the compensating movement remains in effect until you program a new feed rate or rescind M128.
- If M128 is active, the control shows the TCPM icon in the Positions workspace.
- If you always select the first selection option offered for FUNCTION TCPM, you will achieve the same functionality as with M128. In this case program the syntax FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-TIP.
- M128 and FUNCTION TCPM with AXIS POS selected do not take an active basic rotation or 3D basic rotation into account. Program FUNCTION TCPM with AXIS SPAT selected, or CAM outputs with LN straight lines and a tool vector.
Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
- If M128 is active, the control selects the tilting solution with the smallest number of rotary axis movements from the current position for LN straight lines.
- You define the inclination angle of the tool by entering the axis positions of the rotary axes directly. This way the values refer to the machine coordinate system M-CS. For machines with head rotation axes the tool coordinate system T-CS changes. For machines with table rotary axes the workpiece coordinate system W-CS changes.
- If you run the following functions while M128 is active, then the control cancels program run and issues an error message:
- M91
- M92
- M144
- Calling a tool with TOOL CALL
- Dynamic Collision Monitoring (DCM (#40 / #5-03-1)) and simultaneous use of M118 (#21 / #4-02-1)
Notes about machine parameters
- In the optional machine parameter maxCompFeed (no. 201303), the machine manufacturer defines the maximum speed of compensating movements.
- In the optional machine parameter maxAngleTolerance (no. 205303), the machine manufacturer defines the maximum angle tolerance.
- In the optional machine parameter maxLinearTolerance (no. 205305), the machine manufacturer defines the maximum linear axis tolerance.
- In the optional machine parameter manualOversize (no. 205304), the machine manufacturer defines a manual oversize for all collision objects.
- The machine manufacturer uses the optional machine parameter presetToAlignAxis (no. 300203) to define for each axis how the control will interpret offset values. For FUNCTION TCPM and M128 the machine parameter applies only to one rotary axis of the table that rotates about the tool axis (in most cases C_OFFS).
- If the machine parameter is not defined or is defined with the value TRUE, then you can compensate for a workpiece misalignment in the plane with the offset. The offset affects the orientation of the workpiece coordinate system W-CS.
- If the machine parameter is defined with the value FALSE, then you cannot compensate for a workpiece misalignment in the plane. The control does not take the offset into account during program run.
Notes on tools
If you incline a tool while machining a contour, you must use a ball-nose cutter; otherwise the tool can damage the contour.
In order to avoid damaging a contour while machining it with a ball-nose cutter, note the following:
- With M128 the control equates the tool rotation point with the tool location point. If the tool rotation point is at the tool tip, the tool will damage the contour if the tool is inclined. Therefore the tool location point must be at the tool center point.
- In order for the control to display the tool correctly in the simulation, you must define its actual length in the column L of the tool management.
When calling the tool in the NC program, define the sphere radius as a negative delta value in DL and thus shift the tool location point to the tool center point.
For Dynamic Collision Monitoring (DCM (#40 / #5-03-1)), you need to define the actual tool length in tool management, too.
- If the tool location point is at the tool center point you must modify the coordinates of the tool axis in the NC program by the value of the sphere radius.
In FUNCTION TCPM you can choose the tool location point and the tool rotation point separately from each other.
Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
Definition
Abbreviation | Definition |
---|---|
TCPM (tool center point management) | Maintain the position of the tool location point |