- Which Bottom Height offset produces the required final depth?
Answer: Use an offset of −8 mm because the final level is 8 mm below the selected contour.
When working with Bottom Height in Fusion 360's 2D Contour operation, the key concept is understanding how offsets work relative to a selected reference. The offset you enter is a signed distance added to the reference level — positive moves the boundary upward, negative moves it downward.
Here, the selected contour (your reference) sits at Z=0 mm, and you need the tool to reach Z=−8 mm. The math is straightforward: Target=Reference+Offset, so −8=0+Offset, giving an offset of −8 mm. That's exactly what D describes — the final level is 8 mm below the selected contour, requiring a −8 mm offset.
A is wrong because Fusion 360 does not use a positive value to represent downward depth in the Bottom Height offset field. Entering +8 mm would actually raise the bottom boundary 8 mm above the reference, resulting in no material removal at all in this case. B introduces a fabricated rule — Fusion 360 does not double-apply the offset when multiple depths are enabled; each pass stays within the defined boundary as expected. C is tempting but incorrect: "From selected contour" sets the reference point, not the final depth. Without a −8 mm offset, the boundary stays exactly at Z=0 mm, and nothing gets cut.
A reliable tip: whenever a Bottom Height question gives you a target Z-value and a reference Z-value, just subtract — offset equals target minus reference. Keep your sign conventions consistent and you'll avoid the trap that catches most students on A. - After the Face operation completes, what condition should be expected on the top of the model?
Answer: The tool stops 0.15 mm above model top because the positive offset raises the bottom reference level.
When configuring Heights in Fusion 360's CAM environment, each height reference defines a boundary for tool movement — and offsets shift that boundary, not the cutting depth relative to it. The critical insight here is that Bottom Height defines where the tool stops, so a positive offset raises that stopping point upward from the reference.
In this setup, Bottom Height is set to Model top with a +0.15 mm offset. That means the tool's lowest cutting position is Model top plus 0.15 mm — in other words, the tool halts 0.15 mm above the model surface. The stock starts 1.20 mm above model top, so the Face operation clears down to 0.15 mm above the model, leaving a thin layer of material. Answer B correctly captures this behavior.
A is wrong because disabling axial stock to leave does not override the Bottom Height setting. Axial stock to leave is a separate finishing allowance; the Bottom Height offset independently controls where the tool stops. C reverses the offset direction — a positive Bottom Height offset raises the floor, it does not cause the tool to cut deeper than the reference. D confuses the stock height with the offset calculation; the 1.20 mm stock height describes where cutting begins (Top Height: Stock top), not where it ends. You don't sum those two values to find the stopping point.
As a study tip: always trace the tool path from Top Height down to Bottom Height. Ask yourself, "Does this offset push the floor up or down?" Positive = floor rises = less material removed. - Which pair of settings should the machinist evaluate first?
Answer: Reduce optimal load for lower radial engagement, then set maximum roughing stepdown for the axial depth.
When working with 2D Adaptive Clearing in Fusion 360, you need to understand two distinct axes of control: radial engagement (how much the cutter engages sideways) and axial depth (how deep each pass cuts). Keeping these two concepts separate is the key to answering this question correctly.
In Adaptive Clearing, the Optimal Load parameter directly controls radial cutter engagement — it defines the maximum width the cutter engages the material. To reduce radial engagement and protect the cutter in corners, you reduce the Optimal Load. The Maximum Roughing Stepdown then controls how deep each axial pass goes, allowing you to take deeper cuts within the 10 mm pocket while keeping radial forces manageable. This makes B the correct pairing: reduce Optimal Load for radial control, set Maximum Roughing Stepdown for axial depth.
A is a trap because it says to increase Optimal Load — that would increase radial engagement, the opposite of the goal. C confuses Adaptive-specific parameters with finishing and entry parameters. Finishing Stepover applies to contour or parallel finishing passes, not adaptive roughing, and Lead-In Radius controls tool entry geometry, not axial depth. D is similarly off-track: Tolerance controls calculation accuracy and path smoothness, not radial engagement, and Stock to Leave defines remaining material for finishing — neither addresses the stated goals.
A useful rule of thumb: in Adaptive Clearing questions, mentally separate "how wide?" (Optimal Load) from "how deep?" (Roughing Stepdown). Any answer that swaps, mislabels, or substitutes unrelated parameters for these two is a distractor. - Which operation plan best follows a basic, efficient CAM workflow?
Answer: Face the top to establish the reference surface, use 2D Adaptive Clearing with stock to leave for the pocket, then use 2D Contour on the external wall to finish at nominal size.
When planning a CAM workflow in Fusion 360, think sequentially: establish your reference surface first, then rough internal features with material to spare, then finish external features to size. This logical order minimizes rework and protects finished surfaces.
Option C follows this exact logic. Facing the top first creates a flat, accurate datum for all subsequent operations. Next, using 2D Adaptive Clearing with stock to leave on the pocket removes bulk material efficiently while preserving a finishing allowance — exactly what the passage requires. Finally, 2D Contour on the external wall brings the perimeter to nominal size in a controlled finishing pass. Each step builds on the last without contradicting it.
