Extrude Command

Overview#

Extrude is the workhorse of solid modeling in Fusion. It takes a sketch profile (or a planar face) and pushes it along a straight line to create volume.

Extrude does four jobs, chosen with the Operation setting:

• Join adds material to an existing body.
• Cut removes material from an existing body.
• Intersect keeps only the volume shared between the new shape and an existing body.
• New Body / New Component creates a separate solid.

Extrude also produces thin walls (Thin Extrude), tapered features (draft built in), and, from the Surface tab, surface bodies. This page covers solids. Extrude of open profiles into surfaces works the same way but is documented under surface modeling.

Use Extrude when the feature is a straight prism. If the shape needs to rotate around an axis use Revolve; if it follows a curve use Sweep; if the cross-section changes use Loft.

Where to find it#

• Workspace: Design.
• Tab / panel: Solid tab > Create panel > Extrude (the first icon in the panel).
• Shortcut: E.
• Search: Press S to open the Model Toolbox (Autodesk's keyboard-shortcut list names it that) and type "Extrude".
• Shortcut from a sketch: After finishing a sketch, profiles are shaded. You can click a profile and press E directly.
• Press and pull alternative: Pressing Q on a planar face gives a quick extrusion, but without the full option set (see the Press Pull page).

Fusion has moved some buttons between releases. If an icon is not where you expect, press S and type the command name.

Step by step#

1. Create and finish a sketch. Draw a closed profile on a plane or face, for example a rectangle 40 mm by 25 mm. Click Finish Sketch in the toolbar.
2. Start Extrude. Press E. The Extrude dialog opens. If you have only one visible sketch with one profile, Fusion may preselect it.
3. Pick Profiles. With the Profiles selector active, click each shaded region you want. The profiles must be coplanar. You can also select a sketch in the Browser or Timeline to pick all of its profiles and geometry (including sketch text) at once. Nested profiles (for example a circle inside a rectangle) extrude as a ring if you click only the area between them.
4. Set the Start. Leave it at Profile Plane unless you need the feature to begin elsewhere (see the options table).
5. Choose Direction. One Side, Two Sides, or Symmetric.
6. Enter an Extent. Type a distance, drag the arrow, or choose To Object or All. You can type expressions such as thickness + 2 mm or user parameter names.
7. Choose the Operation. When the extrusion touches an existing body Fusion usually offers Join or Cut. Check it and change it deliberately.
8. Optional extras. Add Taper Angle, switch Type to Thin Extrude, or change the Objects to Cut/Participants.
9. Confirm. Click OK or press Enter. A timeline entry named "Extrude" appears. Double-click it later to edit.

Worked example: a bracket with a pocket#

1. Sketch a 60 x 40 mm rectangle on the XY plane and extrude 10 mm as New Body.
2. Select the top face and start a new sketch. Draw a 30 x 20 mm rectangle centered with a Center Rectangle.
3. Press E, select the rectangle, drag the arrow down into the body, type -6. The Operation switches to Cut. Click OK.

You now have a 6 mm deep pocket. Changing the first extrude to 12 mm in the timeline does not alter the pocket depth, because the pocket is measured from the top face.

Options reference#

Dialog fields differ slightly depending on Type and Extent. Names below follow Autodesk's Extrude reference.

Understanding Direction and Extent combos#

• Symmetric plus Whole Length 20 mm produces a 20 mm body centered on the sketch plane. Half Length 20 mm makes a 40 mm body.
• Two Sides with a negative second distance is legal; it just shifts the far side.
• To Object with Direction One Side stops at the selected object and updates when that object moves.

Tips and pitfalls#

Tip: Profiles that share edges are separate selectable regions. If you cannot click the region you want, a stray line or overlapping geometry is splitting it. Delete the stray line or toggle sketch visibility.

Tip: Click directly on the face of a body to extrude it without a sketch. This uses the face's boundary as the profile, like a quick Press Pull but with the full Extrude options.

Tip: Name parameters before you extrude (Modify > Change Parameters) and type the name into the distance field. This keeps the model easy to resize.

Warning: If Operation shows Join when you expected a new body, Fusion found an intersecting body. Join will merge them permanently in the model history. Check the dropdown before clicking OK.

Warning: Extrudes that use To Object with a face that later moves can fail if the face no longer intersects the profile. If the timeline shows a red warning, edit the feature and reselect the object.

Warning: Large taper angles on tall extrusions can make the shape self-intersect or collapse to a point. Reduce the angle or the height.

• Thin Extrude on a closed profile creates a hollow tube. On an open profile it creates a ribbon wall, ideal for brackets and clips.
• Cut only affects bodies that overlap the extrusion. If nothing appears to be cut, the tool body may be extending the wrong way. Flip direction or use the arrow.
• Using Intersect with a profile creates a body shaped like the overlap. Pair it with a second sketch on a perpendicular plane to carve complex shapes (the "intersecting extrusion" technique for visualizing a part from its front and side views).
• Sketch dimensions remain editable after the extrude. Right-click the sketch in the browser and choose Edit Sketch, or double-click it in the timeline.
• If the profile is not closed, Fusion will not shade it, and Extrude (non-thin) will not accept it. Look for gaps at the endpoints and close them with Coincident constraints.
• Hybrid vs. parametric: with design history on, every extrude is a timeline feature. If you turned history off (direct modeling), it executes but no timeline entry exists. See the direct modeling page.

