Fully Constrained Sketch That Still Won't Extrude
A user is sketching a bracket profile on the XZ plane. The sketch contains two arcs, three lines, and a slot created with the Slot tool. The Sketch palette shows the geometry in black, and the status bar reports the sketch is fully constrained. When the user tries to extrude, Fusion refuses and the profile highlight does not appear over the intended region. The user confirms the sketch is closed by zooming in. There is a short line segment near the top arc that the user drew early and then redrew over. The sketch also contains a centerline used for symmetry that crosses the profile. The document units are millimeters and the extrude distance is 10 mm.
1. Diagnose why no profile is being detected despite the sketch appearing fully constrained and closed.
Read the worked answer
Fully constrained does not mean "valid closed profile." Constraint status only reports degrees of freedom, not region closure. The most likely cause is overlapping or duplicated geometry: the early line segment near the top arc was redrawn but not deleted, so two coincident edges lie on top of each other. Fusion cannot form a single clean closed region from coincident overlapping curves, so the profile highlight fails.
Diagnostic steps:
- Use Select > Select Other or window-select the top arc area to expose hidden overlapping curves.
- Check the sketch for duplicate entities; delete the redundant segment.
- Confirm endpoints are coincident rather than merely visually touching - zoom in and drag an endpoint slightly to test whether a coincident constraint exists.
- Verify that the centerline is set as a construction line. Construction geometry is excluded from profiles, but a normal line crossing the profile will split the region into multiple profiles.
- Re-check the profile after cleanup.
The judgement is that visual closure and constraint status are not proof of a valid profile; overlapping edges and non-construction lines are the usual culprits.
2. The centerline crossing the profile is suspected of causing problems. Explain how construction geometry interacts with profile detection and what the user should do.
Read the worked answer
Construction geometry is intentionally excluded from profile generation. If the symmetry line was created with the normal Line tool and never toggled to construction, Fusion treats it as real sketch geometry, and a line crossing a closed region splits that region into two separate profiles. The extrude then sees two profiles instead of one, and a single-profile selection may fail or produce unexpected results.
What to do:
- Select the symmetry line and enable Construction in the Sketch palette (or use the construction toggle).
- Confirm the line changes to a dashed appearance.
- Re-select the profile; the region should now highlight as one continuous area.
- If multiple profiles still appear, use the profile selector to pick the correct one explicitly.
The broader judgement: construction geometry is a semantic flag, not a visual style. A line that looks like a centerline but is not flagged as construction will alter topology. Users should adopt the habit of toggling construction at creation time for reference geometry.