Option A fails immediately by starting with adaptive clearing on the external wall — you'd be roughing the perimeter before even establishing the top surface, leaving the part without a reliable reference. Using contour with tabs on the pocket is also unconventional for a simple roughing scenario and ignores the logical sequencing.
Option B compounds errors by contouring the external wall first (finishing before roughing the pocket), then facing below the model top, which is backwards — facing should come first to establish your reference, not last to clean up.
Option D introduces unnecessary complexity by applying radial stock to leave during facing, which protects nothing meaningful on a top-facing pass. Contouring the pocket floor without first clearing it volumetrically skips the bulk material removal entirely.
As a study tip, remember the general CAM rule of thumb: reference → rough → finish. If an answer reverses this order or skips roughing before finishing, it's almost always wrong.
- Which settings address these two requirements respectively?
Answer: Use Multiple Depths for axial levels and Roughing Passes for additional lateral offsets.
When configuring a 2D Contour operation in Fusion 360, it helps to separate the two axes of cutting control: axial (depth, Z-axis) and lateral (radial, XY-plane). Questions like this test whether you know which setting controls which direction.
Multiple Depths is the setting that divides the total cut depth into several smaller axial steps, allowing the tool to step down incrementally until it reaches the final depth — exactly what you need for a deep external wall. Roughing Passes adds one or more extra lateral (radial) offset passes before the final wall pass, leaving a small amount of material that the finishing pass then cleans up. Together, these two settings address both requirements, making C the correct answer.
Answer A is wrong because Finishing Overlap controls how much a tool overruns the start point at the end of a contour (to close a loop cleanly), and Lead-in Sweep Angle governs the arc angle of the tool's entry move — neither manages axial stepping or extra lateral passes. Answer B reverses the two correct settings — Roughing Passes handles lateral offsets, not axial levels, and Multiple Depths handles axial levels, not lateral offsets. Swapping them reflects a common mix-up. Answer D introduces two unrelated settings: Pass Extension lengthens the tool path beyond the contour endpoint, and Ramp Clearance Height controls safe height during ramp entries — neither addresses depth stepping or lateral roughing.
A useful memory trick: "Multiple = More Depth" (axial) and "Roughing = Radial buffer" (lateral). Keeping axial and lateral controls mentally separated will help you quickly eliminate distractors on any toolpath settings question.
- Which toolpath modification best meets both requirements?
Answer: Enable tabs on the selected contour and size them to leave several controlled bridges around the profile.
When machining a full-profile 2D Contour on sheet stock, you're balancing two competing demands: cut the part to full depth and keep it from falling free or shifting during the operation. The feature designed exactly for this scenario is tabs (sometimes called bridges).
Tabs are small, uncut sections distributed around the contour profile. Fusion 360 automatically lifts the tool over these regions, leaving thin bridges of material that physically anchor the part to the surrounding stock. Once machining is complete, you snap or cut the tabs manually. This directly satisfies both requirements — full-depth profiling everywhere except the tab locations, and the part stays securely in place. Answer A is the correct choice.
B is wrong because "radial stock to leave" offsets the entire contour wall outward, meaning the profile is never cut to the correct dimension. It doesn't selectively retain the part; it simply under-cuts the whole feature and leaves a continuous wall you'd then have to remove in a secondary pass — adding steps and dimensional risk.
C fails because raising the Bottom Height means the floor beneath the part remains uncut, so the part is held by an uncontrolled thin skin of material across the entire base, not discrete retention points. This can cause deflection, vibration, or an inconsistent final cut — and the part still isn't machined to true full depth.
D is a misconception about lead-out moves. Lead-outs control how the cutter exits the material; increasing lead-out distance doesn't skip or bridge sections of the profile — it just changes the retract path.
Remember: whenever a question mentions keeping a part attached to stock mid-operation, think tabs/bridges first — that's their sole purpose in Fusion 360's CAM environment.
- Which configuration best targets only the material left by the larger tool?
Answer: Enable rest machining based on previous operations and retain the pocket as the machining region.
When a larger tool leaves unmachined material in tight corners, Fusion 360's rest machining feature is exactly the right tool to reach for. Rest machining tells a subsequent operation to ignore already-cleared areas and focus only on the stock that the previous (larger) tool couldn't reach — saving significant cycle time and preventing unnecessary re-cutting of open areas.
Answer A is correct because enabling rest machining "based on previous operations" causes Fusion 360 to automatically calculate the remaining material left by the 12 mm end mill. The 6 mm tool then targets only those corner remnants within the same pocket boundary — precisely the behavior the scenario demands.
Answer B describes a workaround that doesn't actually work. Reducing optimal load changes the engagement angle of an Adaptive path, but it won't intelligently isolate corner remnants — the toolpath would still attempt to cover regions that are already clear, just with lighter cuts. You'd waste time and add unnecessary passes.
