How does the Profile Toolpath work in VCarve Pro & Aspire: tabs, ramps, lead-in/out, last pass, and all advanced options?

Overview

The Profile Toolpath cuts along the edge of a vector, either on the vector, inside it, or outside it. It is the most-used toolpath: cutouts, part perimeters, cutting dados and slots, and any operation requiring precise edge cuts. The Profile options section of the form has five pages (Ramps, Leads, Order, Start At and Corners) that control edge quality and cutting order. Tabs, Allowance and Separate Last Pass are separate sections of the form.

---

Step-by-Step

1. Select your vector(s)
2. Open the 2D Profile Toolpath form from the Toolpaths tab
3. Choose Outside, Inside, or On
4. Set Start Depth (usually 0.0) and Cut Depth (depth relative to the Start Depth)
5. Pick your tool (see Tool choice below)
6. Check Add tabs to toolpath if the part will be cut free (see Tabs)
7. Optionally enable Ramps and Do Separate Last Pass
8. Calculate

---

Cut Position: Outside / Inside / On Vector

• Outside: Tool cuts around the outside of the vector, offsetting by the tool radius. Used for cutting parts free from stock.
• Inside: Tool cuts around the inside of the vector, offsetting inward by the tool radius. Used for pockets, holes, and recesses.
• On: Tool center runs directly on the vector line. Used for engraving, scoring, or when the vector represents the tool center path.

For nested vectors (like the letter O), the software automatically determines which side to cut and always cuts inner vectors before outer ones.

For open vectors, the options become Left, Right, or On.

Direction: Conventional or Climb. The best choice depends largely on the material and the tooling.

---

Tool Choice

These are shop-practice guidelines, not software settings. A down-cut spiral leaves the cleanest top face (useful for the visible face of a hardwood part). An up-cut spiral leaves a cleaner bottom edge and clears chips better. A compression bit gives a clean edge on both faces. Test on scrap.

---

Tabs (Bridges)

Tabs hold parts to the sheet while the final passes cut through. Without tabs, parts can shift, catch, or fly off the machine. Tabs work on open and closed vectors.

Setting tabs up: Check Add tabs to toolpath and set the tab Length and Thickness in the toolpath form. Tab thickness is measured from the bottom of the cut depth, not the bottom of the material. Click Edit Tabs to open the tab placement dialog:

• Add Tabs places them automatically, either a Constant number (spread evenly) or a Constant distance between tabs. The first tab can sit at the machining start point, or the Avoid corners and curved regions option can be used
• Or add tabs interactively: click the vector to add a tab, click a tab to delete it, drag a tab to move it, or use Delete All Tabs

2D Tabs: The tool stops at each tab position, lifts vertically by the Tab Thickness, travels across the tab length, then plunges back down. Creates a flat-topped bridge.

3D Tabs: Check Create 3D Tabs. The tool ramps up to the Tab Thickness and back down in a triangular wedge, with no stop to move in Z. The machine often runs quicker and smoother through 3D tabs.

Tab sizing for wood (starting point, test on scrap): Thickness about 1/4 to 1/3 of the material thickness; Length about 0.4" to 0.6" (10 to 15mm). Use at least two tabs per part, more for large or heavy pieces.

---

Ramps

Ramps prevent the cutter from plunging vertically into the material, which reduces heat, vibration, and tool wear. When multiple passes are needed, the ramp is applied at the start of each level. Ramp moves run at the tool's plunge rate.

Smooth Ramp: Gradual ramp into the material using a Distance or an Angle.

Zig-Zag Ramp: The tool ramps down and back in a zig-zag pattern. The Angle option suits cutters that cannot plunge vertically and have an entry angle specified by the manufacturer.

Spiral Ramp: The tool spirals down over the complete circumference of the profile pass. Only available when no Lead In moves are set. A 0.5" deep cut with a tool Pass Depth of 0.5" or more is one spiral pass. With a Pass Depth of 0.25", two spiral passes are made.

Ramp on Lead In: When a Lead In distance is set, this option limits the ramp moves to the lead-in portion of the toolpath.

---

Lead-In / Lead-Out

Lead moves bring the tool onto the profile edge at an angle or along an arc instead of plunging vertically on the edge. This helps prevent the dwell mark, the small mark left where the tool plunges.

Straight Line Lead: A linear lead using an Angle and a Lead length.

Circular Lead: An arc lead using a Radius and Lead length, tangent to the vector where it meets the edge.

Do lead out: Adds an exit lead at the end of the toolpath.

Overcut Distance: Forces the tool to travel past the start point by the specified amount, often used to improve edge quality at the join.

---

Separate Last Pass (Last Pass Allowance)

Adds a final light cleanup pass after all the depth passes.

How it works: All passes except the last are undercut by the last pass Allowance, leaving a thin skin of material. The final pass cuts to size. The last pass allowance also takes any Allowance offset into account, so the two can be used together.

Notes from the official documentation:

• The skin should be thin. The software warns if the last pass allowance is more than 1/3 of the tool diameter, and ideally keeps it a lot smaller
• Keeping it small also stops the final pass from fitting in areas the earlier passes could not reach
• The toolpath fails to calculate if the last pass must cut a significant distance into uncleared material
• A Reverse direction option reverses the cutting direction of the last pass, which can reduce witness marks on the edge

Starting point to test: many users try 0.005" to 0.010" for hardwood, MDF, and acrylic where edge quality matters.

---

Order

Controls the order profiles are cut when multiple vectors are selected. You can pick several options, and the software calculates each and uses the one with the shortest machining time.

• Vector Selection Order: Cuts in the order you selected the vectors (inner vectors are still cut before outer ones)
• Left to Right / Bottom to Top: Machines progressively across the sheet
• Grid: Joins parts within a section of a grid before moving on

---

Start At and Corners

Start At: Keep Current Start Points, Optimize Start Points, or Closest on Bounding Box. Use Vector Start Point forces the plunge at the vector's first point, for example a corner where a dwell mark will not show.

Corners: Sharp External Corner sharpens outside corners of the cut. Sharp Internal Corner (3D) runs a V-bit tip up the inside corner.

---

Allowance (Over/Undercut)

Adds or removes a fixed distance from the profile offset:

• Positive allowance: Undercut, leaves more material (part slightly oversized)
• Negative allowance: Overcut, removes extra material (part slightly undersized)
• If the Allowance is 0, the toolpath machines to the exact size

Used for fitting lid tolerances for boxes, compensating for tool deflection, or deliberately adjusting part dimensions.