Autodesk Fusion 360 Quiz: Extrude

10 questions · exam conditions

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ExtrudeQuestion 1 of 10

A sketch contains two closed rectangular profiles. The first lies over an existing solid, while the second is remote from it. Only the remote profile is selected, and its extruded volume will remain separated from every existing body by a gap.

Which Extrude operation will create valid solid geometry while keeping the result in the current component?

Join, because any extrusion created in the same component merges automatically

Cut, because the separated extrusion does not overlap material to remove

New Body, because the extrusion does not intersect an existing solid

Intersect, because only geometry outside the existing solid must be retained

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Autodesk Fusion 360 Quiz

Autodesk Fusion 360 Quiz: Extrude

Practice Extrude 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 Extrude, 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

Which Extrude operation will create valid solid geometry while keeping the result in the current component?

Join, because any extrusion created in the same component merges automatically
Cut, because the separated extrusion does not overlap material to remove
New Body, because the extrusion does not intersect an existing solid (correct answer)
Intersect, because only geometry outside the existing solid must be retained

Explanation: When working with Fusion 360's Extrude operation, the key question to ask is: what is the spatial relationship between the new extrusion and existing bodies? Each operation type — Join, Cut, New Body, Intersect — is only valid when the geometry satisfies specific conditions. In this scenario, the extruded profile is completely remote from any existing solid, with a gap separating them. New Body is the correct choice (C) precisely because the extrusion has no geometric relationship with existing solids. Fusion 360 creates it as an independent solid body within the same component, which is perfectly valid and intentional when bodies don't touch. Here's why the distractors fail: A (Join) is wrong because Join requires the new extrusion to share a face or overlap with an existing body — it literally merges volumes. If there's a gap, Fusion 360 will reject the Join operation outright since there's nothing to merge with. B (Cut) is invalid for the same geometric reason: Cut removes material from an existing body, but the extrusion doesn't intersect any existing solid, so there's no material to subtract — Fusion 360 will throw an error. D (Intersect) is the most misleading distractor — it retains only the overlapping volume between the new extrusion and existing bodies. Since there's no overlap at all, the result would be empty geometry, which is invalid. A useful rule of thumb: whenever your new extrusion is spatially isolated from all existing bodies, New Body is your only valid solid option. Think of Join, Cut, and Intersect as operations that require geometric contact to function.

Question 2

An enclosure body and a nearby support body both pass through the volume of a proposed vent extrusion. The vent must remove material from the enclosure without modifying the support.

Which Extrude configuration most reliably produces the required result?

Use Cut and specify only the enclosure under Objects to Cut (correct answer)
Use Join and specify only the support under Objects to Join
Use New Body and hide the support before completing the feature
Use Intersect and specify only the enclosure as the target body

Explanation: Whenever you see a Fusion 360 question about cutting material from specific bodies in a multi-body design, the key concept is selective Boolean operations — Fusion 360 lets you target exactly which bodies participate in any given extrude operation. The Cut operation with a manually specified target list is precisely the tool built for this scenario. By choosing Cut and selecting only the enclosure under "Objects to Cut," you remove material exclusively from that body. The support body is never touched because it was never included in the operation's target list. This is the most reliable, explicit, and non-destructive approach — answer A is correct. Each wrong answer breaks down for a specific reason. B uses Join, which adds material rather than removes it, so it cannot create a vent cutout at all — and targeting the support would merge geometry you want to keep separate. C uses New Body, which creates an independent solid from the extrusion profile rather than cutting anything; hiding the support is a display toggle, not a protection mechanism, and the vent geometry still won't be subtracted from the enclosure. D uses Intersect, which retains only the overlapping volume between the extrusion and the target body — this would destroy most of the enclosure rather than just punching a hole through it. As a study tip, always remember: in Fusion 360's multi-body environment, Cut + explicit body selection = surgical precision. Whenever a question describes a scenario where one body must be modified but a neighboring body must not, look immediately for the option that uses Cut with a restricted "Objects to Cut" list.

Question 3

A mounting rib must extend from its sketch plane until it reaches a planar face on another body. The location of that face may change when upstream dimensions are edited, and the rib must continue to terminate on it.

Which extent setting best captures this design intent?

