Autodesk Fusion 360 Quiz: Fixing Sketch Constraints
10 questions · exam conditions
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Fixing Sketch ConstraintsQuestion 1 of 10

A sketch uses projected geometry from an edge of an earlier feature. After that feature is edited, the edge is replaced by a different topological edge. The sketch reports a lost projection, and a downstream Pocket feature fails because its profile is incomplete.

Which workflow most appropriately repairs the model while retaining an associative reference?

Fix the remaining sketch geometry, then suppress the Pocket feature until the design is complete.
Break the link on every projected entity, then position the profile using approximate dimensions.
Redefine the sketch plane so the profile no longer depends on the edited feature.
Remove the unresolved projection, project a suitable replacement edge, and restore required constraints.
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Autodesk Fusion 360 Quiz

Autodesk Fusion 360 Quiz: Fixing Sketch Constraints

Practice Fixing Sketch Constraints in Autodesk Fusion 360 with focused quiz questions that help you check what you know, review explanations, and build confidence with test-style prompts.

What this quiz covers

This quiz focuses on Fixing Sketch Constraints, giving you a quick way to practice the rules, question types, and explanations that matter most for Autodesk Fusion 360.

How to use this quiz

Try each quiz question before looking at the correct answer. Use the explanations to review missed ideas, then come back to similar questions until the pattern feels familiar.

All questions

Question 1

A sketch uses projected geometry from an edge of an earlier feature. After that feature is edited, the edge is replaced by a different topological edge. The sketch reports a lost projection, and a downstream Pocket feature fails because its profile is incomplete.

Which workflow most appropriately repairs the model while retaining an associative reference?

  1. Fix the remaining sketch geometry, then suppress the Pocket feature until the design is complete.
  2. Break the link on every projected entity, then position the profile using approximate dimensions.
  3. Redefine the sketch plane so the profile no longer depends on the edited feature.
  4. Remove the unresolved projection, project a suitable replacement edge, and restore required constraints. (correct answer)
Explanation: When working with parametric models in Fusion 360, projected geometry creates associative links between a sketch and the edges or faces it references. When a feature edit changes the underlying topology — replacing one edge with another — those links break, leaving "lost projection" errors that cascade into downstream failures. Your goal when repairing these situations is always to restore the associative chain, not abandon it. The correct approach, D, does exactly this. You remove the unresolved (broken) projection to clean up the sketch, then re-project a valid replacement edge that now correctly represents the model's current topology. Finally, you restore any constraints (coincident, collinear, etc.) that relied on the old projection. This keeps the sketch parametrically live, so future edits to the referenced feature automatically update the sketch and the Pocket profile downstream. Choice A fails because suppressing the Pocket feature only hides the problem — it doesn't fix the broken projection, so the sketch remains incomplete and the suppression must eventually be undone, with the error still waiting. Choice B breaks associativity entirely by removing the link and replacing it with hard dimensions. You lose the adaptive behavior that makes parametric modeling powerful; any future upstream changes will no longer propagate correctly. Choice C — redefining the sketch plane — addresses where the sketch lives, not what it references. The missing profile geometry still won't exist on the new plane, so the Pocket profile remains incomplete. A useful rule of thumb: whenever you see a "lost reference" scenario, think replace the reference, not the feature. Preserving associativity is almost always the preferred repair strategy in parametric CAD workflows.

Question 2

An imported bracket outline was initially stabilized by applying Fix/UnFix to all sketch entities. The designer now needs to control the bracket width with a driving dimension, but Fusion reports that the new dimension would overconstrain the sketch.

What is the best first step toward a maintainable repair?

  1. Delete all existing dimensions while leaving every profile entity fixed in place.
  2. Unfix the geometry that must move, then constrain and dimension it according to design intent. (correct answer)
  3. Convert the proposed width dimension to driven so it can control the bracket indirectly.
  4. Suppress the downstream features, add the dimension, and then unsuppress the features.
Explanation: Whenever you see a Fusion 360 question about overconstraining sketches, think about the underlying constraint system: every entity needs exactly the right number of constraints — no more, no less. The goal is design intent, meaning your sketch should be structured so that changing one value predictably updates the model in a logical way. When a sketch is imported and stabilized with Fix/UnFix, every entity is essentially "nailed down" in place. Fusion treats Fix as a full constraint, so adding a driving dimension on top of that creates redundancy — hence the overconstrain warning. The correct repair is B: unfix the geometry you want to control, then apply proper geometric constraints and a driving dimension to define its position and size according to your design intent. This gives the dimension actual authority to move geometry, which is the whole point of a driving dimension. A is wrong because deleting all dimensions while leaving entities fixed doesn't solve anything — the fixed entities still can't move, so your driving dimension would still overconstrain or be meaningless. You'd lose existing constraints without gaining control. C is a common trap: converting a dimension to driven (reference) mode makes it a passive readout, not a controller. It reports a value but cannot drive geometry, so the bracket width still wouldn't be parametrically controllable. D is a workflow misconception — suppressing downstream features doesn't resolve a sketch constraint conflict; the sketch's constraint state is independent of whether features above it are suppressed. As a study tip, remember: Fix replaces all degrees of freedom. Before adding driving dimensions, always unfix what needs to move, then rebuild constraints intentionally.

