CourseWiki/Engineering Graphics and CAD/CAD Modeling

Extrude and Revolve

Turn a sketch into a straight or rotational solid, and choose an end condition that preserves the intended shape when dimensions change.

Extrude carries a cross-section in a straight direction

For a plain solid extrusion, select a closed sketch region and give it depth. A rectangular region makes a block; a circular region makes a cylinder. Without draft, the cross-section remains constant along the extrusion.

A boss/base extrusion creates or adds solid material. An extruded cut removes material where the extrusion intersects the target solid. Check the arrow, preview, and selected bodies. A cut pointing away from the part cannot remove material from it.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A closed rectangle is carried along a depth direction to create a rectangular solid. — Sketch → straight depth → solid. This schematic shows the geometry, not a software dialog.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. In section, a rectangular sketch on a block is cut downward to leave a flat-bottomed pocket. — Section through a rectangular cut: the floor and surrounding body remain.

In Onshape, choose the result operation New, Add, or Remove. In SOLIDWORKS, check the boss/cut command and merge or feature scope settings. Adding touching material and creating a separate body are different intentions.

Closed profiles, thin features, and surfaces

Closed regions are the simplest starting point for solids. Open sketches can be used with thin-feature or surface options, but those are different constructions: a surface has no solid volume, while a thin feature adds a wall thickness. Check the result type before accepting the preview. See Onshape: Extrude.

Choose the end condition for what should happen after an edit; Interactive; Practice

Choose the end condition for what should happen after an edit

Condition	What controls the end	Use when
Blind	A specified distance in the selected direction.	A pocket must keep a particular depth.
Through all	All target material along the selected direction.	A cut must remain through as the part thickens. Check body scope and one- versus two-direction settings.
Up to next	The next terminating surface that intercepts the entire profile.	The next suitable boundary is the intended stop. It is not simply the first edge encountered.
Up to surface / face	A selected terminating surface or face.	The feature must follow that particular boundary when it moves. The selection becomes a dependency.
Mid-plane	A total depth split equally about the sketch plane.	The part must stay centered. In SOLIDWORKS, a 14 mm Mid Plane depth extends 7 mm each way.

Worked thickness edit. One rectangular cut starts on the top face of one flat plate, travels downward normal to that face, and removes material from that selected body only. Compare a distance-controlled blind cut with a through-all cut before and after the plate becomes thicker.

All three sections use the same vertical scale: 8 drawing units per millimeter.

The requested blind distance reaches beyond this plate; actual removal stops at the body boundary.

The blind distance stays 12 mm, so the later thickness edit leaves a floor.

Through all follows this selected plate in the stated direction.

Design goal	Choice that survives the edit	Why
Opening must stay through	Through all	The termination follows the selected plate thickness.
Pocket must retain a floor	Blind, with a depth smaller than the final thickness	The fixed distance intentionally stops before the far face.

This teaching model does not cover up-to-face, up-to-next, multiple bodies, opposite directions or revolved cuts. Check the selected sketch region, direction and body scope in the CAD preview.

Do not substitute an oversized blind cut for a through-all requirement. It may work today and leave a thin floor after a later edit. Conversely, through all is wrong for a pocket that must retain its floor.

Onshape uses a Symmetric option for supported end types. Dialog names and available conditions depend on the selected operation; inspect the preview and measured result rather than transferring every setting by name.

Practice end conditions Practice symmetric depth

Vendor help for extrusion boundaries

See SOLIDWORKS: Extrude PropertyManager and Onshape: Extrude. A failed up-to feature may indicate that its target no longer covers the profile, not that the sketch is wrong.

Revolve rotates a section around an axis

Select a section, an axis of rotation, and an angle. A full turn is 360°; a smaller angle produces a partial rotational shape. A boss revolve adds material, and a revolved cut removes it. Start with a closed section on one side of the axis for a straightforward solid revolve.

Three-step sequence: steps 1 and 2 across the top, then step 3 below. A rectangular section offset from a vertical axis rotates through 360 degrees to make a hollow cylindrical sleeve. — The gap between the section and the axis becomes the bore. Rotating a section that reaches the axis can instead make a solid center.

A straight sketch line, centerline, or reference axis can define rotation when supported by the command. The axis must be deliberately located. A diameter describes the distance across a round shape; the distance from the axis to its outer wall is the radius.

A stepped sleeve can often be built with one revolved section including its bore. Repeated extrusions and cuts can also build it, but put the coaxial steps under separate controls. Choose the sequence that makes the important dimensions easiest to change.

Check overlap and axis selection before adding complexity

A section that crosses the axis, overlaps itself during rotation, or creates zero-thickness contact can fail. Simplify the section, verify its closure and axis, and inspect a small-angle preview. For the command entry points see SOLIDWORKS: Sketching with Extruded or Revolved Bosses/Bases. A turned part may suggest a revolve, but CAD history does not specify a lathe process; see Lathe Operations.

Pick the base feature from the shape's main organizing rule; Practice

Pick the base feature from the shape's main organizing rule

Use extrusion when a useful section stays the same along a straight direction. Use revolution when a useful section repeats around an axis. A cylinder can be made either way. A rotationally stepped part often makes the reason for choosing revolve clearer than a plain cylinder does.

Before accepting either feature, confirm the profile, direction or axis, end condition or angle, and result body. Then make one trial dimension change. Does the model still express the intent described in Feature-based Modeling?

Practice choosing a base Practice a scoped feature count

Appears in

DET 102 DET Part Features