Distance, using the currently measured separation between the sketch and face
To Object, selecting the planar face with a zero offset (correct answer)
All, extending the rib through every body in that direction
Distance, using half the separation and enabling Symmetric direction

Explanation: When working with extrusion extents in Fusion 360, the core question to ask yourself is: does this feature need to adapt automatically when the model changes, or is a fixed value acceptable? Design intent questions always push you toward adaptive, parametric solutions. The To Object extent (answer B) is purpose-built for exactly this scenario. By selecting the planar face directly, Fusion 360 creates a live reference — if that face moves because an upstream dimension changes, the rib's termination follows it automatically. A zero offset means the rib terminates flush against the face with no gap or overlap, perfectly honoring the requirement. Here's why the other options fall short. A hardcodes the current distance as a fixed number. The moment any upstream edit shifts that target face, your rib either falls short or passes through it — the design intent is immediately broken. C uses the All extent, which extends the rib through every body in that direction. This is useful for cuts that must pass through everything, but for a rib that should stop precisely at one face, it's far too blunt and doesn't respect the specific termination target. D combines a fixed distance with Symmetric direction, which spreads the feature equally in both directions from the sketch plane — doubly wrong, since it both hardcodes a value and changes the geometry's direction entirely. Study tip: On Fusion 360 exam questions, whenever you see phrases like "may change" or "continues to terminate on," flag them as design intent triggers. That language signals you need a reference-based extent like To Object, not a static Distance value.

Question 4

A profile is sketched on an internal reference plane. It must cut $8\,\text{mm}$ toward Side 1 and $3\,\text{mm}$ toward Side 2. The depths must remain independently editable in one Extrude feature.

Which setup satisfies the requirement?

Symmetric direction, Distance extent, and a total distance of $11\,\text{mm}$
Two Sides direction, separate distances of $8\,\text{mm}$ and $3\,\text{mm}$ , and Cut (correct answer)
One Side direction, a distance of $8\,\text{mm}$ , and a start offset of $3\,\text{mm}$
Two Sides direction, separate distances of $8\,\text{mm}$ and $3\,\text{mm}$ , and Join

Explanation: When working with Extrude features in Fusion 360, the key question to ask is: how many independently controllable directions does this cut require? Here, you need

8\,\text{mm}

in one direction and

3\,\text{mm}

in the other — two distinct, editable values — from a single sketch profile on an internal plane. The Two Sides direction setting is exactly designed for this scenario. It exposes two separate distance fields, letting you specify

8\,\text{mm}

toward Side 1 and

3\,\text{mm}

toward Side 2 independently. Pairing that with the Cut operation removes material in both directions, which is precisely the requirement. That makes B the correct answer. A fails because Symmetric extrudes both sides by the same distance — half of the total value each way. A total of

11\,\text{mm}

would cut

5.5\,\text{mm}

per side, which is neither

8

nor

3\,\text{mm}

, and the two sides cannot be edited independently. C uses One Side direction with a start offset. A start offset shifts where the extrusion begins, but the feature still cuts in only one direction from that offset point. You cannot independently control depth on both sides this way. D is almost correct in setup — Two Sides with

8\,\text{mm}

and

3\,\text{mm}

— but uses Join instead of Cut. Join adds material; it does not remove it. Since the requirement is a cut, this operation type is wrong. A useful habit: always identify both the direction setting and the operation type in any Extrude question. They are independent choices that must both match the design intent.

Question 5

A boss profile is sketched on a construction plane located $4\,\text{mm}$ below the top face of a block. The boss must begin at the block's top face, not at the sketch plane, and then extend $10\,\text{mm}$ outward.

Which Extrude start configuration best avoids creating geometry in the $4\,\text{mm}$ gap?

Start from Profile Plane and increase the extrusion distance to $14\,\text{mm}$
Start from Offset and enter an offset of $4\,\text{mm}$
Start from Object, select the top face, and extrude $10\,\text{mm}$ (correct answer)
Start from Profile Plane and use To Object targeting the top face

Explanation: When working with Fusion 360's Extrude command, the Start option controls where the extrusion originates — which is completely independent of where you drew the sketch. Whenever the sketch plane doesn't coincide with your intended starting surface, you need to deliberately redirect that origin point, or you'll generate unwanted geometry in the gap between them. The cleanest solution here is C: using Start from Object and selecting the top face of the block. This anchors the extrusion exactly at the top face, completely skipping the

4\,\text{mm}

gap, and then the

10\,\text{mm}

distance projects outward from there — precisely the geometry you want, nothing more. A is a common workaround attempt, but it creates real problems: extruding

14\,\text{mm}

from the sketch plane does reach

10\,\text{mm}

beyond the top face, but it also fills the $4\,\text{mm}$ gap below the top face with solid geometry — the opposite of the goal. B sounds promising, but Start from Offset shifts the start plane by

4\,\text{mm}

relative to the sketch plane, which technically starts at the top face. However, this is fragile: if the sketch plane position ever changes, the offset must be manually updated. More critically, it introduces unnecessary dependency rather than directly referencing the face as the true design intent. D misuses To Object, which is an end condition, not a start condition. It controls where the extrusion stops, not where it begins. As a study tip: whenever start and end geometry don't align with your sketch plane, always look to Start from Object first — it's the most direct, parametrically stable way to reference real model faces.

