Compensating for the tool angle of inclination with FUNCTION TCPM (option 9)

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.

  • Advanced Functions Set 2 (software option 9)

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.

M128_inaktiv
M128_aktiv

Behavior without TCPM

Behavior with TCPM

When FUNCTION TCPM is active, the control shows the TCPM icon in the position display.

Positions workspace

The FUNCTION RESET TCPM function resets the FUNCTION TCPM function.

Input

FUNCTION TCPM

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.

 
Tip

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.

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

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.

 
Tip

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.

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_POSITION_1
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_SPATIAL_01
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

PATH_CONTROL_Vector
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 (option 9)

3D tool compensation during peripheral milling (option 9)

PATH_CONTROL_AXIS
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 generate 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.

The option REFPNT TIP-CENTER is optimized for turning tools (option 50). When the control positions the rotary axes, the tool rotation point remains at the same position. This allows you, for example, to machine complex contours by simultaneous turning.

Theoretical and virtual tool tip

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.

Overview

Presets on the tool

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

TURN_MILL_TOOL
Selection options of tool preset 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 800 ADJUST XZ SYSTEM (option 50)
    • Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING (option 158)
    • Cycle 883 TURNING SIMULTANEOUS FINISHING (option 158)
    • Cycle 444 PROBING IN 3-D
  • 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, 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 is to interpret offset values. For FUNCTION TCPM and M128, the machine parameter applies only to the rotary axis that rotates about the tool axis (in most cases C_OFFS).

Basic transformation and offset

  • If the machine parameter axis has not been defined or has been set to TRUE, the offset can be used to compensate a misalignment of the workpiece in the plane. The offset affects the orientation of the workpiece coordinate system W-CS.
  • Workpiece coordinate system W-CS

  • If the machine parameter axis has been defined with FALSE, the offset cannot be used to compensate a misalignment of the workpiece in the plane. The control will not take the offset into account when executing the commands.