Question 3

Two hole-center points are constrained Symmetric about a vertical construction centerline. Each point also has a separate horizontal distance dimension of 30 mm30\ \mathrm{mm} to that centerline. Editing either distance produces an overconstraint warning. The holes must remain symmetric and stay 60 mm60\ \mathrm{mm} apart.

Which constraint arrangement best captures the design intent without redundancy?

  1. Keep Symmetric and one 30 mm30\ \mathrm{mm} centerline distance; remove the other distance dimension. (correct answer)
  2. Remove Symmetric and keep both 30 mm30\ \mathrm{mm} centerline distance dimensions as independent controls.
  3. Keep Symmetric and both distance dimensions, but convert the construction centerline to normal geometry.
  4. Remove both distance dimensions and fix both hole centers at their current locations.
Explanation: Whenever you see a question about sketch constraints in Fusion 360, ask yourself: how many independent pieces of information are needed to fully define the geometry, and does each constraint add unique information or duplicate something already captured? Here, the Symmetric constraint already enforces that both hole centers are mirror images across the centerline — meaning if one point sits 30 mm30\ \mathrm{mm} from the centerline, the other is automatically 30 mm30\ \mathrm{mm} away as well. That single constraint encodes the relationship between both points simultaneously. Adding a second explicit 30 mm30\ \mathrm{mm} distance dimension to the mirrored point tells Fusion 360 something it already knows, creating redundancy and triggering an overconstraint warning. The fix in Answer A is elegant: keep Symmetric (which preserves the equal-distance relationship and keeps holes 60 mm60\ \mathrm{mm} apart) and retain only one 30 mm30\ \mathrm{mm} dimension to define the actual spacing. That single dimension still fully controls the design intent. Answer B is tempting but wrong — removing Symmetric means the two holes are no longer linked. You could accidentally move one without affecting the other, losing the mirrored relationship entirely. Answer C misunderstands the problem; converting the construction line to normal geometry doesn't resolve the overconstrained dimensions at all — the redundancy remains. Answer D using Fix constraints is a design-intent trap: fixing geometry locks points to absolute coordinates, making the sketch inflexible and difficult to modify later, which defeats the purpose of parametric modeling. As a study tip: in Fusion 360 sketching, Symmetric already encodes equality — any explicit dimension that repeats that equality is automatically redundant. Always ask what new information each constraint contributes.

Question 4

Changing a named width parameter causes a sketch warning and several downstream features to fail. The sketch contains Coincident, Equal, and dimensional constraints added at different stages. Returning the parameter to its previous value makes the model compute again.

What is the most reliable troubleshooting approach before deleting constraints?

  1. Delete all Equal constraints because dimensional constraints should always take priority over them.
  2. Suppress every failed downstream feature and leave the sketch unchanged at the old parameter value.
  3. Fix all underconstrained entities before attempting the parameter change a second time.
  4. Edit the sketch, identify the reported conflicting constraints, and replace only those that oppose the change. (correct answer)
Explanation: When Fusion 360 reports a sketch warning after a parameter change, it's signaling a constraint conflict — meaning some existing constraints mathematically contradict the new value. Your goal is surgical precision: resolve only what's broken without disturbing what's working. The most reliable path is D — edit the sketch, read the conflict indicators Fusion highlights (yellow or red entities), and selectively replace only the constraints that are fighting the parameter change. Fusion tells you where the problem is; your job is to interpret that information and make the minimum necessary edits. This preserves your design intent while allowing the parameter to drive geometry correctly. A is wrong because it assumes Equal constraints are inherently inferior to dimensional constraints — they're not. Equal constraints are legitimate design intent. Deleting all of them is destructive and may break geometry that was working perfectly fine. B is wrong because suppressing downstream features and reverting the parameter doesn't actually fix anything — it just hides the problem. You haven't resolved the conflict; you've postponed it. The moment you reintroduce the parameter change, everything fails again. C is wrong because the scenario describes a fully constrained sketch with conflicting constraints, not an underconstrained one. Fixing underconstrained entities addresses a different class of problem. Adding more constraints to an already-conflicted sketch can make things worse, not better. Study tip: On Fusion 360 exam questions involving constraint errors, watch for the distinction between underconstrained (not enough constraints) and overconstrained/conflicting (too many or contradictory constraints). The fix strategy is completely different for each.

