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Sketching · Lesson 12

Trim and extend sketch entities

Trim Entities removes the parts of sketch lines and curves you do not need where they cross other entities. It lets you sketch overlapping simple shapes — a rectangle and a circle, say — and cut them back into one clean outline. Power trim, the default, trims everything your pointer drags across. The same tool can also extend entities to meet others.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Overlapping rectangle and circle being trimmed into one outline with a power trim trail

Where to find it

Sketch tab → Trim Entities (flyout also holds Extend Entities)

Trim options

Option How it works
Power trim Drag across pieces to trim them; a red square marks the last trim
Corner Pick two entities; they are trimmed or extended to meet in a corner
Trim away inside Pick two boundaries, then the entities to trim between them
Trim away outside Removes what lies outside the two boundaries
Trim to closest Click a segment; it is removed to the nearest intersections
Keep trimmed entities as construction geometry Trimmed pieces stay as dashed lines
Ignore trimming of construction geometry Protects centerlines from Power trim

Trimming is often the fastest way to build complex outlines from simple shapes. For outlines that follow existing edges, Convert Entities and Offset Entities are faster still.

Step by step

  1. 1

    Sketch overlapping shapes

    On the Front Plane draw a Corner Rectangle 60 × 40 from the origin, and a Circle Ø40 with its centre on the midpoint of the right edge.

  2. 2

    Power trim

    Trim Entities → Power trim. Hold the left mouse button and drag across the part of the right rectangle edge that lies inside the circle, then across the left half of the circle (inside the rectangle). What the dotted trail touches is removed.

    Power trim trail dragged across the inner part of a circle and rectangle edge
    Drag across the pieces you want to remove.
  3. 3

    Check the outline

    You should have a rectangle whose right end is a half-circle. Turn on Shaded Sketch Contours to see that it is one closed area.

  4. 4

    Re-dimension if needed

    Trimming can remove dimensions or relations attached to the deleted pieces. Check the status bar and add what is missing.

Common mistakes

  • Trimming a piece that carried a dimension — the dimension disappears too. Trim first, dimension last, or check after trimming.
  • Power-trimming across a centerline you wanted to keep. Tick *Ignore trimming of construction geometry*.
  • Leaving tiny leftover segments after trimming; the feature then fails. Use Repair Sketch to find them.

Lesson 12 of 17 in the sketching course.

Practice

Build the shape above (60 × 40 rectangle with a Ø40 circle on the midpoint of the right edge, trimmed to one outline) and extrude it 10 mm. Check: volume 30,283.19 mm³.

Sources

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

Frequently asked questions

What is Power trim in SOLIDWORKS?

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The default trim option: hold the mouse button and drag across the pieces you want to remove. Everything the trail crosses is trimmed back to the nearest intersection.

How do I extend a line in a sketch?

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Use Extend Entities in the Trim flyout and click the line near the end to extend, or in Power trim click a line and move to the side to preview the extension, then click again.

How do I trim without deleting the piece?

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Tick Keep trimmed entities as construction geometry. The trimmed parts stay as dashed construction lines for reference.

Why did my dimension disappear after trimming?

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It was attached to the piece you trimmed away. Add a new dimension to the remaining geometry.