What is CAD?

CAD stands for Computer-Aided Design. It's software that lets you create precise 3D models on your computer. Instead of sculpting freehand (like shaping clay), CAD uses exact measurements — you tell it "make a box 50mm × 30mm × 20mm" and it does exactly that.

Think of it this way: if you wanted to build a bookshelf, you could eyeball the cuts and hope they fit — or you could draw up exact plans first. CAD is the "draw up exact plans" approach, except the plans are the finished product. You design it on screen, then send it to a 3D printer to build it layer by layer.

For 3D printing, CAD is how you go from "I need a stand that holds my air purifier" to an actual file your printer can build.

Fusion vs The Others

Several free CAD tools exist. Here's how they compare for 3D printing work:

Why Fusion Wins for 3D Printing

• Parametric design — Change one dimension and the entire model updates. Measured your air purifier wrong? Just change the number, don't redraw. It's like a spreadsheet for shapes — change cell A1 and everything that references it recalculates.
• Free for personal use — The free license at autodesk.com/products/fusion-360/personal includes everything in this guide. You need to make less than $1,000/year from your designs (hobby use is fine).
• Direct STL/3MF export — Right-click a body → Save as Mesh. No plugins, no workarounds.
• Huge community — Thousands of tutorials on YouTube, active subreddit (r/Fusion360), Autodesk forums with staff answering questions.
• Industry standard — Skills transfer to professional work. Many product designers and engineers use Fusion daily.
• Cloud-based saving — Your designs save to Autodesk's cloud automatically. Switch computers and everything's still there. (You can also export local copies.)

What You'll Be Able to Make

After this guide, you'll have the skills to design:

Step-by-Step Installation

Free License Limits

The personal license is generous, but worth knowing the limits:

For hobby use, 10 active designs is plenty. Finished a project? Export the STL, set it to read-only, move on. You'll rarely have more than 5 active at once.

Other free license limits:

• No simulation/stress analysis (paid feature — you won't need it for printing)
• No generative design (AI-designed parts — cool but not necessary)
• Limited rendering styles (you're printing parts, not making marketing photos)
• No team collaboration features (fine for solo hobby use)

Initial Preferences Worth Changing

Two more settings worth changing while you're in there:

• Default units: Preferences → Design → Default Units → set to mm (millimeters). 3D printing lives in millimeters.
• Orbit type: Preferences → General → Default Orbit Type → "Constrained Orbit" keeps the ground at the bottom (less disorienting when you're learning).

The Four Core Gestures

You'll do these four things every 10–20 seconds while working. They need to feel like breathing.

The View Cube

In the top right corner of your canvas, there's a small 3D cube. This is the View Cube — your orientation compass. It shows which direction you're looking from.

• Click a face (Front, Top, Right, etc.) to snap to that exact view
• Click an edge to get an angled view between two faces
• Click a corner to see the isometric view from that angle
• Drag the cube to orbit freely (alternative to trackpad orbit)

Bottom Navigation Bar

At the very bottom of the screen, there's a thin bar with some important toggles:

• Grid — toggles the grid lines on the ground plane (helpful for orientation)
• Snap — makes your cursor snap to grid intersections (useful for rough alignment)
• Display Settings — wireframe, shaded, with/without edges. Leave on "Shaded with Visible Edges Only" for now.

The "Where Am I?" Panic Protocol

Every beginner gets lost in 3D space. Here's what to do when you can't see your model anymore:

1. Double-tap with two fingers → Zoom to Fit (brings your model back into view)
2. If that doesn't work, click the house icon next to the View Cube
3. If you still can't see anything, click "Top" on the View Cube to look straight down
4. If your model seems to have disappeared, check the Browser panel (left side) — is the body's eye icon (👁️) turned on?

Practice: Fly Around the Origin

Open a new design and spend 3–5 minutes just navigating. Seriously, don't skip this.

1. Pan around with two-finger scroll — move the colored origin lines around the screen
2. Zoom in and out with pinch — get close, then far away
3. Orbit with Shift + two-finger scroll — rotate all the way around. Try to look at the origin from the top, then the bottom, then from behind
4. Click Top on the View Cube, then Front, then Right
5. Double-tap with two fingers to zoom to fit
6. Click the house icon to reset

When these feel as natural as scrolling a web page, you're ready to move on.

