Constant Z finishing

Use the Constant Z finishing page to create a toolpath by slicing the model at specific Z Heights.

Order by — Select whether machining takes place by Region or by Level.

• Region — When selected, one region (such as a pocket or boss) is completely machined before going on to the next. So, pockets are machined in preference to levels.

  

• Level —When selected, one level is completely machined before going down to the next. So, levels are machined in preference to pockets.

  

Spiral — Select this option to create a spiral path between two consecutive closed contours. This minimises the number of lifts of the tool and maximises cutting time while maintaining more constant load conditions and deflections on the tool.

Spiral option — Deselected:

Spiral option —Selected:

Undercut — Select this option to produce a toolpath where the cutter can touch the part, so you can machine areas with undercuts.

If you start with this model:

Undercut — Selected:

Undercut — Deselected:

— Areas not fully machined.

• If a vertical tool axis is used, undercuts work with ball nosed, tapered spherical and tipped disc tools.
• If the tool axis is not vertical then undercuts work with ball nosed, tapered spherical and spherical tipped disc tools.

  Not all tipped disc tools work with a non-vertical axis, only those with a (hemi)spherical end, (where diameter=2*tip radius).

Note: When Undercut is selected, the Additional stock and Machine down to flats options are unavailable. The Unsafe segment removal page is also unavailable.

Machine down to flats — Select this option to add a constant Z slice on flat surfaces at the bottom of steep features.

Machine down to flats — Selected:

— Flat surface

Machine down to flats — Deselected:

Flat tolerance — Enter the Z range that determines whether a surface is flat.

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: Any allows zigzag cutting on open toolpath segments. Closed segments default to Climb cutting. To change the cut direction for closed segments, click Toolpath Edit tab > Edit panel > Reorder.

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.