The Disappearing Sketch Geometry After a Parameter Change
A designer is building a mounting plate in Fusion. The base sketch was created on the XY plane and includes a rectangle whose width is driven by a user parameter called plateWidth, currently set to 120 mm. After the model is complete, the designer edits plateWidth to 60 mm in the Parameters dialog. The sketch reports no errors, but the downstream extrude feature turns yellow in the timeline. Clicking the warning shows that the profile it referenced no longer exists. The designer also notices that a fillet applied to the plate's long edge looks distorted. The browser shows the sketch and extrude as separate features, and the timeline has no unresolved red errors.
1. Explain why the extrude feature lost its profile reference even though the sketch itself reports no error, and describe how the designer should investigate the cause.
Read the worked answer
The sketch is geometrically valid at 60 mm, so Fusion does not flag it. The failure is a topological reference loss: the extrude stored a reference to a specific profile region, and when the parameter shrank the rectangle, that region either changed identity or collapsed in a way the stored reference could not resolve.
The investigation should proceed in order:
- Open Edit Feature on the extrude and inspect the Profile selection. A lost reference usually shows as empty or highlighted in red.
- Re-select the profile and confirm the extrude preview rebuilds.
- Check the timeline for the yellow warning icon and read the full message rather than assuming it is a geometry error.
- Roll the end-of-part marker back before the extrude to confirm the sketch at 60 mm actually produces the profile the extrude expects.
- Verify that no construction geometry or projected edges were deleted or merged during the parameter change.
The key judgement is that a healthy sketch does not guarantee healthy downstream references. The designer should look at the consumer feature, not keep re-editing the sketch.
2. The fillet on the long edge now looks distorted. What is the most likely reason, and what is the correct fix?
Read the worked answer
The fillet was almost certainly applied to an edge whose length or adjacent face geometry changed when the plate narrowed. A fillet radius that was valid on a 120 mm plate may now exceed the available material on one side, or the edge may have been split or merged, so the fillet re-solves against different topology.
Correct fix sequence:
- Edit the fillet and check whether the selected edge still resolves cleanly; if the edge is highlighted as missing, re-select it.
- Confirm the radius is still smaller than the shortest adjacent face dimension at 60 mm.
- If the radius is too large, either reduce it or make it parameter-driven so it scales with
plateWidth. - Reorder if needed: a fillet placed before a feature that changes the edge will behave differently than one placed after.
The judgement being tested is that parameter changes propagate topology changes, and downstream features must be evaluated for geometric feasibility, not just for reference validity. The designer should also consider adding the fillet radius as a derived parameter so future width changes do not silently break it.