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Sketching · Lesson 3

SOLIDWORKS circle tools

The Circle tool draws a circle from its centre: click the centre, then click again (or drag) to set the size. Perimeter Circle draws a circle through three points on its edge, which is handy when a circle must touch existing geometry. A circle is fully defined by its diameter and the position of its centre — two dimensions or relations for the centre, one for the size.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Sketch with a centre circle and a perimeter circle through three points, with a diameter dimension

Where to find it

Sketch tab → Circle flyout (Circle, Perimeter Circle)

Circle vs Perimeter Circle

Circle Perimeter Circle
Defined by Centre and a point on the edge Three points on the edge
Typical use Holes, bosses, shafts Circles that must touch existing geometry
To fully define Centre position + diameter Position of the points or relations + diameter

For drilled and tapped holes in a finished part, the Hole Wizard is usually a better choice than a sketched circle and a cut, because it stores the hole type for drawings. Several circles in a row or ring are faster with sketch patterns or, better, a feature pattern.

Step by step

  1. 1

    Pick the Circle tool

    Open a sketch on the Front Plane and click Circle.

  2. 2

    Place the centre on the origin

    Click the origin for the centre (a coincident relation is added), move out and click again. Click-drag does the same in one motion.

  3. 3

    Dimension the diameter

    Smart Dimension → click the circle edge and place the dimension. SOLIDWORKS shows a diameter (Ø) for circles. Type 50.

  4. 4

    Add a concentric circle

    Draw a second circle with its centre on the same point and dimension it 30. Because both centres are on the origin they are concentric.

    Two concentric circles of 50 and 30 mm extruded into a ring
    Two concentric circles extrude into a ring.
  5. 5

    Equal circles

    For several holes of the same size, dimension one circle, then Ctrl-select the others with it and add an Equal relation. Changing one dimension changes them all.

Common mistakes

  • Dimensioning each of several identical circles. Use one dimension and Equal relations so a later change is one edit.
  • Leaving the centre floating. A circle with only a diameter is still blue — its centre can move.
  • Measuring between two circles centre-to-centre when the drawing needs the gap. Hold Shift while clicking the circles to dimension to their edges.

Lesson 3 of 17 in the sketching course.

Practice

Draw two concentric circles on the origin, Ø50 and Ø30, and extrude 10 mm — SOLIDWORKS makes a ring because the inner circle becomes a hole. Check: volume 12,566.37 mm³. A single Ø50 circle extruded 10 mm gives 19,634.95 mm³.

Sources

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

Frequently asked questions

How do I dimension a circle as a radius instead of diameter?

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Select the dimension and change the display to radius in the dimension PropertyManager (Leaders tab), or right-click it and choose Display Options. The size is the same; only the display changes.

What is a perimeter circle?

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A circle defined by three points on its edge instead of a centre. Use it when the circle must pass through or touch existing points or lines.

How do I make two circles the same size?

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Select both (Ctrl+click) and add an Equal relation from the context toolbar or the PropertyManager.

How do I dimension to the edge of a circle?

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Hold Shift while clicking the circle with Smart Dimension. The dimension goes to the nearest or farthest point of the circle instead of its centre.