Question 6

A clearance opening must remove material through all stock encountered in one direction. Future edits may increase the stock thickness, and the design intent must not depend on selecting a particular rear face as the termination reference.

Which Extrude configuration most directly represents this intent?

Cut with Distance set slightly greater than the stock's current thickness
Cut with Symmetric direction and the current stock thickness entered
Join with All as the extent in the required extrusion direction
Cut with All as the extent in the required extrusion direction (correct answer)

Explanation: When working with Fusion 360's Extrude feature, questions about design intent and future-proofing come down to choosing an extent type that remains valid regardless of how the model changes later. Ask yourself: will this configuration still work correctly if someone edits the stock thickness tomorrow? The All extent tells Fusion 360 to cut through every body it encounters in the specified direction, no matter how thick that geometry is. This directly satisfies both conditions in the passage — material is removed through all stock, and the cut automatically adapts if thickness changes. No face selection is required as a termination reference, so the design intent is fully parametric. D is the correct answer. A fails because hardcoding a distance "slightly greater than current thickness" is fragile. If the stock gets thicker in a future edit, the cut may no longer penetrate fully, breaking design intent. This is exactly the scenario the passage warns against. B is doubly wrong. Symmetric extrudes material in both directions from the sketch plane, which doesn't match a clearance cut intended to go in one direction only. It also relies on entering a specific thickness value, reintroducing the same future-edit vulnerability as A. C uses the correct extent type (All) but selects Join instead of Cut. Join adds material rather than removing it, which is the opposite operation from creating a clearance opening through existing stock. As a study tip: whenever a passage emphasizes that a feature must survive future geometry changes without manual re-selection, that's your cue that All (or a similar through-all extent) is the intended answer — hardcoded distances and face references are maintenance traps in parametric modeling.

Question 7

An Extrude feature was created with the operation explicitly set to New Body. At creation time, the result did not touch any other body. An upstream dimension is later changed so that the extruded volume now overlaps an existing body.

Assuming the feature still regenerates successfully, what is the expected result?

Fusion changes the operation to Join and combines the overlapping solids automatically
Fusion preserves New Body, so the bodies remain separate even where they overlap (correct answer)
Fusion changes the operation to Cut because the new volume enters existing material
Fusion suppresses the feature because New Body cannot overlap another body

Explanation: When you assign an explicit operation type to a Fusion 360 feature, that assignment is sticky — Fusion 360 respects your intent and does not silently reassign the operation just because the geometry changes during parametric updates. This question tests whether you understand how operation types behave when upstream parameters cause new geometric relationships. Since the Extrude was explicitly set to New Body, Fusion 360 preserves that setting even after the dimension change causes overlap. The two solids will occupy the same space simultaneously, resulting in intersecting geometry, but they remain distinct bodies in the browser. Fusion will not auto-correct your design intent. Answer B is correct. A is wrong because Fusion 360 does not automatically promote an operation to Join when overlap occurs. Join must be explicitly selected by you; the software does not assume that overlap means you want a union. C is wrong for the same reason — Fusion does not reinterpret overlapping entry into existing material as a Cut. Cut must also be intentionally assigned. Both A and C describe behaviors that would require Fusion to override your stated intent, which it does not do. D is wrong because overlapping geometry does not cause a New Body feature to be suppressed; Fusion allows geometrically intersecting bodies to coexist — it simply flags them or shows the overlap visually, but regeneration still succeeds. As a study tip: on Fusion 360 exam questions, remember that explicit operation types are honored parametrically. If geometry changes create unexpected overlaps, you are responsible for updating the operation — Fusion will not do it for you.

Question 8

A sketch contains two concentric closed circles. Fusion recognizes an inner circular profile and a separate annular profile between the circles. A hollow sleeve must be created as a separate body in one Extrude feature.

Which profile and operation should be used?

Select only the inner circular profile and set the operation to New Body
Select both recognized profiles and set the operation to New Body
Select only the annular profile and set the operation to New Body (correct answer)
Select only the annular profile and set the operation to Join

