Compensating the tool angle of inclination with FUNCTION TCPM (#9 / #4-01-1)
Application
The FUNCTION TCPM function allows you to influence the positioning behavior of the control. When activating FUNCTION TCPM, the control compensates for any changed tool angles of inclination by means of compensating movements of the linear axes.
FUNCTION TCPM allows, for example, changing the tool angle of inclination for inclined machining while the position of the tool location point relative to the contour remains the same.
Instead of M128, HEIDENHAIN recommends using the more powerful function FUNCTION TCPM.
Related topics
- Compensating for the tool angle of inclination with M128
Compensating the tool angle of inclination automatically with M128 (#9 / #4-01-1)
- Tilting the working plane
- Presets on the tool
- Reference systems
Requirements
- Machine with rotary axes
- Kinematics description
To calculate the tilting angles, the control requires a kinematics description prepared by the machine manufacturer.
- Software option Advanced Functions Set 2 (#9 / #4-01-1)
Description of function
FUNCTION TCPM is an improvement on the M128 function which allows defining the behavior of the control while during the positioning of rotary axes.
Behavior without TCPM | Behavior with TCPM |
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. Please note that the compensation movement is performed in up to three axes.
When FUNCTION TCPM is active, the control shows the TCPM icon in the position display.
The FUNCTION RESET TCPM function resets the FUNCTION TCPM function.
Input
FUNCTION TCPM
10 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT CENTER-CENTER F1000 |
The NC function contains the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION TCPM | Syntax initiator for compensating tool angles of inclination |
F TCP or F CONT | Interpretation of the programmed feed rate |
AXIS POS or AXIS SPAT | Interpretation of programmed rotary axis coordinates |
PATHCTRL AXIS or PATHCTRL VECTOR | Interpolation of tool angle of inclination Interpolation of tool angle of inclination between start and end positions |
REFPNT TIP-TIP, REFPNT TIP-CENTER or REFPNT CENTER-CENTER | Selection of tool location point and tool rotation point Selection of tool location point and tool rotation point Optional syntax element |
F | Maximum feed rate for compensating movements in the linear axes for movements with a rotary-axis component Limiting the linear-axis feed rate Optional syntax element |
FUNCTION RESET TCPM
10 FUNCTION RESET TCPM |
The NC function contains the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION RESET TCPM | Syntax initiator for resetting of FUNCTION TCPM |
Interpretation of the programmed feed rate
The control offers the following options for interpreting the feed rate:
Selection | Function |
---|---|
F TCP | When selecting F TCP, the control interprets the programmed feed rate as the relative speed between the tool location point and the workpiece. |
F CONT | When selecting F CONT, the control interprets the programmed feed rate as contouring feed rate. In this process, the control transfers the contouring feed rate to the respective axes of the active NC block. |
Interpretation of the programmed rotary axis coordinates
The control offers the options below for interpreting the tool angle of inclination between the start and end position:
Selection | Function |
---|---|
When selecting AXIS POS, the control interprets the programmed rotary axis coordinates as axis angle. The control positions the rotary axes on the position defined in the NC program. The AXIS POS selection is primarily suitable in conjunction with perpendicularly arranged rotary axes. AXIS POS can only be used with different machine kinematics (e.g., 45° swivel heads) if the programmed rotary axis coordinates define the desired working plane alignment correctly (e.g., using a CAM system). | |
If AXIS SPAT is selected, the control interprets the programmed rotary axis coordinates as spatial angles. The control preferably implements the spatial angles as orientation of the coordinate system and tilts only required axes. Select AXIS SPAT to allow using NC programs regardless of kinematics. The AXIS SPAT selection item defines the spatial angles relative to the I-CS input coordinate system. The defined angles have the effect of incremental spatial angles. In the first traversing block after the function FUNCTION TCPM, always program with AXIS SPAT, SPA, SPB and SPC, including with spatial angles of 0°. |
Interpolation of tool angle of inclination between start and end positions
The control offers the options below for interpolating the tool angle of inclination between the programmed start and end positions:
Selection | Function |
---|---|
When selecting PATHCTRL AXIS, the control interpolates linearly between the start and end point. Use PATHCTRL AXIS with NC programs with small changes of the tool angle of inclination per NC block. In this case, the angle TA in Cycle 32 can be large. PATHCTRL AXIS can be used both for face milling and also for peripheral milling. 3D tool compensation during face milling (#9 / #4-01-1) 3D tool compensation during peripheral milling (#9 / #4-01-1) | |
If PATHCTRL VECTOR is selected, the tool orientation within an NC block always lies in the plane that is defined by the start orientation and end orientation. With PATHCTRL VECTOR the control generates a plane surface even if there are large changes in the tool inclination angle. Use PATHCTRL VECTOR for peripheral milling if there are large changes in the tool inclination angle per NC block. |
In both cases, the control moves the programmed tool location point on a straight line between the start position and end position.
To obtain continuous movement, define Cycle 32 with a tolerance for rotary axes.
Selection of tool location point and tool rotation point
The control offers the options below for defining the tool location point and the tool rotation point:
Selection | Function |
---|---|
REFPNT TIP-TIP | When selecting REFPNT TIP-TIP, the tool location point and the tool rotation point are located at the tool tip. |
REFPNT TIP-CENTER | When selecting REFPNT TIP-CENTER, the tool location point is located at the tool tip. The tool rotation point is located at the tool center point. |
REFPNT CENTER-CENTER | When selecting REFPNT CENTER-CENTER, the tool location point and the tool rotation point are located at the tool center point. Selecting REFPNT CENTER-CENTER allows executing CAM-generated NC programs which are referenced to the tool center point and still calibrate the tool relative to its tip. Tip This allows the control to monitor the entire tool length for collisions while machining is in progress. Previously, this functionality could only be achieved by shortening the tool with DL and without the control monitoring the remaining tool length. If you use REFPNT CENTER-CENTER to program pocket milling cycles, the control generates an error message. |
The reference point is optional. If you do not enter anything, the control uses REFPNT TIP-TIP.
Limiting the linear-axis feed rate
The optional input of F allows you to limit the feed rate of linear axes for motions with a rotary-axis component.
Thus, you can avoid fast compensation movements (e.g., in case of retraction movement at rapid traverse).
Make sure to select a value for the linear axis feed-rate limit that is not too small because large feed-rate variations may occur at the tool location point. Feed-rate variations impair the surface quality.
If FUNCTION TCPM is active, the feed-rate limit affect only motions with a rotary-axis component, not for entirely linear motions.
The linear axis feed-rate limit remains in effect until you program a new value or reset FUNCTION TCPM.
Notes
- Make sure to retract the tool before changing the position of the rotary axis
- Before positioning axes with M91 or M92, and before a TOOL CALL block, reset the FUNCTION TCPM function.
- The following cycles can be used with active FUNCTION TCPM:
- Cycle 32 TOLERANCE
- Cycle 444 PROBING IN 3-D (#17 / #1-05-1)
- M128 and FUNCTION TCPM with AXIS POS selected do not take into account an active 3D basic rotation. Program FUNCTION TCPM with AXIS SPAT selected, or CAM outputs with LN straight lines and a tool vector.
- Use only ball-nose cutters for face milling in order to avoid contour damage. In combination with other tool shapes, check the NC program for any possible contour damage by using the Simulation workspace.
Notes about machine parameters
The machine manufacturer uses the optional machine parameter presetToAlignAxis (no. 300203) to define for each axis how the control will interpret offset values. With FUNCTION TCPM and M128, the machine parameter is relevant only for the rotary axis that rotates about the tool axis (mostly C_OFFS).
Basic transformation and offset
- 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.