Inlay Wizard — Cutting Depth

Use the options in the Cutting Depth area to specify the cutting depths, tolerance, and allowance.

• Start Depth — Enter the depth (Z) from the surface of the material at which you want to begin machining.
• Finish Depth — Enter the final depth (Z) for the tool.
• Allowance — Enter a zero or positive value to specify the clearance fit between interlocking male and female parts. Depending on the type of inlay selected, enter a positive value to increase the size of the pocket or to decrease the size of the insert.
• Tolerance — Enter a value in the box to specify how closely the tool follows the shape of the selected vectors. Entering excessively small values increases the size of the toolpath file and slows down calculation and machining times.
• Machine safe Z — Click the control bar and enter:
  • a value in the Safe Z box to specify the height at which the tool makes rapid moves between toolpath segments. This value must be sufficient to clear any clamps used to hold your material block or sheet in position.
  • values in the X, Y, and Z boxes to specify the coordinates of the tool's start and end position. This should be a safe distance away from the material block or sheet.
• Shoulder dimensions — Specify the dimensions of the stepped pocket, stepped hole, or stepped insert:
  • Depth (d) — Enter the depth of the shoulder from the Start Depth.
  • Width (s) — Enter the width of the shoulder.
• Tool — Click Select to select the tool you want to use using the Tool Database dialog. When you select the tool, click the control bar showing the name of the tool to display its parameters. To change the selected tool, click Select again.
• Use roughing tool — If you want to use a roughing tool to clear the area, select Use Roughing Tool, and click Select to choose a roughing tool from the Tool Database. If no roughing tool is selected, the finishing tool is used to machine the whole area.
• Allowance — Specify an allowance of material for the roughing tool to leave behind for the finishing tool.
• Strategy — Select a clearance strategy. If you are using a roughing tool, the strategy that you select applies to the selected tool and an Offset strategy with a Climb Mill cut direction is applied by default to the finishing tool. If you are not using a roughing tool, the strategy that you select applies to the finishing tool.
  • Raster — This strategy machines in passes back and forth along the X-axis at a specified angle. If you select this strategy, define the angle you want the tool to move at in the Angle box.
    Tip: Set the default raster angle on the Options panel.

    Select a Profile Pass option:

    None — Select this option if you do not want the tool to profile the selected vector.

    First — Select this option if you want the tool to profile the selected vector first and then raster clear the area.

    Last — Select this option if you want the tool to move outwards to raster clear the area, then profile the selected vector.

  • Offset — This strategy machines in repeated passes, each time moving inwards by the Stepover value of the tool you use.
    Tip: You can see the stepover value of the selected tool when the machining parameters are displayed in the Roughing Tool or Finishing Tool areas.

    Select a Cut Direction option:

    Climb — Climb milling rotates the cutter in the same direction as the feed motion.

    Conventional — Conventional milling rotates the cutter in the opposite direction to the feed motion.

    Tip: Set the default cutting direction on the Options panel.

    Select a Start From option:

    Outside — Select this option if you want the tool to cut into the material at the vector's boundary, then machine inwards.

    Inside — Select this option if you want the tool to cut into the material at the vector's centre, then machine outwards.

• Cut direction — Click the control bar to specify the cut direction of the tool.
  • Climb mill — Select the option to rotate the cutter in the same direction as the feed motion. The option is selected by default.
  • Conventional — Select the option to rotate the cutter in the opposite direction to the feed motion.
• Add Ramping Moves — Select the check box to add ramping moves to the toolpath. This displays the ramping settings. All of the ramping move settings are selected by default. Deselect any of the settings you do not require. The boxes for the deselected options are unavailable.
  • Max Ramp Angle (A) — Enter the maximum angle of descent for each zig and zag movement of the tools.
  • Max Ramp Length (L) — Enter the maximum distance that you want the tools to zigzag across the material surface.
  • Min Ramp Length (Lmin) — Enter the minimum distance that you want the tools to zigzag across the material surface.
  • Zig Start Height (S) — Enter the height at which the ramping moves start.
    Note: If you do not select the Zig Start Height (S) option, the Safe Z level specified in the Machine Safe Z area is used instead.
• Lock start points — Select this option if you want to ensure the start points for the toolpath segments are as near as possible to the start points of the corresponding vectors.
• Add Bridges — Select the check box to add bridges to the vectors you are using to create the toolpath. Bridging is a precautionary measure to prevent profiled vector artwork from shifting in the material block as it is machined.
• Click to define material — Click the control bar and specify the block or sheet of material using the Material Setup dialog. When you specify the material settings, the material's thickness is displayed on the control bar. To change the settings, click Setup.

Note: The availability of some options is dependent on the type of inlay toolpath.

See also

• About cut direction
• About ramping moves
• Adding bridges
• Specifying the material setup