How does the 3D Roughing toolpath work: Z Level vs 3D Raster, machining allowance, and boundary options?

Overview

The 3D Roughing Toolpath removes the bulk of unwanted material from around a 3D model before the finishing pass, when the part is too deep for the finishing tool to cut in a single pass. It uses a large end mill at aggressive settings to cut away stock efficiently. Without roughing, the finish tool (usually a ball nose) would have to remove all that material itself, at very slow speeds and with a risk of breakage. It is available in both VCarve Pro and Aspire.

Two Roughing Strategies

Z Level Roughing (most common)

Uses a series of 2D pocket-like passes that take the 3D model into account and hog out the material around it within the specified boundary. It cuts horizontally at each depth before stepping down to the next level, like slicing an onion layer by layer. For deeper parts it is typically more efficient than 3D Raster.

Best for:

• Deep models (multiple pass depths required)
• Faster overall machining time on deeper parts

Settings:

• Raster direction (Along X or Along Y): the main cutting direction of the fill pattern on each level
• Profile: First (profile cut before the raster on each level), Last (profile after the raster), or None (raster only). The choice depends on the material and tooling. More brittle material may benefit from Profile First to reduce chipping
• Order: Level by level (the default) makes a complete pass at a given depth over the whole model before moving down. Depth-first is the alternative: if the model has separate regions at a given depth, all passes at increasing depths are made over one region before moving to the next
• Reverse step direction: By default, with raster direction Along X the tool steps from one raster line to the next from bottom to top, and with Along Y from right to left. This option reverses that. In 12.5 it is only available for the Z Level strategy

3D Raster Roughing

A 3D cut that passes over the whole model. It leaves a more even amount of material for the finish cut to remove, but depending on the depth and style of the part it may take significantly longer to run.

Best for:

• Shallow models (roughing takes only one or two passes)
• Models where an even amount of stock for the finish tool matters more than raw speed

Settings:

• Raster direction: Along X or Along Y

Avoid Machined Areas

If checked, an area machined by an earlier pass of the toolpath is not machined again by later passes. It may be quicker, but that is not guaranteed: extra retracts and extra acceleration and deceleration can make it slower. Compare the results on your job.

Machining Limit Boundary

Options:

• Model Boundary: The combined boundaries of all components in the job (not just the selected models). The tool tip, rather than the cutting side, will not leave the boundary, so roughing removes enough material at the boundary
• Material Boundary: The whole material block
• Selected Vector(s): Use with Create Vector Boundary from Selected Components for precise control
• Selected Level: The combined boundaries of all components on a named level

Boundary Offset: Enlarges the machining boundary by a specified amount. Useful for raised models, where the tool often will not fully machine down the edge. A value of at least the tool radius is a sensible starting point.

Machining Allowance

The Machining Allowance is a virtual thickness added to the 3D model when the roughing toolpath is calculated, so some extra material is left on the roughed part. The finish tool then removes this final layer.

Why it matters:

1. Roughing uses relatively large tools and aggressive cuts and is prone to chipping depending on the material. The skin helps prevent chipping from affecting the finished surface
2. Most tools cut best when they are constantly removing material, so the allowance makes sure the finishing toolpath always has some material to remove
3. Size the allowance to what the finish tool can handle. Starting point to test: 0.5mm to 1.5mm (0.02" to 0.06")

Critical warning: The 3D Finish toolpath makes a single pass and does not use Pass Depth. If the roughing allowance is too large (for example 3mm) but the finish tool can only safely cut 1mm, the finish tool is asked to cut 3mm in one pass, risking breakage.

Ramp Plunge Moves

When enabled, the cutter ramps over a distance into the pocket instead of plunging vertically. This reduces heat build-up that damages the cutter and also reduces the load on the spindle and Z axis bearings. It is a good idea for harder materials.

Tool Selection for Roughing

• Use the largest end mill that fits the tightest area of the model
• Typical: a 1/2" or 1/4" end mill for roughing, then a 1/8" ball nose for finishing
• If the model has areas too narrow for the roughing tool, those areas remain un-roughed and the finish tool must remove all the material there. Always check the toolpath preview for missed areas