Overview#
The Sketch Palette is a small floating panel that appears at the right side of the canvas while a sketch is active. It collects the view and behavior toggles that affect how you draw: whether new geometry is normal or construction, whether the camera looks straight at the sketch, whether the grid snaps your cursor, whether the model is cut away by the sketch plane, and which overlays (profiles, points, dimensions, constraints) are drawn.
Knowing the palette is a cheap way to become faster. Many "Fusion is behaving strangely" problems in sketches (the cursor will not snap, dimensions have disappeared, the part is in the way, a profile will not shade) come down to one checkbox in this palette.
Where to find it#
- Appears automatically when you create or edit a sketch, docked at the right side of the canvas.
- If it is not visible, check that you are actually inside a sketch (the Sketch contextual tab is showing).
- The palette has a Contextual Options section (creation types for the active tool, or options for the selected object) and an Options section.
Contextual options and status#
The top of the palette adapts to what you are doing. With a creation tool active, the Contextual Options (also called Feature Options) list that tool's types, so you can switch between line types, arc types, circle types, rectangle types, polygon types, slot types, chamfer types or blend curve types without restarting the command. With an object selected, they list options for that object: a selected spline offers Normal/Construction and a curvature comb toggle, and a selected Control Point Spline adds Change Spline Degree.
The palette also shows the sketch Status (Under-Constrained or Constrained) and the Find Under-Constrained, Compute Sketch and AutoConstrain buttons that are described on the fully constrained sketches page. AutoConstrain, and Finish with AutoConstrain, are not available in Fusion for personal use.
Step by step#
- Start or edit a sketch so the palette appears.
- Expand the Options section if it is collapsed.
- Click Look At if you want the camera to face the active sketch plane.
- Check Sketch Grid and Snap if you want grid-aligned drawing, and Slice if the model is blocking your view of the plane.
- Turn on Show Profile, Show Points, Show Dimensions, Show Constraints, Show Construction Geometries and Show Projected Geometries according to how much visual information you want.
- When you finish drawing, click Finish Sketch on the Sketch contextual tab.
Options reference#
The entries below are those listed in Autodesk's Sketch Palette reference. Defaults are not stated in the help, so check them in your build.
| Option | What it does | Notes/default |
|---|---|---|
| Linetype | Converts selected sketch geometry to a different linetype | Also available as Normal/Construction in the marking menu; construction geometry is not part of the boundaries of the sketch |
| Construction | Creates construction geometry | Click it, then draw |
| Centerline | Creates centerline geometry | Centerlines show orange when unconstrained |
| Look At | Rotates the camera to look directly at the active sketch plane | One-shot button |
| Sketch Grid | Shows or hides the sketch grid | |
| Snap | Enables or disables snapping to the sketch grid | |
| Slice | Temporarily cuts through bodies where they intersect the active sketch plane | Display aid only |
| Show Profile | Shows or hides blue shading for closed profiles | |
| Show Points | Shows or hides sketch points | |
| Show Dimensions | Shows or hides sketch dimensions | Hiding does not delete them |
| Show Constraints | Shows or hides sketch constraints | |
| Show Construction Geometries | Shows or hides construction geometry in the active sketch | |
| Show Projected Geometries | Shows or hides projected geometry in the active sketch | |
| 3D Sketch | Enables or disables the ability to sketch in 3D | |
| Change Spline Degree | Appears when a Control Point Spline is selected; changes its degree | See the splines page |
Linetype in detail#
The Construction and Centerline entries work as modes: click one before drawing and everything you create is construction or centerline geometry, or select existing geometry and click it to convert. Clicking Construction again on construction geometry converts it back to normal sketch geometry.
Linetype is the only palette entry that modifies your data rather than the display. Selecting geometry and clicking the Construction option next to Linetype flips it between normal and construction (clicking it again on construction geometry converts it back). With nothing selected, the geometry you create next is construction. The X key is widely used as a shortcut for this, but it is not listed in Autodesk's help. The practical consequence is that you can switch to construction mode, drop a few centerlines or reference circles, switch back, and keep going without restarting the tool.
Look At#
Look At rotates the camera so you are looking directly at the active sketch plane. Use it whenever you have orbited away.
Sketch Grid and Snap#
The grid is a drafting aid. Per Autodesk's help, snapping to the grid or to other geometry shows object snap symbols and, when you snap to a specific point, the logical constraints are added. Geometry that is merely placed near a grid point is not constrained, so still dimension or constrain it.
Slice#
Slice temporarily cuts through bodies where they intersect the active sketch plane. This is handy when you sketch on an internal plane and need to see what you are drawing relative to existing geometry. It is a display aid: no geometry is actually cut.
Show options#
The Show group controls overlays. When working on a complicated sketch you will often hide Points and Constraints to see clean geometry, then bring Constraints back to diagnose a problem. If a dimension or constraint "disappeared", it very likely was hidden here and not deleted. If a profile does not shade, check Show Profile first, then check whether the loop is actually closed.
Automatic constraints while drawing#
While you draw, object snap symbols appear near the cursor when you snap to the grid or other geometry, and snapping to a specific point adds the logical constraints. For example, ending a line on another line's endpoint makes the endpoints coincident.
Note: not confirmed in Autodesk's documentation: a Constraint Settings list in the Sketch Palette, and a Ctrl modifier to suppress inference. Neither appears in the palette reference. If an unwanted constraint appears, delete it afterwards.
Preferences that complement the palette#
The palette controls per-sketch display. Fusion's Preferences also contain sketch-related settings (for example whether the view looks at the sketch plane on creation, and whether edges are auto-projected when you start a sketch on a face).
Note: not confirmed in Autodesk's documentation: the exact names and locations of these preferences. Look through the Preferences dialog in your build rather than relying on a name from this guide.
Tips and pitfalls#
Tip: When a sketch looks wrong, open the palette and toggle display options one at a time. A hidden profile, hidden dimensions, or hidden projected geometry is a frequent cause of a sketch that looks broken.
Tip: Turn on Slice when sketching on a plane inside a body so you can see what is on the plane.
Tip: Use Linetype before you draw, not after, when you know the next entities are construction. You avoid selecting and toggling later.
Warning: A rectangle snapped to grid points looks tidy but is still under-defined (blue). Dimension it.
Warning: Hiding Constraints or Dimensions does not remove them, and they still drive the geometry. Do not assume the sketch is unconstrained because you cannot see the badges.
Practice exercise#
- Create a sketch on the XY plane and open the Sketch Palette.
- Turn off Sketch Grid and Snap, then draw a line that is close to horizontal and note whether a Horizontal constraint badge appears.
- Draw another near-horizontal line, deliberately slightly tilted, and apply Horizontal/Vertical manually from the Constraints panel if it did not get one.
- Select a line and click Construction next to Linetype to make it a construction line (or use Normal/Construction in the marking menu), then draw a circle that touches it and note that the circle forms a profile but the line does not.
- Toggle Show Profile, Show Dimensions, and Show Constraints one at a time to observe what each hides.
Expected result: you can predict exactly what each overlay toggles and can convert geometry between normal and construction.
Related#
- Sketch basics (02-sketching/sketch-basics)
- Constraints (02-sketching/constraints)
- Dimensions (02-sketching/dimensions)
- Troubleshooting sketches (02-sketching/troubleshooting)