Exporting DXF and SVG

Overview#

Most small-shop 2D fabrication runs on vector files. A laser cutter's software, a vinyl cutter's driver, an online cutting service and a CNC router's CAM program all accept DXF, and many accept SVG as well. Fusion can produce these from sketches, from sheet metal flat patterns and from drawing sheets. The export is easy; making the file arrive at the machine at the correct scale, with closed contours and no junk, is where people lose material.

This page covers the main export routes, how to prepare a sketch so the file is clean, what each format carries, and a checklist for checking the file before you cut. The sheet metal route is covered in more depth in the sheet metal section and on the next page.

Where to find it#

Autodesk's help says that to laser cut the profile of a body you create a sketch on its top or bottom face, and the face edges are automatically projected into the sketch. Otherwise project edges or faces into the sketch with P.

Note: not confirmed in Autodesk's documentation: an SVG export command. The help covers Insert > Insert SVG (import) and DXF export only. For SVG output, convert the DXF in Inkscape, LightBurn or the target software, or look for an add-in. Likewise, the help does not describe exporting a planar face directly to DXF or a File > Export DXF route; use the sketch route.

Step by step#

Export a clean sketch to DXF#

1. Create a dedicated export sketch. In the Browser right-click a component and choose New Sketch on the plane or face that holds your part. Using a separate sketch avoids exporting construction lines and unrelated geometry.
2. Project geometry. Use Project/Include, Project (P), and select the faces or edges you want. For a solid, select the planar face; the outline plus holes project as sketch curves. Linked projected geometry stays associative with the model.
3. Clean up. Convert helper lines to Construction (X), delete stray points and zero-length lines, and remove overlapping duplicates. Construction and projected geometry are exported only if ticked in the Export DXF dialog, so leave them unticked and inspect the DXF.
4. Confirm closed contours. Click inside each region and check that a profile highlights (Fusion shades closed profiles). A contour with a gap, even 0.001 mm, will not close, and laser software may refuse to treat it as a shape or may cut it with an out-of-order pass.
5. Orient and place. Make sure the sketch is on the XY plane or properly oriented. Some DXF exports behave best with sketches on the XY plane; sources report issues with rotated sketches, so if the output appears rotated, create the sketch on the XY plane (in a new component) and re-project, or use Sketch Plane/Move.
6. Set units. In Design, check the document units (Modify, Change Parameters shows the units, or Document Settings, Units). Millimeters are the usual choice for laser software.
7. Export. Right-click the sketch in the Browser and choose Export DXF. In the Export DXF settings dialog pick the unit (default is the design's active unit) and tick any extra visible geometry you want: Points, Projected Geometry, Construction Geometry. Click OK, name the file and save (optionally to a Fusion project).
8. Verify. Open the DXF in your machine software or a viewer (LibreCAD, Inkscape, QCAD, the shop's online uploader). Measure a known dimension. Check the shape count and open contours.

Export multiple parts in one file#

1. Place each part's flat outline in a single export sketch, positioned with spacing between them. Do this manually, via Move/Copy, or use Nest (later page).
2. Leave at least 2 times the kerf or tool diameter between parts, and more for plasma and waterjet.
3. Name the sketch with the project and version, for example box_v3_parts.

Import SVG and artwork for use as outlines#

1. Choose Insert > Insert SVG in the Design workspace, pick the file and select a planar face. The geometry is centered on the sketch origin; X Distance, Y Distance, Z Angle, flips and Scale are set in the dialog.
2. Check the scale. SVG pixel-to-unit scaling can differ between tools (general guidance); verify one known dimension with the Scale option.
3. Clean the imported spline curves. Complex traced SVG art can create hundreds of fit points, which slows Fusion and the machine. Simplify in a vector editor first.
4. Fusion's sketches can then be exported as DXF (see above) for the cutter.

Layers and colors#

Laser software often assigns cut and engrave operations by layer or color. Autodesk documents layer assignment only for flat pattern export (outer profiles, interior profiles, bend center lines, bend extent lines and text each go to a different layer); sketch export has no documented layer controls. Good practice: export cut contours and engrave geometry as separate DXF files, or import into LightBurn/Inkscape and assign operations there. The Fusion Manufacture workspace is not the place to define raster engraving. Check the LibreCAD or machine software to see the layer names that arrived.

Options reference#

File format notes#

DXF. The universal exchange format between CAD and CAM. Contains lines, arcs, circles, splines, polylines, text and layers. Supports units in the header, but many readers ignore them. Fusion writes ASCII DXF compatible with common software. Pitfalls: splines can be unsupported in very old controllers, text is converted differently in each tool, and arcs may be broken into line segments (faceted curves) when an app prefers polylines.

DWG. Autodesk's native CAD format, available from drawings. Less common for lasers. Use DXF for fabrication.

SVG. XML vector graphic. Sizes may be in pixels or user units; scale can silently differ (for example 72 versus 96 dpi). Supported by vinyl cutter apps, Inkscape, Illustrator and LightBurn. Contains strokes and fills; cut machines care about stroke vs fill and line color.

PDF. Sometimes used for printing templates or for cutters that accept PDF paths. Export drawings with the Drawing workspace's PDF command; see section 10.

STEP/IGES/STL. 3D formats, not used for 2D cutting except for routers that read 3D.

Tips and pitfalls#

Tip: Draw a 100 mm reference line or square as a separate item in your DXF during first-time tests. Delete it for production. It saves wasted material when units misbehave.

Tip: Cut order matters. Lasers should cut inner holes first and the outer contour last. Many laser programs reorder paths; if yours does not, split inner and outer shapes into layers.

Tip: Online cutting services have their own rules: minimum hole diameter, minimum web width, preferred layer names, no text or splines. Read their DXF checklist before exporting.

Warning: Overlapping or duplicate lines are cut twice, which burns edges and can ruin thin material. Use "remove duplicates" in your laser software or clean the sketch. Shared edges between neighboring parts (common line cutting) are only intentional when you designed them that way.

Warning: DXF scale mistakes are common. Check the unit chosen in the Export DXF dialog and always verify a measurement.

Warning: Do not export text without converting it. Fonts may not match on the other machine. Use Text with explode/convert to curves where available, or use a stencil font whose curves are part of a sketch.

Practice exercise#

Open a model with a mounting plate (a rectangle with four holes and one slot). Create a new sketch on its top face, project the face, and verify that all four holes, the slot and the outer boundary are closed profiles. Add a 100 mm construction line and confirm it is not exported. Export DXF. Open the DXF in LibreCAD or Inkscape and check: outline 100 mm by the expected length, holes present, no extra lines. Expected result: a DXF with six closed contours (one outer, four holes, one slot), measured within 0.01 mm of the model.

Related#

• Sheet metal flat pattern for cutting
• 2D Fabrication Processes Overview
• Flat Pattern and DXF Export (section 08)
• Exporting PDF, DWG and DXF (section 10)