Table of Contents

Heidenhain Controller Support

This chapter explains HiNC support for NC codes of Heidenhain TNC640 and TNC530 controllers.

Heidenhain controllers support general ISO syntax. The general ISO syntax supported by HiNC is documented in other files.

If not mentioned in the documentation, it generally means it's not supported. R radius compensation command is not supported.

Format Support

Except for L code and FQ code, there must be spaces between letter instructions, otherwise, they cannot be parsed.

Can be parsed:

  • FMAX M03
  • LX-26.3 Y+43.1 Z+100.3 A-90.0 C+13.123 FQ3

Cannot be parsed: FMAXM03

Support for L move command.

Can be parsed:

  • LX+0Y+0FMAX
  • L X+0 Y+0 FMAX

Macro Support

Q Variable Assignment

Support for Q variable assignment.

Can be parsed:

  • Q1 = 5000
  • Q2 = 123
  • Q3 = 1000
  • LX-26.3 Y+43.1 Z+100.3 A-90.0 C+13.123 FQ3

Q Variable Operations

Support for the following macro operations:

  • FN0 specify a value.
  • FN1 calculate and specify the sum of two values.
  • FN2 calculate and specify the difference of two values.
  • FN3 calculate and specify the product of two values.

Can be parsed:

  • FN0: Q1 = 5000
  • FN1: Q1 = -Q2 + -5
  • FN2: Q1 = +10 - +5
  • FN3: Q2 = +3 * +3

TOOL CALL

Support for TOOL CALL, but the tool name must be a number.

Can be parsed:

  • TOOL CALL "1" Z S5000
  • TOOL CALL 1 Z S5000

Cannot be parsed: TOOL CALL "ET1" S5000

CYCL DEF 7

Support for CYCL DEF 7 workpiece origin offset command.

Can be parsed:

CYCL DEF 7.0 DATUM SHIFT
CYCL DEF 7.1 X10.123
CYCL DEF 7.2 Y22.223
CYCL DEF 7.3 Z32.97

CYCL DEF 247

Support for CYCL DEF 247 workpiece origin setting. Supports Q339 coordinate index.

Can be parsed: CYCL DEF 247 Q339=+1

PLANE Series Instructions

Motion Behavior Instructions

Support for one of three motion behavior instructions: { STAY , TURN , MOVE } .

SEQ

Support for { SEQ+ , SEQ- } active spindle rotation direction instructions.

TABLE ROT

Support for TABLE ROT worktable rotation instructions.

PLANE SPATIAL

Can be parsed: PLANE SPATIAL SPA-60.3 SPB+0 SPC-19.88 STAY SEQ- TABLE ROT

PLANE RESET

Can be parsed: PLANE RESET STAY

Heidenhain Specific M Codes

Support for the following Heidenhain specific M codes. General ISO M codes are documented elsewhere.

M91

Support for M91 single-line effective mechanical coordinate displacement.

Can be parsed: L Z-1 F5000 M91

M107

Skip M107 display error message command.

M108

Skip M108 reset M107 command.

M126

Support for M126 move on the rotary axis with a shorter path.

M127

Support for M127 reset M126 command.

Controller Parameter Field 300401

Support for controller parameter field 300401, if this parameter is true, regardless of whether M127 is issued, it will move on the rotary axis with a shorter path.

Parameter field 300401 default value is true.

M128

Support for M128 enable Tool Center Point Management (TCPM).

M129

Support for M129 disable Tool Center Point Management (TCPM).

M140

Support for M140 MB M140 MB MAX retract tool command.

Can be parsed:

  • M140 MB MAX
  • M140 MB+50 F6000