Question 5

A circular arc is constrained Tangent to each of two parallel lines. The lines are dimensioned 20 mm20\ \mathrm{mm} apart, and the arc radius is dimensioned 10 mm10\ \mathrm{mm}. A revision changes the line spacing to 24 mm24\ \mathrm{mm}, causing a sketch conflict. The arc must remain tangent to both lines.

Which change resolves the conflict while preserving the stated design intent?

  1. Remove or revise the arc radius dimension so it is compatible with the new line spacing. (correct answer)
  2. Remove one Tangent constraint while retaining the fixed 10 mm10\ \mathrm{mm} radius.
  3. Keep all constraints and convert the 24 mm24\ \mathrm{mm} spacing dimension to driven.
  4. Fix the arc center and retain both Tangent constraints with the 10 mm10\ \mathrm{mm} radius.
Explanation: When a sketch has both driving dimensions and geometric constraints, they must all be mathematically consistent. Here, the tangency rule means the arc must simultaneously touch both parallel lines — which geometrically forces the arc's diameter to equal the line spacing. So if the lines are 24 mm24\ \mathrm{mm} apart, the radius must be 12 mm12\ \mathrm{mm}. The conflict arises because the old 10 mm10\ \mathrm{mm} radius dimension contradicts this reality. Answer A is correct because it targets the root cause: the radius dimension is now geometrically impossible given the new spacing and retained tangent constraints. Removing or updating the radius dimension (to 12 mm12\ \mathrm{mm}) eliminates the conflict while keeping both tangent relationships intact — which is exactly the stated design intent. Answer B fails because dropping one tangent constraint changes the design intent itself. The problem explicitly says the arc must remain tangent to both lines, so this is a non-starter regardless of whether the radius is preserved. Answer C is a common trap. Converting the spacing dimension to "driven" means Fusion 360 will display whatever value the geometry produces rather than enforcing it — but the conflict between the 10 mm10\ \mathrm{mm} radius and the two tangent constraints still exists internally. You'd still have an over-constrained or inconsistent sketch. Answer D fixing the arc center locks its position, which — combined with the 10 mm10\ \mathrm{mm} radius — makes it geometrically impossible to remain tangent to lines 24 mm24\ \mathrm{mm} apart. Study tip: In Fusion 360 sketches, always ask "what does the geometry require?" when a dimension conflict appears — constraints like Tangent impose hidden dimensional requirements that must align with your driving dimensions.

Question 6

A rectangular profile is fully constrained by its width, height, and position relative to the origin. A reviewer wants the diagonal length displayed for verification, but the diagonal must not control the rectangle or cause an overconstraint.

How should the diagonal dimension be added?

  1. Remove the width dimension and use the diagonal as a new driving dimension.
  2. Apply an Equal constraint to the sides before adding a driving diagonal dimension.
  3. Add the diagonal dimension and set it to Driven so it reports the resulting value. (correct answer)
  4. Fix the rectangle before adding the diagonal as another driving dimension.
Explanation: Whenever you encounter a Fusion 360 sketching question involving constraints and dimensions, the key distinction to understand is the difference between driving and driven dimensions. A driving dimension controls geometry — it defines the shape. A driven dimension (sometimes called a reference dimension) simply reports a value calculated from existing geometry without influencing it. In this scenario, the rectangle is already fully constrained by its width, height, and position. That means every geometric degree of freedom is already resolved. Adding another driving dimension on top of a fully constrained sketch would create an overconstraint, which Fusion 360 flags as an error. The solution is to add the diagonal dimension as a driven dimension — setting it to "Driven" mode in the dimension dialog. This way, Fusion 360 calculates and displays the diagonal value based on the existing width and height (essentially reporting d=w2+h2d = \sqrt{w^2 + h^2}), without attempting to control the geometry. A is wrong because removing the width dimension to replace it with the diagonal would change which dimensions drive the sketch, altering the design intent and making width no longer directly editable — a poor practice for a rectangle that needs to be defined by width and height. B is wrong because applying an Equal constraint before adding a diagonal driving dimension would force the rectangle into a square, which is an unintended geometric change. D is wrong because fixing the rectangle locks its position but doesn't resolve the overconstraint problem — you'd still be adding a redundant driving dimension. As a study tip: whenever a sketch is already fully constrained and you need a measurement for reference only, always reach for a driven dimension — it's Fusion 360's built-in tool for non-controlling annotations.

