Steep and shallow finishing

Use the Steep and shallow finishing page to create a Constant Z toolpath in the steep regions of a model and a 3D offset or Raster toolpath in the shallow regions.

This differs from Optimised constant Z finishing as you can specify when to change from 3D offset machining to constant Z machining using the Threshold angle field, and you can specify an Overlap where both steep and shallow toolpaths are created. Also, optimised constant Z finishing only uses whole segments, whereas steep and shallow finishing will split segments at the shallow boundary. This means that steep and shallow finishing toolpaths have far more retracts than optimised constant Z toolpaths.

Additional stock — Use this option to aid ordering when machining between two steep walls so PowerMill produces a safe order with the level of stock specified here. Providing the passes are within the distance specified, an alternating toolpath is created, machining at one Z height on one wall, and then at the same Z height on the neighbouring wall before descending to the next Z height.

Note: If the Additional stock is zero, PowerMill uses a default value of one tenth of the tool radius.

Note: This option is available only if you have an Order of Steep first.

Threshold angle — Enter the surface slope, measured from the horizontal, that determines the split between constant Z (steep) and shallow machining.

— Shows the 3D Offset toolpath in the shallow areas.

— Shows the Constant Z toolpath in the steep areas.

Steep shallow overlap — Enter the size of the overlap area where constant Z (steep) and shallow machining occur. This minimises marks on the model caused by a sudden switch from constant Z to shallow machining.

— Shows the 3D Offset toolpath overlapping into the steep areas.

— Shows the Constant Z toolpath.

Steep — The options for the constant Z portion of the toolpath.

Shallow — The options for the raster/offset portion of the toolpath.

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.

Selecting Spiral converts this:

to this:

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.

Stepdown — Enter the distance between successive machining passes. The Stepdown is for the steep portions of the toolpath.

Stepover — Enter the distance between successive machining passes. The Stepover is for the shallow portions of the toolpath.

— Shows the 3D Offset toolpath stepover in the shallow areas.

— Shows the Constant Z toolpath stepdown in the steep areas.

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.

Note: 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.

Calculate using cusp — Select this option to determine the stepdown by the Cusp height, with a maximum stepdown determined by the Maximum stepdown value. When deselected, the stepdown between successive Z heights has a constant value equal to the Minimum Stepdown value.

Type — Select whether PowerMill creates a Raster or Offset toolpath in the shallow regions.

Type — Offset

Type — Raster

Note: As a general rule, use raster on open-edged parts and 3D offsets at the bottom of a pocket.

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

Selecting the Smoothing option converts this:

to this:

Note: This option is available only if you have a Type of 3D offset.

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:

Note: This option is available only if you have a Type of 3D offset.

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

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.

Note: When 3D offsetting the bottom of a pocket, PowerMill machines from outside, inwards. However, when machining the top of a boss (an area with no steep regions above it) PowerMill machines from inside, outwards.