The Five Zones

Fusion's interface has five main areas. You don't use every one constantly, but you need to know where they are.

Sketch Mode vs Model Mode

This confuses everyone at first. Understanding it now saves a lot of frustration later:

• 3D Mode Model Mode — the default. You see your 3D objects. The toolbar shows 3D tools (Extrude, Fillet, Shell). You can click on faces, edges, and bodies.
• Sketch Mode Sketch Mode — you enter this when you "Create Sketch" on a plane. The toolbar changes to 2D drawing tools (Line, Rectangle, Circle). The background may dim, and your view flattens to look at the sketch plane head-on.

Model Mode is your workshop — you work with 3D pieces. Sketch Mode is your drafting table — you draw flat blueprints. You bounce between them constantly.

Essential Keyboard Shortcuts

Nine shortcuts. That's it. These cover 90% of what you'll do:

Ready to Design? — Quick Quiz

Quick check before moving on. See if the interface basics stuck:

Sketch Mode 2D Sketch Tools

These tools work when you're in a sketch — drawing flat shapes on a plane. You'll use these to create the 2D "blueprints" that become 3D objects.

3D Mode 3D Modeling Tools

These tools turn flat sketches into solid objects, or modify existing 3D shapes. This is where your designs become real.

What is a Sketch?

A sketch is a 2D drawing on a flat plane. You draw shapes (rectangles, circles, lines), set their exact dimensions, then pull them into 3D with Extrude.

Think of it as drawing a blueprint on a sheet of paper, except the paper floats in 3D space. Once you're happy with the drawing, you pull it upward into a solid object. Sketch = recipe. Extrude = cooking.

Creating a Sketch

• XY plane (red-green) = Top-down view — most common for flat parts. Imagine laying a sheet of paper flat on a table.
• XZ plane (red-blue) = Front view — good for side profiles. Like a picture on a wall facing you.
• YZ plane (green-blue) = Side view — looking from the right side.

For your first sketch, click the XY (top) plane. Fusion zooms in and switches to sketch mode — you'll see the toolbar change to show sketch tools.

Understanding Constraints

Constraints are rules that lock parts of your sketch in place. Instead of hoping things stay aligned, you tell Fusion to guarantee it.

Fusion applies many constraints automatically — for example, when you draw a rectangle, it automatically makes the sides horizontal/vertical. You mainly need to add dimensions and position constraints manually.

Blue vs Black Lines — The Most Important Visual Cue

This color system tells you whether your sketch is "finished" or still needs work:

• Blue lines = under-constrained. Something isn't locked down. You can grab and drag these lines — they'll move. Dimensions or position constraints are missing.
• Black lines = fully constrained. Every dimension and position is defined. Nothing can shift. The sketch is "solved."

Practice: Centered Rectangle

1. Create a new sketch on the XY plane
2. Press R and draw a rectangle — click the origin point (where the red and green lines cross) as your first corner so it's pinned automatically
3. Set dimensions: press D, click the top edge, type 50. Click the side edge, type 30.
4. All lines should turn black — the sketch is fully constrained
5. Click "Finish Sketch" (green ✅ in the toolbar) or press Esc

Extrude — The Most Used Tool in All of CAD

Extrude grabs a 2D sketch profile and pulls it into 3D space. Like stretching taffy upward. Select a closed shape (your rectangle from Chapter 6), press E, and drag or type a distance.

• New Body — creates a separate solid (use for your first extrude on a blank design)
• Join — merges the new extrusion into an existing body (adds material)
• Cut — subtracts from an existing body (this is how you make holes!)
• Intersect — keeps only the overlap (rarely needed for beginners)

Direction options: One Side (default — extrudes one way), Both Sides (extrudes equally in both directions), or Symmetric (same as Both Sides).

Revolve

Revolve spins a sketch profile around an axis. Draw a half-cross-section, pick an axis line, and it spins it 360°. Pottery wheel for CAD.

Good for anything round: cylinders, tubes, vases, bowls, rings, handles.

Other 3D Tools

Practice: Make a Box

1. Use your 50mm × 30mm rectangle sketch from Chapter 6
2. Click inside the rectangle to select it (it highlights blue)
3. Press E to extrude
4. Type 20 for the height
5. Make sure Operation is "New Body"
6. Press Enter — you now have a 50 × 30 × 20mm box!

