How do I set feed rate and plunge rate for 3D toolpaths in VCarve Pro & Aspire, and when should plunge rate match feed rate for 3D finishing?

Overview

One of the most important and frequently misunderstood settings for 3D toolpaths is the relationship between feed rate and plunge rate. Unlike 2D toolpaths where the tool moves primarily in XY and plunges only at the start, 3D finishing toolpaths are constantly moving in all three axes simultaneously. This changes how plunge rate should be set. This applies to both VCarve Pro and Aspire.

Why 3D Toolpaths Are Different

In a 2D pocket or profile toolpath:

• The tool plunges straight down at the start (pure Z movement)
• Then moves in XY at the programmed feed rate
• Plunge rate mostly applies to the straight-down entry move (and to ramp moves, which run at the tool's plunge rate)

In a 3D raster or offset finishing toolpath:

• The tool is always moving in X, Y, and Z simultaneously
• Every pass up and over a peak or into a valley involves Z movement combined with XY movement
• There is no "straight plunge". It is all compound angled moves

Setting Plunge Rate for 3D Finishing

The official documentation describes the plunge rate as the cutting rate at which the cutter moves vertically into the material or during ramping moves. Many users therefore set Plunge Rate = Feed Rate for the ball nose or tapered ball nose tools used in 3D finishing. If the plunge rate is much lower than the feed rate (for example feed rate = 100 ipm, plunge rate = 30 ipm), the moves that descend into the material can run at the slower rate, and the finishing toolpath can take far longer (for example 2.5 hours instead of 45 minutes) with no quality benefit.

How much this affects a job depends on your post-processor and controller, so check the time estimate and test on scrap.

Practice: In the Tool Database and in each toolpath form, set the plunge rate equal to the feed rate for tools used in 3D finishing.

Note: This is not a concern for the 3D Roughing toolpath, which does have true plunge moves at depth changes. For roughing, keep the plunge rate at a conservative value appropriate for your material.

Feed Rate Guidelines for 3D Finishing

General starting points (adjust for material and machine rigidity):

Always test on scrap and adjust. A 1/8" ball nose in hard maple at 150 ipm will likely chatter. Slow down to 80 to 100 ipm for better finish quality.

Stepover vs. Feed Rate Trade-off

For 3D finishing quality, the key variables are:

1. Stepover: smaller stepover = smoother surface = longer machining time
2. Feed rate: faster = shorter time but potentially rougher cuts at high speed
3. Tool diameter: a larger ball nose gives a wider stepover for the same cusp height, so faster machining

The finishing toolpath is always a single pass. It does not use the tool's Pass Depth setting, and the entire model is finished in one pass. Make sure your roughing allowance leaves enough stock that the finishing pass is removing material, not just re-tracing rough cuts.

Toolpath Preview Simulation Quality

For checking 3D finish quality before machining:

• Set the simulation quality to Maximum in the toolpath preview to reduce pixelation in the preview render. Higher quality is slower to compute
• Lower quality settings can show scallop marks that won't exist in the actual cut. Check at a high quality setting before judging a toolpath's finish quality
• The built-in preview simulation is a good guide to the machined result, but always test on scrap for critical work