3D tool compensation during face milling (#9 / #4-01-1)

Application

Face milling is a machining operation carried out with the front face of the tool.

The control displaces the tool in the direction of the surface normals by the total of the delta values from tool management, tool call and compensation tables.

Requirements

Description of function

The variants below are possible with face milling:

  • LN block with tool orientation T, M128 or FUNCTION TCPM is active: Tool keeps the set tool orientation
  • LN block without M128 or FUNCTION TCPM: The control ignores the direction vector T even if it is defined
  • LN block without tool orientation T, but with a surface-normal vector N, with M128, or FUNCTION TCPM active: The control interprets the surface-normal vector N as the tool vector T, too, and approaches the tool perpendicularly to the workpiece contour. For safety reasons, HEIDENHAIN does not recommend this kind of programming.

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.If the axis position does not change, you can nevertheless program more than four axes.

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.

Example

11 L X+36.0084 Y+6.177 Z-1.9209 R0

; No compensation is possible

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.

11 LN X+36.0084 Y+6.177 Z-1.9209 NX-0.4658107 NY+0 NZ+0.8848844 TX+0.0000000 TY+0.6558846 TZ+0.7548612 R0 M128

; Compensation is possible, DL is effective along the T vector and DR2 along the N vector

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.

11 LN X+36.0084 Y+6.177 Z-1.9209 NX-0.4658107 NY+0 NZ+0.8848844 R0 M128

; Compensation perpendicular to the contour is possible

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.

11 LN X+36.0084 Y+6.177 Z-1.9209 NX-0.4658107 NY+0 NZ+0.8848844 R0

; Compensation perpendicular to the contour is possible

Notes

 
Notice
Danger of collision!
The rotary axes of a machine may have limited ranges of traverse (e.g., between –90° and +10° for the B head axis). Changing the tilt angle to a value of more than +10° may result in a 180° rotation of the table axis. There is a danger of collision during the tilting movement!
  1. Program a safe tool position before the tilting movement, if necessary.
  2. Carefully test the NC program or program section in the Single Block mode
  • If no tool orientation was defined in the LN block, and TCPM is active, then the control maintains the tool perpendicular to the workpiece contour.
  • If a tool orientation T has been defined in the LN block and M128 (or FUNCTION TCPM) is active at the same time, then the control will position the rotary axes automatically in such a way that the tool can reach the specified tool orientation. If you have not activated M128 (or FUNCTION TCPM), then the TNC ignores the direction vector T, even if it is defined in the LN block.
  • The control is not able to automatically position the rotary axes on all machines.
  • The control generally uses the defined delta values for 3D tool compensation. The entire tool radius (R + DR) is only taken into account if you have activated the FUNCTION PROG PATH IS CONTOUR function.
  • 3D tool compensation with the entire tool radius with FUNCTION PROG PATH (#9 / #4-01-1)

Examples

Compensate re-worked ball-nose cutter
CAM output at tool tip

Use a re-worked Ø 5.8 mm ball-nose cutter instead of Ø 6 mm.

The NC program has the following structure:

  • CAM output for Ø 6 mm ball-nose cutter
  • NC points output on the tool tip
  • Vector program with surface normal vectors

Proposed solution:

  • Tool measurement on tool tip
  • Enter the tool compensation into the tool table:
    • R and R2 the theoretical tool data as from the CAM system
    • DR and DR2 the difference between the nominal value and actual value

R

R2

DL

DR

DR2

CAM

+3

+3

Tool table

+3

+3

+0

-0.1

-0.1

Compensate re-worked ball-nose cutter
CAM output at the center of the ball

Use a re-worked Ø 5.8 mm ball-nose cutter instead of Ø 6 mm.

The NC program has the following structure:

  • CAM output for Ø 6 mm ball-nose cutter
  • NC points output on the center of the ball
  • Vector program with surface normal vectors

Suggested solution:

  • Tool measurement on tool tip
  • TCPM function REFPNT CNT-CNT
  • Enter the tool compensation into the tool table:
    • R and R2 the theoretical tool data as from the CAM system
    • DR and DR2 the difference between the nominal value and actual value

R

R2

DL

DR

DR2

CAM

+3

+3

Tool table

+3

+3

+0

-0.1

-0.1

 
Tip

With TCPM REFPNT CNT-CNT the tool compensation values are identical for the outputs on the tool tip or center of the ball.

Create workpiece oversize
CAM output at tool tip

Use a Ø 6 mm ball-nose cutter for achieving an even oversize of 0.2 mm on the contour.

The NC program has the following structure:

  • CAM output for Ø 6 mm ball-nose cutter
  • NC points output on the tool tip
  • Vector program with surface normal vectors and tool vectors

Proposed solution:

  • Tool measurement on tool tip
  • Enter the tool compensation into the TOOL CALL block:
    • DL, DR and DR2 the desired oversize
  • Suppress the error message with M107

R

R2

DL

DR

DR2

CAM

+3

+3

Tool table

+3

+3

+0

+0

+0

TOOL CALL

+0.2

+0.2

+0.2

Create workpiece oversize
CAM output at the center of the ball

Use a Ø 6 mm ball-nose cutter for achieving an even oversize of 0.2 mm on the contour.

The NC program has the following structure:

  • CAM output for Ø 6 mm ball-nose cutter
  • NC points output on the center of the ball
  • TCPM function REFPNT CNT-CNT
  • Vector program with surface normal vectors and tool vectors

Proposed solution:

  • Tool measurement on tool tip
  • Enter the tool compensation into the TOOL CALL block:
    • DL, DR and DR2 the desired oversize
  • Suppress the error message with M107

R

R2

DL

DR

DR2

CAM

+3

+3

Tool table

+3

+3

+0

+0

+0

TOOL CALL

+0.2

+0.2

+0.2