Why does my toolpath say 'No toolpath generated' or fail to calculate in VCarve Pro & Aspire, and how do I fix it?

Overview

A message saying that no toolpath was generated for the current parameters (and to check that the tool can fit into the selected vectors at machining depth) is one of the most frequently seen toolpath errors in both VCarve Pro and Aspire. It almost always comes down to one of a few root causes: open vectors, a tool too large for the space, overlapping or duplicate vectors, or incorrect depth or material setup. This guide covers the known causes and their fixes. The exact wording of the message can vary with the toolpath type.

Cause 1: Open Vectors (Most Common)

Most toolpaths (V-carve, pocket, profile inside/outside) require closed vectors. If a vector has any gap, even one invisible at normal zoom, the toolpath can fail.

How to check:

• Use Edit > Select All Open Vectors. All open vectors are selected. If you see any, those are likely the problem
• Open the Vector Validator. It finds issues after file imports that stop toolpath creation, such as overlapping contours, intersections and zero-length spans. With nothing selected it checks all visible vectors on the current side of the current sheet

How to fix:

1. Zoom into each open endpoint. You will often see a tiny gap or two nodes that should be touching but aren't
2. Use Join Vectors (Edit menu). The form joins open vectors whose endpoints are within the tolerance you set
3. Alternatively, in Node Edit mode (N), drag the open endpoint onto the matching node
4. Use the close vector options to close a vector by force

The invisible gap trap: Vectors imported from DXF, SVG, or traced bitmaps often have gaps of 0.001" or less. They look closed at normal zoom but aren't. Zoom in a long way when cleaning up imported files.

Cause 2: Tool Too Large to Fit Between Vectors

If the gap between your vectors is narrower than the selected tool's diameter, the tool can't physically fit and no toolpath is calculated.

Example: Vectors define a 0.1" wide channel. You selected a 0.25" end mill. The tool is 2.5 times wider than the channel, so no toolpath is generated.

How to fix:

• Select a smaller diameter tool
• Widen the design channel
• Use a V-bit, which can reach into narrow spaces via its angled geometry

V-carve specific: For V-carve toolpaths, the bit's tip must fit into the narrowest point of the design. If your design has features narrower than the V-bit tip diameter, those areas won't be carved.

Cause 3: Duplicate/Overlapping Vectors

A common problem with imported files: two identical vectors sitting exactly on top of each other. The software sees them as a self-intersecting shape and may not toolpath it.

How to detect: Run the Vector Validator, which flags overlapping contours. Another quick test: click the vector and press Delete. If the line is STILL there, you deleted the top copy and there is another underneath.

Fix:

1. Click the visible vector and delete it
2. The underlying duplicate is now the only one. Check it with the Vector Validator
3. Or zoom in and use Node Edit to confirm the endpoints are single nodes, not stacked

Common source: CorelDRAW exports, Illustrator exports, and SketchUp imports frequently produce duplicate stacked vectors.

Cause 4: Clearance Tool Can't Fit Anywhere

When using a V-carve toolpath with a clearance tool (a flat-bottom end mill to clear the center of wide areas), an "empty toolpath" result for the clearance tool means the end mill can't fit anywhere between your vectors at the specified depth.

Fix:

• Try a smaller clearance tool
• Increase the flat depth slightly so the clearance area is wider
• Remove the clearance tool entirely if the design doesn't have wide flat-bottomed areas

Cause 5: Vectors Outside the Material Boundary

If vectors extend outside the job boundary, the toolpath may not cover those sections as you expect.

Fix: Select all vectors and use the Align tools to make sure everything is within the job boundary. Check that the job size matches your design size.

Cause 6: Incorrect Start Depth

For toolpaths with a Start Depth specified (for example carving into a pocket bottom), if Start Depth + Cut Depth exceeds the material thickness, the toolpath may fail or produce unexpected results.

Fix: Verify that Start Depth + Cut Depth is not more than the Material Thickness in Material Setup.

Cause 7: Self-Intersecting Vectors

Vectors that cross themselves (figure-8 shapes, loops in traces) can stop the toolpath from calculating.

Fix: The Vector Validator flags intersections. Fix them in Node Edit mode by deleting the crossing spans and rejoining.

The Systematic Fix Workflow

When a toolpath fails to calculate, run through this checklist in order:

1. Edit > Select All Open Vectors: is anything selected? Fix it with Join Vectors.
2. Vector Validator: are any errors listed? Fix each one.
3. Zoom into corners and endpoints a long way, looking for micro-gaps and overlapping nodes.
4. Check tool diameter vs. the narrowest vector gap: does the tool physically fit?
5. Test for duplicates: click, delete, and see if the vector is still there.
6. Check Start Depth: is it too deep for the material thickness?
7. Fit Curves to Vectors on traced or imported data to clean up faceted polylines.