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PDF to Fusion 360: Get a PDF Drawing Into a Sketch at the Right Size

Updated 30 October 2026

Bringing a PDF to Fusion 360 works through one of two doors: convert the PDF to DXF and use Insert > Insert DXF, or export the page as an image and trace it on a calibrated canvas. Fusion 360 has no PDF vector import, so a direct File > Open on a PDF goes nowhere.

The DXF method gives you real sketch lines you can extrude in minutes. The canvas method gives you a picture to draw over. Here is when to use each, how to keep the scale right, and how the same job works in SolidWorks.

Can Fusion 360 import a PDF?

Only through a converted file or an image. This table shows what each option produces:

Starting point Fusion 360 tool Result
Vector PDF, converted to DXF Insert > Insert DXF Editable sketch lines, one sketch or one per layer
Any PDF, exported as PNG or JPG Insert > Canvas A reference image you calibrate and trace
Vector PDF, converted to SVG Insert > Insert SVG Sketch curves, at paper size
Scanned PDF, traced to DXF Insert > Insert DXF Ink outlines of every drawn line

To tell which PDF you have, zoom to 1,600% in a PDF viewer. Lines that stay sharp are vector; blocky pixels mean a scan.

How do you bring a PDF into Fusion 360 as a sketch?

This is the method for any vector drawing: brackets, flat patterns, enclosures, signs.

  1. Open the free PDF to DXF converter and drop in the PDF. It runs in the browser without uploading the file; one PDF up to 5 pages and 20 MB is free.
  2. Use Set scale: click both ends of a printed dimension, such as the 180 mm length of a bracket, and type 180. A drawing printed at 1:2 or 2:1 comes out at true size.
  3. Download the DXF. It is DXF R12, with one layer per PDF colour, text as TEXT and curves as polylines.
  4. In Fusion 360’s Design workspace, choose Insert > Insert DXF.
  5. Select a plane or planar face. The DXF origin lands on the sketch origin.
  6. Pick the file and set Units to Millimeter (or Inch for an imperial drawing).
  7. Under Insert Mode, choose One Sketch per Layer when the PDF used colours for meaning (cut lines, bend lines, dimensions). Choose Single Sketch for a simple outline.
  8. Untick the layers you do not want, such as hatching or the title block, then click OK.

When the DXF carries no unit information, Fusion falls back to the design’s units. So ALWAYS set the Units field yourself instead of trusting the default.

Why do profiles fail to close?

Fusion 360 shades closed areas as profiles, and only profiles can be extruded. If a shape you expected to fill stays empty, one of these is the cause:

  • A gap at a corner. PDF lines can stop 0.01 mm short of each other. Zoom in, drag the endpoint onto its neighbour, and the profile fills.
  • Duplicate lines. Two identical lines on top of each other split or confuse profiles. Window-select the edge, check the selection count, and delete the extra copy.
  • Hatching and text. Short hatch lines and outlined letters cut a profile into hundreds of tiny pieces. Put them on their own layer and leave that layer out in step 8.
  • Too many segments. Curves arrive as polylines, so a 30 mm hole arrives as dozens of short lines. Fusion handles that, and the sketch slows down noticeably once it holds thousands of segments. For a part you will keep editing, redraw holes as circles and add dimensions.

Check scale before you extrude anything. Measure the longest known dimension with Inspect > Measure. If the 180 mm bracket reads 90 mm, the drawing was printed at 1:2 and the scale step was skipped. The causes are in why a converted PDF is not to scale.

How do you trace a scanned PDF on a canvas?

A scanned drawing holds pixels only, so the job is tracing. Fusion’s canvas accepts PNG, JPG and TIFF, so export the PDF page as an image first.

  1. Export the page as a PNG at 300 dpi from your PDF viewer.
  2. Choose Insert > Canvas (older builds call it Attached Canvas), pick the image and select the face or plane to place it on.
  3. In the Browser, expand Canvases, right-click the image and choose Calibrate.
  4. Click two points of a known dimension, type the real distance and press Enter.
  5. Start a sketch on the same plane and draw over the image with lines, arcs and circles.

Two honest warnings. Calibrate has no snapping, so you are clicking on pixels by eye. And at 300 dpi one pixel is 0.085 mm on paper, which on a drawing printed at 1:5 means 0.42 mm on the real part. Calibrate across the longest dimension available, use printed dimensions for every toleranced feature, and treat the canvas as a shape guide only.

For a scan with lots of linework, the converter can trace the page into ink outlines: each pen stroke becomes a thin closed shape following both edges of the line. Insert that DXF and you get endpoints to snap to, then draw clean centre-line geometry on top. Scan settings and redrawing tips are in how to convert a scanned drawing to CAD.

How accurate is a converted PDF for CNC and laser work?

For a vector PDF exported straight from CAD, the converted coordinates match the original drawing closely, and Set scale removes the paper scale. Three things still deserve a check before you send a part to the machine:

  • Overall dimensions against the numbers printed on the drawing. A 0.5% error on a 600 mm panel is 3 mm.
  • Hole positions against their dimensions, because PDF exports round coordinates.
  • Closed profiles for every cut path, since an open contour makes CAM toolpaths fail or leave tabs.

The machine side of this, with kerf, tolerances and joining polylines, is in PDF to DXF for CNC.

How do you do the same in SolidWorks?

SolidWorks has no PDF vector import either, and it handles DXF well through the DXF/DWG Import wizard.

  1. Convert the PDF to DXF as above, with Set scale.
  2. In SolidWorks, choose File > Open, set the file type to DXF, and open the file. The import wizard starts.
  3. Pick Import to a new part as, then 2D sketch, to get sketch geometry you can extrude. Pick Create new SOLIDWORKS drawing if you only need the 2D drawing.
  4. On the document settings page, set the units of the imported data to match the DXF, such as millimetres.
  5. Finish, then run Repair Sketch if the wizard reports gaps or overlaps.

For scanned drawings, SolidWorks has Sketch Picture (Tools > Sketch Tools > Sketch Picture), which places an image in a sketch so you can scale it and trace over it, the same idea as a Fusion canvas.

Next steps: convert one page with Set scale, insert it with millimetre units, and measure the longest edge. If it matches the print, extrude.

Questions people ask

Can Fusion 360 import a PDF?

Fusion 360 has no PDF vector import. Convert the PDF to DXF and use Insert > Insert DXF for editable sketch geometry, or export the page as an image and place it as a canvas to trace over.

Why is my inserted DXF the wrong size in Fusion 360?

The Units setting in the Insert DXF dialog decides the size, and a PDF converted without a scale step stays at paper size. Set the real scale during conversion, pick the matching unit, and check one long dimension after inserting.

Why won't Fusion 360 extrude my imported sketch?

Extrude needs closed profiles. Gaps, duplicate lines and leftover hatching or text break them, so delete extra layers and close any open corners before extruding.

Does SolidWorks import PDF drawings?

SolidWorks has no PDF vector import either. Convert the PDF to DXF, open it with File > Open, and use the DXF/DWG Import wizard to bring it in as a 2D sketch in a new part or as a drawing.

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