Turn bore finishing

Use the Turn bore finishing page to create a toolpath that machines a finishing pass for a bore feature in a turned part.

Cycle — Select from:

• Turn — This cycle roughs within the defined material boundaries by feeding parallel to the part's centre line along the Z axis while stepping down in the X axis. If you select a Negative cut direction, the tool cuts from right to left. If you select a Positive cut direction, the tool cuts from left to right.
• Face — This cycle roughs within the defined material boundaries by feeding perpendicular to the part's centre line while stepping into the face of the part along the Z axis in the negative direction. If you select a Negative cut direction, the tool cuts down the X axis, from the top to centreline. If you select a Positive cut direction, the tool cuts up the X axis, from the centreline to the top.
• Back face — This cycle roughs within the defined material boundaries by feeding perpendicular to the part's centre line while stepping into the face of the part along the Z axis in the positive direction. If you select a Negative cut direction, the tool cuts down the X axis, from the top to centreline. If you select a Positive cut direction, the tool cuts up the X axis, from the centreline to the top.

Tolerance — Enter a value to determine how accurately the toolpath follows the contours of the model.

Below centreline — Select this option to make the tool work on the negative X side of the turning centreline.

Cut direction — Select an option to specify the cutting direction of the tool:

• Positive — The tool cuts in the positive direction of the cutting axis, which depends on the selected Cycle.
  • Turn — The tool cuts in the +Z direction.
  • Face — The tool cuts in the +X direction.
  • Backface — The tool cuts in the +X direction.
• Negative — The tool cuts in the negative direction of the cutting axis, which depends on the selected Cycle.
  • Turn — The tool cuts in the -Z direction.
  • Face — The tool cuts in the -X direction.
  • Backface — The tool cuts in the -X direction.
• No drag — The tool cuts all vertical faces first, then cuts the horizontal areas. This can extend tool life and prevent chips from being dragged across the part.

Thickness — Enter the amount of material to be left on the part. Click the Thickness button to separate the Thickness box in to Radial thickness Axial thickness . Use these to specify separate Radial and Axial thickness as independent values. Separate Radial and Axial thickness values are useful for orthogonal parts. You can use independent thickness on sloping walled parts, although it is more difficult to predict the results.

Radial thickness — Enter the radial offset to the tool. When 2.5-axis or 3-axis machining, a positive value leaves material on vertical walls.

Axial thickness — Enter the offset to the tool, in the tool axis direction only. When 2.5-axis or 3-axis machining, a positive value leaves material on horizontal faces.

Previous thickness — Enter the amount of material left on the part from a previous roughing strategy.

Number of cuts — Enter the number of finishing passes.

Deburring — Select to automatically insert arc moves on outside corners.

— Deburring on.

— Deburring off.

The effects of deburring are:

• Wasted motion by the machine is minimised; however the posted part program may be slightly longer in the number of blocks used.
• Burrs are removed, but otherwise the part has the same shape and dimensions given by the feature curve because the radius of the inserted arc is the same as the tool nose radius.
• Machine motion is smoother.

Undercuts — Select an option to specify how the toolpath considers undercuts.