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Sketching · Lesson 14

SOLIDWORKS Convert Entities

Convert Entities copies model edges, faces or other sketches into the sketch you are editing, projected onto its plane. The copies are tied to the original edges with an On Edge relation, so they follow when the model changes. Use it when a new feature must match the shape of an existing one — a lid on a box, a boss on a face, a cut through an outline.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Model face edges projected into a sketch as black lines with On Edge relation icons

Where to find it

Sketch tab → Convert Entities (flyout also holds Intersection Curve and Silhouette Entities)

Tool What it creates
Convert Entities Exact copies of selected edges, faces or sketch entities
Intersection Curve Sketch lines where the sketch plane cuts the selected faces
Silhouette Entities (2020+) The outline of a body as seen normal to the sketch plane
Offset Entities Copies at a distance — see Offset Entities

Since SOLIDWORKS 2024 SP1 converted entities can be created as construction geometry, for references you do not want to build on. In assemblies, converting edges of another part creates an external (in-context) reference; if those files are later moved or renamed, see missing references.

Step by step

  1. 1

    Make a base block

    Extrude an 80 × 50 mm Center Rectangle 10 mm on the Front Plane.

  2. 2

    Sketch on the front face

    Click the large front face of the block and click Sketch.

  3. 3

    Convert the face edges

    With the face still selected, click Convert Entities. The four outer edges are projected into the sketch instantly and turn black — they are fully defined by the model.

    Front face of an 80 by 50 block selected and converted into a sketch outline
    Select the face and click Convert Entities — the outline becomes sketch geometry.
  4. 4

    Build on it

    Extrude the new sketch 5 mm away from the block. The boss matches the face exactly, and changes with it if the block is resized.

Common mistakes

  • Converting edges in an assembly sketch without meaning to — it creates external references to other parts. Use it in parts where the reference is intended.
  • Expecting inner loops (holes) to convert when you pick a face — only the outer loop is converted by default; use the inner-loop options.
  • Dragging a converted endpoint — it can move along the edge, so check the shape after editing.

Lesson 14 of 17 in the sketching course.

Practice

Do the steps above: an 80 × 50 × 10 mm block with a converted-edge boss of 5 mm on its front face. Check: total volume 60,000 mm³. Change the block's width to 100 mm and rebuild (Ctrl + B) — the boss follows and the volume becomes 75,000 mm³.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

What does Convert Entities do in SOLIDWORKS?

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It projects selected model edges, faces or sketch entities onto the current sketch plane and ties them with On Edge relations, so the sketch updates when the model changes.

How do I convert the edges of a hole?

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Selecting a face converts its outer loop by default. Use the inner loops options in the Convert Entities PropertyManager, or select the hole edges directly.

What is the difference between Convert Entities and Offset Entities?

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Convert copies edges exactly; Offset copies them at a distance. Both stay linked to the originals.

What is Silhouette Entities?

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A tool added in SOLIDWORKS 2020 that projects the outline of a body or component as seen normal to the sketch plane — useful for round or complex parts with no single edge to convert.