Fusion 360: import an SVG, scale it, export a sketch

Fusion 360, which Autodesk’s help now calls Fusion, imports an SVG with Insert, Insert SVG in the Design workspace. The drawing becomes sketch geometry on the planar face you pick, ready to extrude. Two things catch people out. Autodesk’s help lists a Scale box in the Insert SVG dialog but no setting for units, so check the size of the sketch once it is in. And the export the help documents for a sketch is DXF, not SVG.

The steps and menu names below are from Autodesk’s online help for Fusion, read in October 2026. Fusion is updated often, so a menu may have moved if you read this much later.

Insert an SVG

1. In the Design workspace, choose Insert, Insert SVG.
2. In the Insert dialog, pick the file and click Insert. The Insert SVG dialog opens.
3. In the canvas, select a planar face to hold the sketch. Autodesk’s help says “a sketch is created and the image geometry is centered on the sketch origin”.
4. Adjust the placement in the dialog, with the manipulators or by typing:

Setting	What Autodesk’s help says it does
X Distance	Positive values move the geometry to the right of the origin, negative to the left
Y Distance	Positive values move it below the origin, negative above
Z Angle	Rotates the geometry around the origin point. Positive is clockwise
Horizontal Flip	Mirrors the geometry using the Y axis
Vertical Flip	Mirrors the geometry using the X axis
Scale	Changes the scale, with the manipulator or a typed value
Control Point Frame	For splines: gives access to the control point frame so you can change the shape

5. Click OK.

Autodesk describes the result as “a fixed sketch object”, and suggests SVG “for detailed sketches such as logos, text, or PCB silkscreens”. Once it is placed you can add to it or change it with the ordinary sketch tools.

Getting the size right

The help describes Scale in the Insert SVG dialog only as a value that changes the scale. It does not ask how many millimetres the drawing should be, and the help page does not say how Fusion turns the numbers in an SVG into lengths. So do not trust the size on arrival: measure it.

Measure, then scale

1. Choose Inspect, Measure on the toolbar and click a line in the sketch whose real length you know, such as the width of a border. The dialog shows its length.
2. Work out the factor: the length you want, divided by the length you measured. If a border that should be 60 mm measures 48 mm, the factor is 60 ÷ 48 = 1.25.
3. Right-click the sketch and choose Edit Sketch.
4. On the Sketch tab, choose Modify, Scale. Select the geometry, select the point to scale from, and type the factor.
5. Click OK, and measure again to check.

The Scale box in the Insert SVG dialog can change the size at the moment of inserting, but the help does not say what its number is measured against, so measure afterwards either way.

It helps to know what size the file claims before you start. The SVG viewer shows an SVG’s width, height and viewBox, and Resize SVG sets them to an exact size in millimetres or inches. A file with a clear stated size makes the factor easy to work out, whatever a program does with it.

Or bring it in as a DXF, which has a units setting

Fusion’s other 2D import does ask about units. Insert, Insert DXF has a Units setting, described in the help as “specify the units to scale the imported DXF”.

That gives a route where the unit is stated at both ends. We have not been able to try it in Fusion, so measure one length afterwards to confirm:

1. Convert the drawing with SVG to DXF. Check the width it shows in millimetres, or type the width you want.
2. In Fusion, choose Insert, Insert DXF, select a face or plane, and pick the file.
3. Set Units to the unit the file is in, which is millimetres, and click OK. The help does not list the choices in that box.

We checked what the converter writes: for a 60 mm test drawing, the DXF’s header states millimetres ($INSUNITS 4) and gives the extents of the drawing as 1 to 59 in each direction, the true size of the artwork in millimetres.

There are two costs. A DXF from this converter holds polylines only, so every curve becomes a run of short straight lines, within 0.05 mm of the true curve unless you change the tolerance. A logo with many curves makes a sketch with many small segments. And fills are not carried, which does not matter here, because a sketch has no fills.

The gain, besides the size, is layers. With “One layer for each colour” ticked in the converter, each colour of the SVG becomes a DXF layer, and Fusion’s Insert DXF can then use One Sketch per Layer to put each on its own sketch. Its other mode, Single Sketch, puts the layers you tick into one.

What to do to the SVG first

Autodesk’s page says what the tool is for but not what it skips, so prepare the file as you would for any program that reads only outlines:

• Convert text to paths. In Inkscape, select the text and choose Path, Object to Path. Then the letters are shapes and do not depend on a font.
• Turn thick strokes into outlines if you want their width. A sketch line has no thickness. In Inkscape that is Path, Stroke to Path.
• Remove pictures. An embedded photo or PNG is not geometry. To use a picture as a tracing guide, Fusion has a separate tool, Canvas, which “places an image on a planar face or sketch plane”.
• Close the shapes you mean to extrude. The Extrude type fills closed profiles.
• Delete what you do not need, such as a background rectangle or hidden shapes. The SVG viewer counts the paths, text elements and images in a file, which is a quick way to see whether any of the above applies.

Extrude the sketch

1. On the toolbar, choose Solid, Create, Extrude.
2. Select the closed profiles to raise. To take everything at once, select the sketch itself in the Browser or Timeline: the help says this selects “all profiles and geometry in that sketch” in one step.
3. Set the distance and click OK.

The Extrude type “extrudes the entire area within selected closed profiles”. If a region will not select, its outline is probably open: look for a gap where two lines should meet.

Export a sketch as an SVG

We found no topic in Fusion’s help for saving a sketch as SVG. What it documents is DXF:

1. In the Browser, find the sketch.
2. Right-click its name and choose Export DXF.
3. Choose the unit type. The design’s active units are the default.
4. Optionally include points, projected geometry and construction geometry.
5. Click OK, name the file and save it.

Autodesk’s own tip is to “save a sketch as a DXF for use in different manufacturing methods, such as laser cutting”, and to sketch on the top or bottom face of a body when you want its outline, because the edges of the face are projected into the sketch automatically.

To get an SVG, convert that file with DXF to SVG. It reads the units from the DXF when the file states them, writes the SVG at real size in millimetres, and keeps arcs and circles as true curves. It reads ASCII DXF only and says so if a file is binary. SVG vs DXF covers when each format is the better one to hand on.

Problems

What you see	Likely cause	What to do
The sketch is not the size you expected	The help lists no units setting for Insert SVG	Measure a known length and scale by wanted ÷ measured, or insert a DXF with Units set
Lettering is missing or wrong	The SVG may hold live text, which depends on a font	Convert the text to paths and insert again
The drawing is mirrored or upside down	It was placed that way round on the face you chose	Use Horizontal Flip or Vertical Flip in the Insert SVG dialog
A region will not select for Extrude	Its outline is not closed	Close the gap in the sketch, or fix the shape in the SVG

Other ways in

A flat shape that only needs thickness does not have to be a sketch at all. SVG to STL raises the filled shapes of an SVG into a solid, and Fusion’s Insert Mesh “inserts an existing STL, OBJ, or 3MF file as a mesh body”. A mesh body is not as easy to edit as a sketch, so use this for parts you will print as they are.