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.

 
Tip

Instead of M128, HEIDENHAIN recommends using the more powerful function FUNCTION TCPM.

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 Positions workspace

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

Interpretation of the programmed feed rate

AXIS POS or AXIS SPAT

Interpretation of programmed rotary axis coordinates

Interpretation of the programmed rotary axis coordinates

PATHCTRL AXIS or PATHCTRL VECTOR

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

AXIS POS

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).

AXIS SPAT

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°.

Input coordinate system I-CS

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

PATHCTRL AXIS

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.

Cycle 32 TOLERANCE

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)

PATHCTRL VECTOR

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.

 
Tip

To obtain continuous movement, define Cycle 32 with a tolerance for rotary axes.

Cycle 32 TOLERANCE

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.

Tool data within variables

If you use REFPNT CENTER-CENTER to program pocket milling cycles, the control generates an error message.

Milling pockets

Presets on the tool

The reference point is optional. If you do not enter anything, the control uses REFPNT TIP-TIP.

Selection options of tool location point and tool rotation point

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).

 
Tip

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

 
Notice
Danger of collision!
Rotary axes with Hirth coupling must move out of the coupling to enable tilting. There is a danger of collision while the axis moves out of the coupling and during the tilting operation.
  1. 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.
  • Basic rotation and 3D basic rotation

  • Straight line LN

  • 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

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.
  • 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.