Extent and start combinations with numbers#

Work through a few concrete cases to see how the options combine.

• Start Offset. Sketch on XY, set Start to Offset 15 mm, Extent 20 mm: the solid occupies Z = 15 to 35 mm. Its bottom floats above the sketch plane, so it does not touch a body that stops at Z = 10. Make Start Offset negative (-5 mm) to push the base below the plane so the new extrusion overlaps and joins an existing body.
• To Object. Extruding a 10 mm circle "To" a face 47.3 mm away yields a length that tracks the face. If you later change the base height to 50 mm, the boss stays flush. A fixed Distance would stop short, so use To Object for bosses that must always reach a mating surface.
• Symmetric. Whole Length 30 mm gives 15 mm each way; Half Length 30 mm gives 30 mm each way (60 total). A common error is entering the wrong measurement and getting a part twice or half the length expected.
• Two Sides with taper. Side 1 distance 20 mm with 0 degrees taper, Side 2 distance 10 mm with 5 degrees: a straight upper section and a draft below. The top width of a 30 mm square on the tapered side shrinks by 2 x 10 x tan(5) = 1.75 mm.
• Taper arithmetic. If the taper shrinks the profile as it grows (flip the sign if your preview goes the other way), a 40 mm square, 50 mm tall, at 2 degrees on all sides narrows by 2 x 50 x tan(2) = 3.5 mm at the far end, producing 36.5 mm. As general guidance (not Autodesk data), injection-molded parts commonly want roughly 1 to 3 degrees of draft.

Join, Cut and Intersect behaviors that surprise people#

Cut with several bodies. When you create a cut, the visible bodies participate and hidden bodies do not. If a screw body sits inside the hole location, cutting also nicks the screw. Hide bodies you do not want affected before you cut; when editing the feature, Objects To Cut lets you recompute (Auto-Select) or keep the original bodies.

Join with faces that merely touch. If a new boss sits exactly on a face, Join succeeds because the profile plane is shared. If it sits 0.01 mm above, the new body does not touch the old one, so there is nothing to join to. Always dimension the start from the face, not from an estimated number.

Intersect for compound shapes. Create a 60 x 40 mm front-view profile and extrude it 50 mm through (New Body). Sketch a 50 x 40 mm side view on the YZ plane and Extrude with Operation Intersect through All. The result is only the volume that satisfies both views, which is how you block out complex shapes from drawings.

New Component. In parametric design, creating a new component from an extrude is the right choice when you want each part to be assembled later. Create the component before sketching so that sketches live inside it.

Thin Extrude in practice#

For a thin extrude, Wall Location Side 1 grows the wall to one side of the profile curve, Side 2 to the other, and Center straddles it. If you want a 3 mm-thick wall whose outer dimension is exactly 50 mm, draw the 50 mm outline and choose the side that grows inward; with Center the outside would become 53 mm. For an open U channel in 3 mm material, remember the profile is a centerline unless you choose a side. Thin Extrude on a closed profile gives a hollow tube; with several nested closed profiles you get multiple walls in one feature.

Failure modes and fixes#

Workflow advice#

1. Dimension sketches from the origin or from the stable base edges, not from faces added late.
2. Make the first extrude symmetric about an origin plane when the part is symmetric, so mirrored features are easy.
3. Use one extrude per distinct feature. Combining unrelated features in one extrude means editing one changes the other.
4. Give extrudes meaningful names ("Boss: mounting", "Cut: wire channel") so the timeline reads as a recipe.
5. Drive distances with parameters whenever the same value appears twice. For example, wall used in both the base thickness and a rib thickness.

Practice exercise#

Model a small tray with drafted walls, a boss that tracks a surface, and an intersected shape, using numbers you check.

1. Sketch an 80 x 50 mm rectangle on XY and extrude 20 mm as a New Body with a Taper Angle of 2 degrees. Predict the top size (80 - 2 x 20 x tan 2 = 78.6 mm by 48.6 mm) and confirm with Measure.
2. Sketch a 70 x 40 mm rectangle on the top face and Cut 17 mm deep leaving a 3 mm floor, with a 2 degree taper in the direction that makes the pocket widen upward (flip the sign if the preview narrows). Check floor thickness with Measure.
3. Sketch a 12 mm circle on the pocket floor. Extrude it with Extent To Object, selecting the top face of the tray. This is a boss that always reaches the rim.
4. Change the first extrude's distance to 25 mm. The boss should follow; the pocket depth should not, since it was a fixed distance. Fix this by editing the pocket's distance to height - floor, with floor = 3 mm as a user parameter.
5. Thin Extrude: sketch an open U (50 mm wide, 30 mm tall), Thin Extrude 3 mm Center wall, Symmetric Whole Length 100 mm. Measure the outer width (53 mm); then redo it with the wall growing inward to keep 50 mm.
6. Create the Intersect example described above with front and side silhouettes of 60 x 40 and 50 x 40 mm.

Expected result: a drafted tray with predicted dimensions, a boss that follows the rim, a U-channel with a correctly placed wall, and an intersected block. Record any prediction that differed from the measurement and why.

Related#

• Revolve (rotational features)
• Sweep and Loft (path-driven and blended shapes)
• Press Pull and direct modeling (quick face edits)
• Combine, Split and Boundary Fill (booleans on existing bodies)
• Sketch profiles (in the sketching section)