3D offset finishing

Use the 3D offset finishing page to create a series of offsets starting at the outer boundary and offsetting towards the centre.

Pattern — This defines the shape of the offsets. If no pattern is selected, then the block is offset.

• If no pattern is selected, assuming a block at the extents of the model, this toolpath is generated.

  

• If you select this pattern:

  

  This toolpath is generated:

  

Create pattern — Click to create a new empty pattern.

Selected pattern — Select a pattern from the list. If no pattern is displayed, or is selected, then no pattern is selected. The list contains a list of all available patterns.

Select picked pattern — Click to select a pattern by picking in the graphics window, rather than by name in the Select pattern list.

Clicking displays the Pick Entity tab. Select a pattern in the graphics window to close the Pick Entity tab and display the pattern in the Selected Pattern field.

Collect curves — Click to copy the selected curves into the pattern. This provides a fast, powerful means of extracting curve geometry from a surface model and copying it into the active pattern/boundary. For more information, see the collecting curves example.

Offset direction — Specify the direction that the toolpath offset is calculated from.

• Outside In — The toolpath offset is calculated from the outside in.
• Inside Out — The toolpath offset is calculated from the inside out.

Spiral — Select to create a spiral 3D offset toolpath by converting multiple closed contours into a single spiral.

Spiral on:

Spiral off:

This minimises the number of lifts of the tool and maximises cutting time while maintaining more constant load conditions and deflections on the tool.

Smoothing — Select to smooth offsets of toolpath segments over the model.

Smoothing on:

Smoothing off:

Centreline — Select to include a pass over the centreline of toolpath corner junctions. This removes small cusps created at the junctions.

Centreline off:

Centreline on:

Maximum offsets — Enter the maximum number of offsets used for the toolpath.

With Maximum offsets deselected gives this result:

With Maximum offset selected and a number of offsets of 5 gives this result:

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

Cut direction — Select the milling technology.

Select a Cut Direction from the following:

• Climb — Select to create toolpaths using only climb milling, where possible. The tool is on the left of the machined edge when viewed in the direction of tool travel.

  

• Conventional — Select to create toolpaths using only conventional or upcut milling, where possible. The tool is on the right of the machined edge when viewed in the direction of tool travel.

  

• Any — Select to create toolpaths using both conventional and climb milling. This minimises the tool lifts and tool travel.

Note: If you select a Cut direction of Any, closed segments default to Climb cutting.

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.

Component thickness — Click to display the Component thickness dialog, which enables you to specify the thicknesses of the different surfaces.

Stepover — Enter the distance between successive machining passes.

• Copy stepover from tool — Click to load the radial depth of cut from the active tool's cutting data. The radial depth of cut is measured normal to the tool axis.
• Edited — When displayed, shows value entered by you (or another user). Click to change this value to the automatically calculated value.
• Stepover — Enter the distance between successive machining passes.

  If you enter a Stepover value, then changes to .

• Cusp height — Enter the maximum cusp height and use this value to determine the stepover. PowerMill calculates the stepover value to give a cusp height of the machining tolerance using the current tool, when machining a plane inclined at 45. This is the worst case cusp height for any given tolerance.

  

  Stepdown

  Stepover

  Cusp height

  For more information see Linkage between stepover and cusp height.