Explanation: When working with Extrude in Fusion 360, the key skill is understanding how Fusion recognizes profiles from sketch geometry and how the operation type controls body creation. Two concentric circles produce exactly two selectable profiles: the filled inner circle and the annular (ring-shaped) region between the two circles. Your goal is to match the correct profile to the shape you actually want to build. For a hollow sleeve — a tube with empty space through its center — you need only the annular region. Selecting that profile and setting the operation to New Body creates an independent solid body shaped exactly like a ring or tube, which is precisely what answer C describes. This is the correct approach. Answer A fails because selecting only the inner circular profile extrudes a solid cylinder, not a hollow sleeve. The resulting body would have no hole through it, which is the opposite of what's needed. Answer B is a common trap. Selecting both profiles together extrudes a solid disc — Fusion fills the entire area covered by both profiles, effectively merging them into one solid cylinder. You lose the hollow center entirely. Answer D selects the correct annular profile but uses the wrong operation. Join merges the result into an existing body rather than creating a separate one. Since the problem explicitly requires a separate body, Join is disqualifying regardless of the profile choice. A useful rule of thumb: always ask yourself "what shape is my profile actually tracing?" and separately "what should happen to that shape relative to existing bodies?" Keeping profile selection and operation type as two distinct decisions will prevent most Extrude mistakes on this exam.

Question 9

A rectangular profile lies on the top face of an existing base. It must form a joined boss whose far face is smaller than its profile at the base. The side faces must draft uniformly inward by $3^\circ$ over an extrusion distance of $12\,\text{mm}$ .

Which Extrude settings produce the intended boss?

Join, distance $12\,\text{mm}$ , and a positive $3^\circ$ taper angle (correct answer)
Join, distance $12\,\text{mm}$ , and a negative $3^\circ$ taper angle
New Body, distance $12\,\text{mm}$ , and a positive $3^\circ$ taper angle
Cut, distance $12\,\text{mm}$ , and a negative $3^\circ$ taper angle

Explanation: When working with Fusion 360's Extrude command, you need to think about three independent decisions: the operation type (Join, Cut, New Body, etc.), the distance, and the taper angle sign convention. Getting all three right is what this question tests. A boss is a raised feature that joins onto an existing body, so the operation must be Join — this merges the new extrusion with the base solid seamlessly. The distance is straightforwardly given as

12\,\text{mm}

. The trickier decision is the taper angle sign. In Fusion 360, a positive taper angle causes the profile to draft inward as it extrudes away from the sketch plane — meaning the far face ends up smaller than the base profile. This matches exactly what the passage describes: a boss whose far face is smaller, with sides drafting uniformly inward by

3^\circ

. That makes A the correct answer. B is wrong because a negative

3^\circ

taper would cause the profile to draft outward, producing a boss that widens as it rises — the opposite of what is needed. C uses the correct distance and taper angle, but "New Body" creates a separate, disconnected solid rather than merging with the base, so you don't get a true joined boss. D specifies a Cut operation, which would remove material from the base rather than add a boss, and the negative taper compounds the error by flaring outward. A handy rule to memorize: in Fusion 360 Extrude, positive taper = inward draft (shrinks), negative taper = outward draft (grows). Pair this with operation type — Join for additive features, Cut for subtractive — and you can decode any similar question quickly.

Question 10

A sketch lies on the midplane of a part. A reinforcing extrusion must extend equally in both directions and have a total end-to-end length of $20\,\text{mm}$ .

Which Direction and Measurement settings achieve the requirement without calculating a half-distance?

Symmetric, Whole Length, with a distance of $20\,\text{mm}$ (correct answer)
Symmetric, Half Length, with a distance of $20\,\text{mm}$
Two Sides, with each side set to $20\,\text{mm}$
One Side, with a distance of $20\,\text{mm}$ and Join

Explanation: When working with extrusions in Fusion 360, the Direction and Measurement settings control both how the extrusion grows and what value you type in. Understanding these two independent controls together is key to answering questions like this efficiently. The goal here is a

20\,\text{mm}

total length extending equally in both directions from a midplane sketch — with no manual division required. Symmetric direction automatically mirrors the extrusion on both sides of the sketch plane, and pairing it with Whole Length means Fusion 360 interprets your typed value as the total end-to-end distance. So entering

20\,\text{mm}

gives you exactly

10\,\text{mm}

on each side — no arithmetic needed. That makes A the correct answer. Choice B is the classic trap here. Symmetric with Half Length still extends equally in both directions, but now your input represents only one side. Typing

20\,\text{mm}

would produce a

40\,\text{mm}

total extrusion — twice what you want — and it requires you to calculate half the target distance yourself, which the question explicitly asks to avoid. Choice C uses Two Sides, which does allow independent control of each direction, but you'd be entering

20\,\text{mm}

per side, yielding a

40\,\text{mm}

total — again double the requirement. Choice D, One Side, extrudes in only a single direction from the sketch plane, so the result would not be symmetric at all, violating the core requirement. A helpful memory rule: in Fusion 360, always confirm whether your measurement setting is "Whole" or "Half" before accepting a Symmetric extrusion — that single toggle is responsible for a 2× error if overlooked.