Overview#
A sketch is a flat, 2D drawing that lives on a plane or planar face and sits in the timeline as a feature. Almost every solid model in Fusion starts the same way: you draw 2D geometry, close it into one or more profiles, and then turn those profiles into 3D with a command such as Extrude, Revolve, Sweep, or Loft. Sketches are therefore the foundation of parametric modeling in Fusion. A clean, well-constrained sketch gives you a model that updates predictably when you change a dimension. A sloppy sketch gives you a model that explodes the moment you edit it.
This page covers the lifecycle of a sketch: creating it, choosing its plane, drawing inside the sketch environment, finishing it, and re-editing it later. It also explains the vocabulary used throughout this section (profile, sketch plane, origin, construction geometry, under-defined versus fully defined) so the later pages can go deeper without repeating the basics.
Fusion offers sketching in the Design workspace. The Create Sketch icon appears on the Solid, Surface, Form, Sheet Metal, Base Feature Solid and Base Feature Surface tabs, and selecting it reveals the dedicated Sketch contextual tab (highlighted blue to show you are in a temporary mode). The Sketch tab is also where nearly every tool covered in this section lives.
Where to find it#
- Create a sketch: Solid tab > Create panel > Create Sketch. The same command exists on the Surface, Form, Sheet Metal and Base Feature tabs. Valid selections are origin planes, work planes and planar faces.
- Find any tool by name: Press S to open the toolbox search and type "Create Sketch".
- Marking menu: Right-click in the canvas to use the marking menu; sketch commands such as Finish Sketch live under its Sketch entry.
- Edit an existing sketch: Right-click the sketch node in the Browser or timeline and choose Edit Sketch, or double-click the sketch node in the timeline. Note that if you select an existing sketch entity or sketch node while Create Sketch is running, that sketch is edited instead of a new one being created.
- Finish: Click Finish Sketch on the Sketch contextual tab, or right-click and choose Sketch > Finish Sketch in the marking menu. Its menu also offers Finish with AutoConstrain (not available in Fusion for personal use).
Step by step#
- Open or create a design. Make sure you are in the Design workspace. If you have a fresh document, the Browser shows the Origin folder with three planes (XY, XZ, YZ), three axes, and the origin point, all hidden by default until you toggle their visibility.
- Start Create Sketch. Click Create Sketch on the Solid tab. The cursor now asks you to select a plane or planar face.
- Pick the sketch plane. Click one of the three origin planes that appear in the canvas, any flat face on an existing body, or a construction plane that you made earlier. If the view is not facing the plane, use the Look At option in the Sketch Palette, covered on the next page.
- Draw. The Sketch tab opens. Pick a creation tool such as Line (L), Center Diameter Circle (C), or 2-Point Rectangle (R) and click in the canvas. Detailed behavior of each tool is in the following pages.
- Constrain and dimension. Press D to launch Sketch Dimension and give lengths, diameters, and angles their real values. Add geometric constraints (Coincident, Horizontal/Vertical, Tangent, and so on) from the Constraints panel (visible by default) or let Fusion apply them as you draw.
- Check the profile. Make sure the area you want to extrude is shaded blue. Show Profile in the Sketch Palette shows or hides the blue shading of closed profiles. A shaded region means the loop is closed and a feature command can pick it.
- Finish the sketch. Click Finish Sketch. The sketch becomes a timeline entry and its profiles are available to Extrude and other commands.
- Use the profile. Start Extrude (E) and click inside the shaded region. You do not need to select the whole sketch. Selecting a profile is how Fusion decides what to make solid.
- Edit later. Double-click the sketch in the timeline to re-enter it. Any change you make will cascade forward through every feature that depends on it.
Understanding sketch planes#
Every sketch is attached to a plane. The plane determines the sketch coordinate system: the sketch X and Y axes lie in the plane, and the sketch origin is the point where the plane's coordinate system projects. Which plane you pick matters more than beginners expect.
| Plane choice | Behavior | When to use it |
|---|---|---|
| Origin plane (XY, XZ, YZ) | Stable, never moves, aligned to the global origin | The first sketch of almost any part; anything that needs to be symmetric about the origin |
| Planar face of a body | Sketch is attached to the face and follows it if the face moves | Features that must sit on a specific surface, such as a boss or a pocket on top of a block |
| Construction plane | Sketch follows the work plane, whatever its definition | Angled features, mid-planes, offsets, or planes tangent to curved surfaces |
| Face of a body, then edited | The plane reference may break if the face is deleted or the feature order changes | Convenient but fragile. See best practices |
A key point: when you sketch on a face, the sketch inherits a dependency on the feature that created that face. If you later edit or reorder that feature, the sketch can lose its plane (the timeline shows a warning icon). For stable designs, sketch on origin planes or on explicit construction planes wherever practical.
Orientation and the sketch coordinate system#
Fusion lets you choose between Z-up and Y-up modeling orientation, which changes whether the XY plane looks like the floor or a wall. Check your setting before you follow a tutorial.
