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For a constant-thickness part, import a DXF/DWG profile into a SOLIDWORKS part sketch, confirm units and dimensions, repair unintended contour gaps or overlaps, and extrude by a known thickness. This works when the drawing defines that profile and thickness. An arbitrary flat view does not determine all features of a three-dimensional part.
Jump to: Check the source · Import and extrude · Troubleshoot · Verify the result
Start with a profile you can verify
This original exercise assumes a flat plate: 80 × 40 mm outside rectangle, a centered 20 × 10 mm rectangular through-opening, and a separately specified thickness of 4 mm. There are no fillets, chamfers, bends or hidden pockets. Preserve the received drawing and use a working copy. A plate outline plus a thickness requirement is different from a whole equipment drawing.
With the outside lower-left corner at X = 0, Y = 0, the opening extends from X = 30 to 50 and Y = 15 to 25. These coordinates provide an independent way to check location after import. If the actual drawing lacks thickness or opening depth, request those values; do not infer them from how the sketch looks.
Before importing, identify which layers contain part geometry. Dimensions, text, centerlines, borders and multiple projected views should not accidentally become extrusion contours. Keep the original annotations available as a reference while isolating the intended profile in the working sketch.
Import the sketch and create the volume
- Open the DXF/DWG with the SOLIDWORKS import wizard and choose a new part with a 2D sketch where that option is available. Confirm your installed version’s options in the official DXF/DWG import instructions.
- Select the intended geometry and units. After import, measure the outside rectangle and opening. For this exercise they must be 80 × 40 mm and 20 × 10 mm; a visually similar profile is not enough.
- Inspect the contours for unwanted duplicates, short segments, gaps and overlaps. The official import workflow offers Repair Sketch for gap/overlap problems. Repair only after checking the intended drawing; an opening in the linework might be deliberate.
- Create a boss extrusion with 4 mm depth. Inspect the preview so the centered inner contour leaves an opening through the plate. If selection behavior differs, identify the intended region explicitly; do not accept a filled center just because an extrusion succeeds.
- Inspect the solid from the side and through the opening. Save a native working document, close it and reopen it before completing the checks below.
If the source contains multiple orthographic views or varying depths, it needs a reconstruction plan with multiple features. SOLIDWORKS’ imported 2D data overview describes using drawing views as sketches for subsequent modeling. It does not make missing dimensions known.
Why will the imported DXF not extrude?
The contour is open or overlapping
Zoom into reported endpoints and intersections. Compare with the reference drawing, identify whether a segment is missing or duplicated, and correct one issue at a time. Recheck the preview after each repair. Closing every visible gap indiscriminately can remove a real opening or connect separate parts.
The wrong region extrudes
Hide or remove unintended drawing geometry from the working profile, while preserving the source. Inspect selected contours and the preview. In the plate exercise the 20 × 10 mm rectangle is a through-opening, not a second raised block.
The size is wrong
Compare measured dimensions with the drawing’s written values and review the import units. Check more than one independent dimension. If one correction fixes width but breaks height, investigate source distortion or mixed geometry instead of continuing with a stretched model.
The sketch is under defined
Under defined and open contour describe different issues. A closed profile may still move because its position or other relations are unconstrained. Use the under-defined sketch exercise to inspect remaining movement. Fully constraining an incorrect imported shape does not make it correct.
Acceptance checklist for the plate exercise
- One intended plate body, 80 × 40 × 4 mm envelope.
- Centered 20 × 10 mm opening visible through the full thickness.
- Opening bounds X = 30..50 mm and Y = 15..25 mm in the declared source coordinates.
- No border lines, text or other drawing views included as unintended features.
- Saved working file reopens with the checked geometry and required editing behavior.
If printing is the next step, choose a compatible model handoff format, inspect its imported dimensions and follow the print-preparation checks. Successful extrusion is not physical-print acceptance.
For a broader multi-view reconstruction task, see MST’s drawing-to-model workflow. Describe your drawing type and intended output before sharing protected files. This tutorial documents a general SOLIDWORKS workflow, not a claim that MST supports every DXF variant. Discuss a drawing-to-model demonstration.
Reviewed 7 October 2026. Documentation-based procedure and original hypothetical plate; no SOLIDWORKS execution or physical print was performed for this publication. Commands and import results depend on the installed release and actual source file.
MST Engineering Intelligence. “DXF to 3D Solid in SOLIDWORKS: Import, Extrude and Check.” MST Engineering Intelligence. Updated 2026-10-07. https://mst-us.ai/dxf-to-3d-solid-solidworks/
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