Answer C confuses rest machining with depth control. Multiple depths with a stepdown value controls how deep each pass goes in Z, not where the tool engages in XY. Using the prior tool diameter as a stepdown is also conceptually meaningless for isolating corner material.
Answer D mixes up two unrelated features. "Stock to leave" adds a deliberate offset of remaining material for a finishing pass — it doesn't use a previous operation as a boundary definition, and it wouldn't target corner remnants automatically.
Study tip: Whenever a question mentions a smaller tool cleaning up after a larger one, think "rest machining" immediately — it's Fusion 360's dedicated solution for this exact scenario. - Which Face-operation geometry strategy most directly ensures that the passes cover the required area?
Answer: Select the stock perimeter as the face boundary and use enough pass extension for complete edge cleanup.
When setting up a Face operation in Fusion 360, the core principle is simple: the boundary you select defines where the cutter is allowed to travel. If your stock extends beyond your model, you need to explicitly tell the CAM system about that larger area — it won't infer it automatically from the model geometry alone.
Since the stock extends 3 mm past every side of the model, selecting the stock perimeter as your face boundary directly communicates the true extents of the material that needs machining. Adding appropriate pass extension on top of that ensures the cutter fully cleans up the edges without leaving uncut witness marks. This is exactly what A describes, making it the most direct and reliable solution.
B is a trap — changing the Bottom Height controls the depth of the operation, not its horizontal extents. Lowering it won't push the cutter laterally out toward the stock edges.
C misunderstands what stepover does. Maximum stepover controls the spacing between parallel passes, not the outer boundary of where passes begin and end. Increasing it would actually reduce coverage density, potentially leaving strips unmachined rather than extending reach to the stock edges.
D conflates two unrelated settings. "Bottom reference" is a depth parameter, and "axial stock to leave" refers to leaving material in the Z-axis direction — neither of these expands the horizontal face boundary to cover the overhanging stock.
Study tip: In Fusion 360 CAM, always match your boundary selection to the actual material footprint. When stock exceeds the model, select stock geometry — not model geometry — as your boundary reference. - What is the most direct correction before changing compensation or tool data?
Answer: Reverse the selected contour side or direction so the cutter is generated outside the chain.
When a 2D Contour operation places the cutter on the wrong side of a chain, the issue is almost always about cutter side assignment — Fusion 360 uses the direction of the selected chain to determine whether the tool compensates to the left or right, which ultimately decides inside versus outside placement. This is the core concept being tested here.
The most direct fix is D: reversing the contour side or direction. In Fusion 360's 2D Contour, you can explicitly flip which side of the chain the tool follows without reselecting geometry or touching any other parameter. This immediately moves the cutter centerline from inside to outside the profile, which is exactly the symptom described.
Choice A is wrong because switching to a Face operation changes the machining strategy entirely — Face is for surfacing flat stock tops, not profiling external contours. It doesn't solve a side-assignment problem.
Choice B is incorrect because Bottom Height controls the depth of the cut, not which side of the chain the tool is on. Changing it to Stock bottom affects Z-axis behavior and has no influence on radial cutter placement.
Choice C is a tempting workaround — increasing radial stock to leave by one tool radius would push the toolpath outward — but this is a compensation hack, not a correction. The question explicitly asks for the fix before changing compensation or tool data, and this approach would also leave incorrect stock on the part rather than cutting to the true profile dimension.
Study tip: In Fusion 360 contour questions, always ask yourself direction → side → offset in that order. Cutter-on-wrong-side problems are solved by reversing direction first, not by tweaking offsets.
- Which compensation type is most appropriate?
Answer: Use Wear so Fusion calculates the nominal path and the controller applies a small wear correction.
When working with cutter compensation in Fusion 360's 2D Contour, the key question is always: who does what? Fusion can calculate the full offset (computer), split the work with the controller (wear), leave everything to the controller (control), or output no offset at all (off). Understanding this division of responsibility is essential here.
The scenario asks for Fusion to calculate the nominal cutter path while still leaving the operator room to dial in small diameter corrections at the machine controller — without regenerating the toolpath. That's exactly what Wear compensation does. Fusion computes the toolpath based on the nominal tool diameter, then the controller applies only a tiny residual correction (typically a few thousandths) stored in an offset register. This is the standard shop-floor workflow for maintaining dimensional tolerance through a tool's life.
A is wrong because "In computer" means Fusion calculates and bakes in the complete cutter-radius offset. The controller outputs the path as-is, so there's no register value for the operator to tweak — defeating the entire purpose of the scenario.
C ("Off") outputs the raw part profile coordinates with no offset applied anywhere. The controller doesn't "infer" anything; you'd simply cut undersized. This option is essentially no compensation at all.
D flips the roles entirely — describing something closer to "Control" mode, where the controller handles the full nominal offset. That's the opposite of what the question describes, and it misrepresents how Fusion's compensation types actually divide the work.
As a study tip, memorize the Wear = Fusion handles nominal, controller handles the small remainder split. Exam questions on this topic almost always hinge on that specific division of labor.
