SheetCAM reports open paths? Your DXF endpoints do not meet.

The file looks fine on screen, but SheetCAM will not build the cut path, VCarve complains about open vectors, or the torch runs straight down the drawn line with no kerf compensation. Three different symptoms, one cause: contours that do not quite close.

Why CAM is stricter than your drawing program

A drawing program only has to display the geometry, and an open shape displays fine. CAM has to answer a harder question: where does the torch or cutter actually travel? Kerf compensation on a plasma table and tool radius compensation on a router both shift the programmed path to one side of the contour, and "one side" only exists when the contour has an inside and an outside. An open path has neither, so the offset is mathematically undefined. Some programs refuse and name the problem. Others quietly fall back to cutting on the line, and you only find out when the part measures wrong. The worst ones skip the profile entirely and leave you a sheet with a missing part.

Where the gaps come from

The usual three suspects are drawing without object snap, so segments never met exactly in the first place; floating point rounding when the CAD writes the file; and exploded polylines that fall apart into loose lines and arcs. Plasma files add a fourth: exploded splines. When an exporter flattens a spline into line segments with a loose tolerance, neighbouring segments can end short of each other, and one smooth curve turns into dozens of micro-gaps. That is why a file can have far more open paths than it has shapes.

None of this is visible at working zoom. A gap of 0.05 mm on a 1200 mm sheet is a pixel you will never see, but the toolpath engine sees it every time.

Fixes, tool by tool

SheetCAM

SheetCAM has an import tolerance in its DXF import options: endpoints closer together than that distance get snapped into one when the file loads. If parts still come in open after raising it, the gaps are bigger than a snapping tolerance should be, and the honest fix moves upstream. The standing advice on the plasma forums is blunt: learn to use object snaps in your CAD, because a gap you never draw is a gap you never have to close.

VCarve and Aspire

Use Edit Vectors, then Join Open Vectors with a tolerance, to merge endpoints within the threshold. Vectric's Vector Validator is worth running on incoming customer files anyway: it flags open vectors before you waste time setting up toolpaths that will fail.

QCAD, the free route

Delete zero-length entities first, then run "Polyline from segments" with a tolerance of 0.1 to rebuild closed polylines from the loose pieces. Two minutes, and it works on files that arrive as thousands of disconnected segments.

Fix the file once, not in every program

Import tolerances patch the symptom inside one program. The gaps stay in the file. If the same DXF goes to SheetCAM today, VCarve next week and FireControl on someone else's table, each import starts the hunt again. Repairing the file once, or re-exporting it cleanly with snaps enabled, gives every downstream tool a closed contour. That matters most with customer files: send back a repaired DXF and the back-and-forth ends. The laser-side view of the same problem, with the LightBurn workflow, is in the open contours guide.