About NC Machine Parameters

This section provides essential information about some NC machine parameters.

This page discusses:

Cutter Compensation

You can set cutter compensation options in the Compensation tab of the Generic Machine dialog box.

Cutter compensation instructions are generated on the NC data output depending on the selected mode as follows:

2D radial tip
Compensation is computed in a plane normal to the tool axis, and activated with regard to a cutter side (left or right). The radius that is compensated is the cutter radius. Output is the tool tip point (XT).
2D radial profile
Compensation is computed in a plane normal to the tool axis, and activated with regard to a cutter side (left or right). The radius that is compensated is the cutter radius. Output is the tool profile point (XP).
3D radial
Compensation is computed along a 3D vector (PQR), normal to the drive surface, in contact with the flank of the tool. The radius that is compensated is the cutter radius. Output is the tool tip point (XT) and PQR vector. Tool axis vector (IJK) is output in multi-axis.
3D contact
Compensation is computed along a 3D vector (XN), normal to the part surface, in contact with the end of the tool. The radius that is compensated is the corner radius. Output is the contact point (XC) and XN vector. The tool tip point (XT) may also be given if this choice is set on the machine. Tool axis vector (IJK) is output in multi-axis.

The table below specifies the compensation output modes available for each operation.

Machining Operation2D Radial Tip2D Radial Profile3D Radial3D Contact
Profile Contouring (between planes) Yes Yes - -
Pocketing Yes Yes - -
Circular Milling Yes Yes - -
Sweeping - - - Yes(*)
Contour Driven - - - Yes(*)
Spiral Milling - - - Yes(*)
ZLevel - - - Yes(*)
Isoparametric Machining - - - Yes
Multi-Axis Sweeping - - - Yes
Multi-Axis Curve (Contact) - - - Yes
Multi-Axis Contour Driven - - - Yes
Multi-Axis Helix Machining - - - Yes
Multi-Axis Flank Contouring - Yes Yes -

(*) In this release, only available when Offset Group with Offset Area is not used.

Circular Interpolation

This describes the machining operations supporting circular interpolation.

Machining Operations supporting circular interpolation are:

  • Roughing, Cavities Roughing, Multi-Pockets Machining: only when the Tool path style is set to Spiral, Concentric, Helical, or Offset from Part
    Note: contouring passes do not support circular interpolation.
  • Zlevel: only for circular macros.
  • Facing, Pocketing, Profile Contouring, Curve Following, and Groove Milling.
  • Circular Milling, Thread Milling (for circular macros), and T-Slotting.
  • Multi-Axis Curve Machining.
  • Circular macros of all Machining Operations but only for planar trajectories.