Question 7

A downstream Extrude uses a closed profile from a sketch. After a dimension is edited, the Extrude reports that no valid profile is available. In the sketch, the endpoint of one line appears to touch the endpoint of an adjacent arc, but the endpoints can be dragged apart independently.

What is the most direct repair for the sketch?

  1. Apply a Coincident constraint between the line endpoint and the arc endpoint. (correct answer)
  2. Apply a Tangent constraint between the entire line and the entire arc.
  3. Dimension the gap between the endpoints as 0 mm0\ \mathrm{mm}.
  4. Apply Fix/UnFix to both entities at their current displayed positions.
Explanation: Whenever you see a Fusion 360 sketch that looks closed but breaks an extrude, your first instinct should be to check geometric continuity — specifically whether endpoints that appear touching are actually constrained to share the same point, or are merely coincidentally positioned near each other. The scenario describes two endpoints that can be dragged apart independently. This is the classic symptom of a false closure: the endpoints are visually overlapping but have no geometric relationship forcing them together. When the dimension changes, the geometry shifts and the hidden gap is exposed, leaving the Extrude without a valid closed profile. The direct fix is to apply a Coincident constraint between the line endpoint and the arc endpoint, which forces them to occupy the exact same location regardless of how other dimensions drive the sketch. This is answer A, and it's the most direct, parametrically robust repair. Answer B is tempting but wrong — a Tangent constraint controls the angular relationship between two curves, ensuring smooth, direction-matching continuity. It does not force endpoints to merge; you can have tangency with a gap still present. Answer C is a trap. Dimensioning the gap as 0 mm0\ \mathrm{mm} adds a driven dimension but doesn't create a true geometric constraint. It may appear to work in one state but is fragile and not the proper Fusion workflow for closing a profile. Answer D, Fix/UnFix, locks entities in absolute space. It doesn't close the gap; it just freezes the problem in place, defeating the purpose of a parametric sketch. Study tip: In Fusion 360, always use constraints — not dimensions or visual proximity — to enforce profile closure. If an extrude suddenly loses its profile after an edit, open the sketch and look for missing Coincident constraints at endpoints.

Question 8

A closed profile was created by offsetting a fully constrained source loop by 2 mm2\ \mathrm{mm}. The offset geometry retains its Offset relationship. A user then adds separate length and position dimensions to each offset segment, after which the sketch becomes overconstrained.

Which repair best preserves a robust parametric offset?

  1. Delete the Offset relationship and control every offset segment with independent dimensions.
  2. Retain the Offset relationship and offset distance, removing dimensions that duplicate the derived geometry. (correct answer)
  3. Keep all dimensions but convert the fully constrained source loop into construction geometry.
  4. Fix every offset segment and remove the dimension defining the 2 mm2\ \mathrm{mm} distance.
Explanation: Whenever you see a question about parametric constraints in Fusion 360, think about the hierarchy of relationships: parent geometry drives child geometry, and the software tracks every degree of freedom. An Offset relationship is a derived constraint — it automatically defines the position, shape, and distance of the offset curve relative to its source. Adding independent dimensions on top of that derived geometry creates redundant constraints, which is exactly what causes the overconstrained state here. Retaining the Offset relationship and removing the conflicting dimensions — choice B — is the correct repair. The 2 mm2\ \mathrm{mm} offset distance is already a parameter you can edit globally. Keeping it means any future change to the source loop automatically propagates to the offset curve, which is the entire value of a parametric workflow. You eliminate overconstrained segments by trusting the relationship to do the work it was designed for. Choice A destroys the parametric chain entirely. Once you delete the Offset relationship, the offset profile becomes independent geometry, meaning source-loop changes will never update it — fragile and error-prone. Choice C misunderstands what construction geometry does: converting the source loop to construction removes it from the profile boundary but doesn't resolve the overconstrained offset segments, which still have conflicting dimensions. Choice D fixes (pins) the offset segments to absolute positions in space, eliminating adaptability and defeating the purpose of a parametric model; removing the 2 mm2\ \mathrm{mm} dimension afterward leaves you with immovable geometry and no editable driver. As a study tip: on Fusion 360 questions, always ask which constraint is the authoritative driver. Relationships like Offset, Equal, and Concentric are hierarchical — adding dimensions that restate what a relationship already defines is the classic overconstrain trap.

