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How to Import a PDF Into FreeCAD and Get Usable Geometry

Updated 30 October 2026

You cannot import a PDF into FreeCAD as editable geometry in one click, because FreeCAD has no built-in PDF vector importer. It reads DXF and SVG very well, and it can place an image on a plane and calibrate it. So every working method starts by turning the PDF into one of those three things.

Pick the right one and you get closed wires you can pad into a part. Pick the wrong one and you get 4,000 loose line segments at paper scale. Here is how to tell them apart.

Which method fits your PDF?

Start with one question: does the PDF hold real vector lines, or is it a scan? Zoom to 1,600% in a PDF viewer. Sharp lines mean vector; blocky grey pixels mean scanned.

Your PDF Best method What you get in FreeCAD
Vector drawing from CAD PDF to DXF, then File > Import Lines, arcs as polylines, layers, text
Vector logo or outline Inkscape to plain SVG, then “SVG as geometry” Paths as wires, at paper size
Scanned drawing Export page as PNG, import as image plane, calibrate A scaled picture to sketch over
Scanned drawing, many shapes Trace to DXF first, then import Ink outlines of every line

How do you import a PDF into FreeCAD through DXF?

This is the cleanest method for mechanical and architectural drawings, because the DXF can come out at real size instead of paper size.

  1. Open the PDF to DXF converter. It works in your browser and the PDF is never uploaded; one file up to 5 pages and 20 MB is free.
  2. Use Set scale: click both ends of a dimension printed on the drawing (say the 120 mm overall width of a bracket) and type 120. Everything else scales with it.
  3. Download the DXF. It is DXF R12, with one layer per PDF colour, text as TEXT and curves as polylines.
  4. In FreeCAD, choose File > Import and pick the DXF.

Before step 4, open Edit > Preferences > Import-Export > DXF once. Two settings matter here:

  • The scale factor. FreeCAD treats each DXF unit as one millimetre. If your DXF is in inches, set the factor to 25.4. If it is already in millimetres, leave it at 1.
  • The importer. The default C++ importer is fast. The older Python importer offers extra options such as Join geometry, which merges touching segments into wires on import, and it needs its support files downloaded, which the same preferences page lets FreeCAD do for you.

Why does a drawing at 1:2 come in half size?

Because the PDF stores the printed picture. A bracket drawn at 1:2 on an A4 sheet is half its real size on paper, and without a scale step the DXF keeps that. Measure one known dimension in FreeCAD (the Measure tools or a Draft Dimension show it), and if 120 mm reads as 60 mm, either redo the conversion with Set scale or apply the Draft Scale tool with a factor of 2. The causes are covered in why a converted PDF is not to scale.

How do you turn imported lines into a sketch you can pad?

Imported DXF geometry arrives as separate Draft or Part objects. To make a solid, those segments need to become closed wires, then a sketch.

  1. Switch to the Draft workbench and select the segments of one outline.
  2. Run Draft Upgrade. Touching segments join into a wire; run it again on a closed wire and it becomes a face.
  3. Run Draft to Sketch to convert the wire into a Sketcher sketch.
  4. Open the sketch and use Validate sketch to find missing coincidences and open ends. A gap of 0.001 mm is enough to stop a Pad.
  5. In PartDesign, attach the sketch to a Body and Pad it to the plate thickness, such as 6 mm.

One honest limit: the converter writes arcs as polylines, so a 20 mm hole arrives as a ring of short straight segments. That pads fine for a laser or CNC profile. For a parametric model you will edit later, redraw holes and fillets as true circles and arcs in the sketch, then add constraints. Ten minutes of redrawing saves an hour of fighting a sketch with 600 unconstrained vertices.

Text from the PDF arrives as text objects. You cannot pad those directly, so for engraved lettering rebuild it with Draft ShapeString.

How does the SVG method compare?

Inkscape opens a PDF page as editable paths, and FreeCAD imports SVG. The steps:

  1. Open the PDF in Inkscape and pick the page.
  2. Ungroup everything and convert text with Path > Object to Path.
  3. Save as Plain SVG.
  4. In FreeCAD, use File > Import and choose SVG as geometry (importSVG) when asked.

This works well for logos, gaskets and sign lettering. It has two drawbacks for technical drawings: you lose the layer-per-colour split that DXF gives you, and the result arrives at paper size, so a 1:5 drawing needs a scale factor of 5 afterwards. Hatching also comes through as thousands of tiny paths, so delete it in Inkscape before saving.

How do you trace a scanned drawing in FreeCAD?

A scan holds pixels and nothing else, so the job becomes tracing. Current FreeCAD releases handle this well:

  1. Export the scanned page as a PNG at 300 dpi (600 dpi for small parts).
  2. Use File > Import and pick the PNG. FreeCAD places it on the XY plane as an image plane.
  3. Double-click it in the tree to open Image Plane Settings, press Calibrate, click two points of a known dimension and type the real length.
  4. Give the image a small negative offset, such as -0.1 mm, so your sketch lines sit above it instead of fighting it.
  5. Sketch over the image in Sketcher, using the image only as a guide.

Expect limits. At 300 dpi one pixel is 0.085 mm on paper; on a 1:5 drawing that is 0.42 mm on the real part. Use printed dimensions for anything with a tolerance, and the scan only for shape and layout.

For drawings with dozens of shapes, the scanned PDF to CAD mode traces every line into an ink outline, both edges of each pen stroke as a closed shape. Import that DXF and you get snap points on every edge, then redraw centre lines and true geometry on top. The scanning side is covered in how to convert a scanned drawing to CAD.

Which problems come up most, and how do you fix them?

  • Hatching turns into hundreds of lines. With layers per colour it sits on its own layer, so remove that layer’s objects before building wires.
  • Duplicate lines stop Draft Upgrade from making faces. Delete one copy where two outlines overlap.
  • Outlined text in the PDF arrives as tiny closed shapes. Delete it and add your own text.
  • Dimensions come in as loose lines, arrows and text. Read them, then delete them before building wires.
  • Wrong scale almost always means a drawing scale like 1:2 or 1:10 was never undone. Measure first, model second.

For CNC or laser work, the DXF itself can go straight to your CAM software, and PDF to DXF for CNC covers units, tolerances and joining polylines.

Next steps: convert one page with Set scale, import it, and measure the longest dimension on the drawing. If it matches, build your first sketch from it.

Questions people ask

Can FreeCAD open a PDF file?

FreeCAD has no built-in PDF vector import. Convert the PDF to DXF or SVG first and use File > Import, or export a scanned page as an image and import it as a calibrated image plane.

Why is my imported DXF the wrong size in FreeCAD?

FreeCAD reads each DXF drawing unit as one millimetre, so a drawing at paper size stays at paper size. Set the real scale during conversion, or change the scale factor in Edit > Preferences > Import-Export > DXF before importing.

How do I turn imported DXF lines into a solid in FreeCAD?

Join the lines into closed wires with Draft Upgrade, convert them with Draft to Sketch, check the sketch for gaps with Validate sketch, then Pad it in PartDesign.

Is the DXF or the SVG method better for FreeCAD?

DXF keeps layers and text and is easier to scale correctly. SVG through Inkscape works well for logos and outlines, but it arrives at paper size and needs a scale step afterwards.

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