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Features · Lesson 1

SOLIDWORKS Extruded Boss/Base

Extruded Boss/Base pushes a 2D sketch straight out into a solid. It is the first feature of most parts. You choose where it starts (From), how far it goes (the end condition — a set depth, up to a face, through everything), and optionally a second direction, a draft angle or a thin wall. A closed sketch makes a solid; an open sketch makes a thin-walled feature.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Sketch profile extruded into a solid with a drag arrow and depth value

Where to find it

Features tab → Extruded Boss/Base (Insert → Boss/Base → Extrude)

End conditions

End condition Extrudes…
Blind A set distance from the sketch plane
Through All Through all existing geometry
Through All – Both Through everything in both directions
Up To Next To the next surface that blocks the whole profile
Up To Vertex To a plane through a chosen vertex, parallel to the sketch
Up To Surface To a chosen face or plane
Offset From Surface To a set distance from a chosen face
Up To Body Up to a chosen body
Mid Plane Equally to both sides of the sketch plane

From the official SOLIDWORKS Help list of extrude end conditions.

Other options in the PropertyManager

Option What it does
From Start at the sketch plane (default), an offset, a vertex or another face or plane — no extra plane needed
Direction 2 A second, independent extrusion the other way
Draft Tapers the sides by an angle, for moulded and cast parts
Thin Feature Gives the profile a wall thickness — one direction, two directions or mid-plane
Selected Contours Extrude only some regions of the sketch
Merge result Joins the new solid to the existing body (on by default)
Feature Scope Chooses which bodies the feature affects in multibody parts

Next: remove material with Extruded Cut.

Step by step

  1. 1

    Sketch the profile

    On the Front Plane sketch a Circle Ø40 centred on the origin and fully define it.

  2. 2

    Start the extrude

    With the sketch selected (or still open), click Features → Extruded Boss/Base. A yellow preview and a drag arrow appear.

  3. 3

    Choose Mid Plane

    In Direction 1 change Blind to Mid Plane and type 30 mm. The cylinder now grows 15 mm to each side of the Front Plane, so the part stays symmetric about it.

    Diagram of extrude end conditions — Blind, Through All, Up To Next, Up To Surface, Offset From Surface, Mid Plane
    How the main end conditions decide where the extrude stops.
  4. 4

    Confirm

    Click the green tick. You can also set the depth by dragging the arrow (Instant3D) — a ruler appears for exact values.

Common mistakes

  • Using Blind in one direction for a symmetric part. Mid Plane keeps it centred on the sketch plane, which helps mirroring and mating later.
  • Leaving a tiny gap in the sketch. An open profile turns the extrude into a thin feature, which is rarely what beginners want.
  • Up To Next when the next face does not cover the whole profile — it then fails. Use Up To Surface instead.
  • Unticking Merge result by accident, which leaves a separate body in the part.

Lesson 1 of 18 in the features course.

Practice

Extrude a Ø40 circle on the Front Plane with Mid Plane, 30 mm. Check: volume 37,699.11 mm³, and the Front Plane cuts the cylinder exactly in half.

Sources

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

Frequently asked questions

What is the difference between Blind and Mid Plane?

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Blind extrudes the set distance in one direction from the sketch plane. Mid Plane extrudes the total distance split equally on both sides.

What does Up To Next do?

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It extrudes up to the next surface that blocks the entire profile in the same part. If no single surface blocks the whole profile, use Up To Surface.

Can I extrude an open sketch?

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Yes, as a thin feature: SOLIDWORKS adds a wall thickness to the open profile. You can also tick Thin Feature with a closed profile to get a hollow shape.

How do I extrude only part of a sketch?

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Use Selected Contours in the PropertyManager and pick the regions or contours to extrude. One sketch can then drive several features.