Question 9

A sketch contains a vertical construction line and a profile line. The profile line has both a Horizontal constraint and a Perpendicular constraint to the construction line. A design revision requires the profile line to be angled at 5∘5^\circ from horizontal while the construction line remains vertical.

Which edit best resolves the constraint conflict while preserving the revised design intent?

  1. Remove only the Horizontal constraint, then add the 5∘5^\circ angular dimension.
  2. Remove only the Perpendicular constraint, then add the 5∘5^\circ angular dimension.
  3. Remove both the Horizontal and Perpendicular constraints, then add the 5∘5^\circ angular dimension. (correct answer)
  4. Keep both geometric constraints and convert the 5∘5^\circ angular dimension to a driven dimension.
Explanation: When working with sketch constraints in Fusion 360, your goal is to always achieve a fully defined sketch with no conflicting constraints. The key principle: every geometric constraint you keep must be compatible with your intended geometry. Think of constraints as rules — if two rules contradict each other or contradict your dimension, they must both be removed before the dimension can do its job. Here, the profile line currently carries a Horizontal constraint (forces 0°0°) and a Perpendicular constraint to a vertical construction line (also forces 0°0°, since perpendicular to vertical = horizontal). These two constraints are actually redundant and both directly conflict with your new 5°5° intent. To place a valid 5°5° angular dimension, both geometric constraints must be deleted — which is exactly what option C does. Once freed, the angular dimension fully and cleanly defines the line's orientation. Option A fails because removing only the Horizontal constraint still leaves the Perpendicular constraint, which continues to force the line to 0°0° — the angular dimension would conflict with it or become driven (not driving). Option B has the same problem in reverse: removing only the Perpendicular constraint leaves the Horizontal constraint still locking the line at 0°0°, so your 5°5° dimension cannot drive the geometry. Option D is the worst choice — keeping both conflicting constraints and converting your dimension to driven means the dimension is just a passive readout, not controlling anything; the line stays horizontal. A useful rule of thumb: before adding a driving dimension, audit every existing constraint on that geometry and ask, "Does this constraint allow the value I want?" If not, delete it first.

Question 10

A designer trims a line at the corner of a closed profile. The Trim operation removes the original corner segment and one associated constraint. The profile works temporarily, but after a nearby dimension changes, the new endpoint separates from the adjacent line and the downstream Extrude fails.

What should the designer do to make the repair stable?

  1. Fix the trimmed endpoint at its current coordinates and leave the adjacent line unconstrained.
  2. Add a dimension between the separated endpoints using their current measured distance.
  3. Restore the Coincident relationship and any intended geometric constraint at the trimmed corner. (correct answer)
  4. Remove the nearby driving dimension so the endpoints cannot separate during future edits.
Explanation: Whenever you see a question about sketch failures after edits in Fusion 360, think about parametric constraints — the rules that hold geometry together when dimensions drive changes. A healthy sketch relies on constraints like Coincident (which forces two points to share the same location) rather than on geometry accidentally lining up at a fixed moment in time. Here's what happened in the scenario: Trim removed a corner segment and deleted its Coincident constraint. The sketch looked fine at that instant because the points happened to share coordinates — but when a nearby dimension changed, nothing was forcing those endpoints to stay connected. The result was a gap, and Extrude failed because the profile was no longer closed. The correct repair is C: restore the Coincident relationship so the endpoints are governed by a rule, not just a lucky coordinate match. If additional geometric intent existed at that corner (tangency, perpendicularity, etc.), restoring that too ensures the sketch behaves correctly under any future edit. A is wrong because fixing an endpoint locks it in place globally — it becomes immune to intentional design changes and creates rigidity that breaks parametric design intent. B is a subtler trap: adding a dimension between separated endpoints sets a distance, not a connection. A dimension of zero looks like it merges the points, but it doesn't create a topological link — the profile can still be open. D is counterproductive; removing driving dimensions reduces control rather than adding the stability the sketch needs. Your study takeaway: in Fusion 360, constraints define relationships, while dimensions define sizes. A missing constraint is never safely replaced by a coincidentally correct value — always restore the geometric rule.