Note: not confirmed in Autodesk's documentation: the exact Preferences path of the orientation setting.
A sketch also has a visible Sketch Origin. If you started on an origin plane, the sketch origin coincides with the global origin. If you started on a face, the sketch origin is placed according to the face and may not be where you expect. You can project the global origin into the sketch with Project (P) if you need to dimension from it.
What is a profile?#
A profile is a closed region bounded by sketch curves. Fusion computes profiles automatically each time the sketch changes. A few rules apply:
- Nested closed loops create profiles with holes. A circle drawn inside a rectangle yields two selectable profiles: the ring-shaped region (rectangle minus circle) and the inner disc.
- Where curves cross, every enclosed area becomes its own profile. Two overlapping circles produce three regions: the left crescent, the lens in the middle, and the right crescent.
- Construction lines (dashed) and points never create profiles.
- A single open chain of curves has no profile, but it can still be used as a path for Sweep or as a rail for Loft.
- Gaps, overlapping segments, and self-intersections usually prevent a profile from forming. See the troubleshooting page.
Construction geometry and normal geometry#
Every curve has a Linetype: Normal or Construction. Normal geometry is drawn as a solid line, participates in profiles, and is used by features. Construction geometry is drawn dashed, never creates profiles, and exists only to help you constrain other geometry (for example, a centerline to mirror about, or a reference circle that drives the position of other holes). To change linetype, use the Linetype > Construction option in the Sketch Palette (before drawing, or with geometry selected), or right-click selected geometry and choose Normal/Construction in the marking menu. The X key is a commonly used shortcut for this, but it is not listed in Autodesk's sketch help. Most experienced users build sketches with a skeleton of construction geometry and then draw normal geometry that is constrained to it.
Sketch color and state cues#
Fusion uses color to tell you what the solver knows:
| Appearance | Meaning |
|---|---|
| Blue | Unconstrained (under-defined) geometry |
| Orange | Unconstrained centerline geometry |
| Black | Fully constrained geometry |
| Dashed line | Construction geometry |
Two more colors are documented elsewhere in the help: projected geometry is shown in purple, and geometry locked with the Fix constraint turns green. Other states (such as over-constrained warnings) are not described in the sketch docs and can vary with the theme, so check them in your own installation.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Create Sketch | Starts a new sketch on a selected plane or face | You can also select the plane first, then run the command |
| Edit Sketch | Re-enters an existing sketch | Double-click the timeline entry |
| Finish Sketch | Exits the sketch environment | Also in the marking menu; Finish with AutoConstrain is not in Fusion for personal use |
| Look At | Rotates the camera to look directly at the active sketch plane | In the Sketch Palette |
| Linetype (Normal/Construction) | Converts selected geometry, or sets what you draw next | Sketch Palette or marking menu |
| Sketch Origin | Reference for the sketch's coordinate system | Project it to dimension from it |
Tips and pitfalls#
Tip: Name your sketches. Right-click the sketch in the timeline or Browser and rename it to something like "Base profile" or "Hole pattern skeleton". A model with forty sketches named Sketch1 through Sketch40 is miserable to edit.
Tip: Draw the first sketch on an origin plane and center it on the origin (or put its key corner on the origin). Having a fixed, known anchor makes the rest of the model easier to constrain and mirror.
Tip: If you cannot find a sketch, check the Browser. A sketch that has been consumed by a feature is automatically hidden; use the lightbulb icon next to the sketch to show it again.
Warning: Sketching on a face of a body ties the sketch to that body's history. If you later suppress or reorder the feature that created the face, the sketch can lose its plane. Fusion marks this with a warning in the timeline. Prefer origin or construction planes for the geometry that the rest of the model depends on.
Warning: Never extrude a sketch where multiple profiles overlap unless you mean to. Check which profiles are highlighted before confirming the Extrude dialog.
Tip: Sketches are visible only while their lightbulb is on. If you finish a sketch and it vanishes, the sketch was probably automatically hidden because you used it in a feature. Toggle the lightbulb in the Browser.
Practice exercise#
- Create a new design and save it as "Sketch Practice".
- Create a sketch on the XY plane.
- Draw a rectangle with a corner on the origin and dimensions 60 mm by 40 mm. Dimension both sides with D.
- Draw a circle inside the rectangle and dimension its diameter as 10 mm and its center 20 mm from each of the two rectangle edges that meet at the origin. All geometry should turn black.
- Finish the sketch, then run Extrude (E) and click the ring-shaped profile (the rectangle minus the circle). Extrude it 8 mm.
Expected result: a flat plate with a 10 mm hole, 60 by 40 by 8 mm. Edit the sketch, change the width to 80 mm, and watch the plate and the hole position update.
Related#
- Sketch Palette: toggles and display options (02-sketching/sketch-palette)
- Lines and arcs (02-sketching/lines-and-arcs)
- Constraints (02-sketching/constraints)
- Fully constrained sketches (02-sketching/fully-constrained-sketches)
- Troubleshooting sketches (02-sketching/troubleshooting)