How does the 3D Finish toolpath work in VCarve Pro & Aspire: Raster vs Offset, stepover, tool choice, and quality settings?

Overview

The 3D Finish toolpath makes the final surface pass over your 3D composite model. It runs at a fine stepover to produce smooth, detailed results. It is always a single-pass toolpath and does not use the tool's Pass Depth setting, so your Rough toolpath must have removed most material first. It is available in both VCarve Pro and Aspire.

Machining Limit Boundary

The area in which the tool operates. Options: Model Boundary (the combined boundaries of all components in the job), Material Boundary (the whole material block), Selected Vector(s), or Selected Level (the components on one named level). When machining a raised object, a Boundary Offset enlarges the boundary so the tool can go past the actual edge.

Two Fill Strategies

Raster

Moves back and forth across the model in parallel lines (a "lace cut" projected onto the 3D surface) at a controlled angle.

Raster Angle: Between 0 and 90°. 0° is mainly parallel to the X axis, 90° is mainly parallel to the Y axis.

When to use Raster:

• Flat or shallow models
• Models with a dominant direction (grains, flows, directional textures)
• Faster to calculate and a simpler toolpath structure
• Running with the wood grain to minimize tearout on the finish

Offset

Moves in concentric paths that follow the model's contours, stepping inward (or outward) by the stepover amount. Climb or Conventional cutting is chosen mainly by the material and tooling.

Stepover Retract: A value greater than 0 lifts the tool off the surface of the model by that amount when stepping between offset contours. Depending on material and tooling, a small lift can eliminate perpendicular tool marks between contours. You get a warning if the value is too small to lift the tool over the previous cusp height.

When to use Offset:

• Curved profiles, mouldings, bowls, round elements
• Models with radial symmetry (Turn and Spin results, which are Aspire only, and round plaques)
• The offset lines follow the shape and look more natural in the final surface
• Arched and curved mouldings: select the boundary vector and use Offset for passes that follow the curve

Stepover: The Most Important Setting

Stepover controls scallop height, the tiny ridges left between tool passes. Smaller stepover = smoother surface = much longer machining time. The official documentation says 8 to 12% of the tool diameter is typical for ball nose finishing.

Starting points for wood (test on scrap):

• Rough finish: 10 to 15% of tool diameter
• Standard finish: 8 to 12% of tool diameter
• Fine detail: 4 to 8% of tool diameter

Real-world example: A 6mm ball nose at 8% stepover = 0.48mm stepover. On a 600 x 600mm panel that's a very long finish pass.

The tradeoff: Doubling the stepover roughly halves the time but makes the scallops about four times taller. Finding the right balance depends on how closely the piece will be inspected and whether it will be painted (painted pieces can use larger stepovers than a natural wood finish). Use the preview to check finish quality and detail. If it is not good enough, you may need a smaller tool or a smaller stepover.

Tool Choice

Ball nose end mill is standard for 3D finishing. The rounded tip traces the surface smoothly.

Tapered ball nose offers more strength at very small diameters, which makes it a good choice for fine detail work with sub-3mm tip diameters.

General rule: Use the smallest ball nose that gives the detail you need, but not so small that it risks breaking on any remaining material the rough pass left behind.

Multiple Tools and Rest Machining

You can select any number of tools in the toolpath. With several tools in the list, the first tool removes as much as it can, and each later tool machines only areas the earlier tools could not. The tool order in the list should match the order they run on the machine, and an allowance may be left for the final tool.

Minimum Detail

Controls how small an unmachined area can be and still be ignored by a tool. Setting a higher minimum detail means the pass skips very small unmachined areas, which is useful when those areas would need an impractically small or slow tool. A lower value gives more complete coverage and a longer run time. There is also a Boundary Offset for the unmachined areas: a low value means the tool machines many smaller areas, a high value means fewer but larger areas.

Two-Toolpath Alternative

You can also make two finish toolpaths:

1. Large ball nose (e.g., 6mm) at a moderate stepover to cover most of the surface quickly
2. Small ball nose (e.g., 1.5 to 3mm) targeted only at areas the large tool couldn't reach

Set the Machining Limit Boundary on the second pass to Selected Vector(s) with vectors drawn only around the detailed areas. This can greatly reduce the time of the fine detail pass.

Critical Rule: Single Pass Only

The 3D Finish toolpath does not use the tool's Pass Depth. It runs the full surface in one pass. This means:

• If your rough pass left too much material, the finish bit will be cutting full depth in those areas, risking bit breakage or poor surface quality
• Make sure the Machining Allowance in your roughing toolpath is appropriate for your finish bit
• Preview both toolpaths together before cutting

Quality Check

Always preview the 3D finish toolpath before cutting:

• Simulate the roughing pass first, then add the finish pass
• Look for any remaining large bumps or flat areas the roughing missed
• Check the scallop pattern. If the parallel lines are too coarse, reduce the stepover
• Check edge coverage. If edges aren't smooth, increase the Boundary Offset (for raised models, at least the tool radius)
• With Raster, a diagonal angle (30 to 45°) is often less obvious on the surface than pure X or Y. Test on scrap