Orbit around it (Shift + two-finger scroll). That flat sketch is now a real 3D object. First time going from 2D to 3D. Feels good, right?

Fillet — Your Best Friend

Press F, then click any edge. Rounds it off with a smooth curve. Almost every printed part looks better with fillets. They're also structurally stronger — stress spreads across a curve instead of concentrating at a sharp corner.

Hold Cmd (Mac) and click multiple edges to fillet them all at once with the same radius.

Essential Modifiers Reference

Practice: Box → Rounded Tray

Turn your 50 × 30 × 20mm box into a rounded tray. This four-step workflow builds most functional parts:

1. Select the top four edges of the box (hold Cmd and click each edge)
2. Press F for Fillet. Set radius to 3mm. Press Enter.
3. Now go to Modify → Shell (or press S and search "Shell"). Click the top face of the box (this is the face that gets removed — the "opening" of the tray). Set wall thickness to 2mm. Press Enter.
4. You now have a tray with rounded edges and 2mm walls!

Calipers Are Your Best Friend

Before designing anything that fits around or into a real object, measure it with calipers. Digital calipers cost ~$10–15 online. Best $15 you'll spend on this hobby.

Measure everything: diameter, width, depth, screw hole sizes, cable diameters. Write them down before opening Fusion.

3D Printing Tolerances

3D printers aren't perfect. Molten plastic expands slightly when deposited and contracts as it cools. You add tolerance (extra space) to account for this:

Critical Print Rules

FDM printing has hard physical limits. Break these and your print fails or comes out fragile:

• Minimum wall thickness: 1.2mm (3 perimeters × 0.4mm nozzle). Thinner walls may not print or will be fragile. For structural parts, use 2mm minimum.
• Overhangs: Keep angles under 45° from vertical to avoid needing support material. Steeper overhangs sag, curl, or produce ugly bottom surfaces.
• Bridging: Horizontal spans up to ~10mm print fine without support. Longer spans may sag — add supports or redesign with chamfers.
• Minimum feature size: ~0.8mm (twice the 0.4mm nozzle diameter). Smaller details won't resolve clearly.
• First layer elephant's foot: The first layer is slightly squished wider than designed. Add a 0.5mm chamfer to bottom edges if fit matters.

Useful Fusion Tools for Printing

Exporting for Print

For 3MF (recommended for Bambu Lab printers), the process is the same. 3MF preserves more data than STL and is the modern standard. Set mesh refinement to High for smooth curved surfaces.

Step 1: Measure with Calipers

This is the first step for any custom design: measure the real thing before touching Fusion. Grab your calipers and measure the base diameter of your purifier — the flat bottom that'll sit in the groove.

If you don't have calipers (you should — they're ~$15 and you'll use them constantly), wrap a string around the base, measure the string length, and divide by 3.14159 to get the diameter.

Also check the purifier's weight (label on the bottom, or Google the model number). Heavier purifiers need thicker legs.

Write down: base diameter = 180mm, weight ≈ 2kg.

Step 2: Plan the Dimensions

Before sketching, work out the numbers on paper (or in your head):

• Top plate diameter: purifier base + 20mm margin = 200mm
• Top plate thickness: 5mm (sturdy enough for the weight)
• Groove diameter: caliper measurement + 0.5mm tolerance = 180.5mm
• Groove depth: 3mm (just a shallow lip to keep it centered — not a deep pocket)
• Leg height: 70mm (enough clearance for cables and a power brick underneath)
• Leg size: 20mm × 20mm rounded rectangles, positioned near the plate edge
• Number of legs: 4, evenly spaced at 90° intervals

              ◄─────── 200mm ────────►
         ┌────────────────────────────────┐
         │          Top Plate             │
         │    ┌──────────────────────┐    │
         │    │                      │    │
         │    │   Groove: ⌀180.5mm   │    │  ← 0.5mm tolerance
         │    │    depth: 3mm        │    │
         │    └──────────────────────┘    │
         │                                │
         │  ■ 20×20mm legs (×4 at 90°)   │  ← 15mm from edge
         └────────────────────────────────┘

         ◄──── 200mm ────►
         ┌────────────────┐ ─┬─ 5mm plate
    ─ ─ ─│▓▓▓▓  3mm  ▓▓▓▓│─ ┘  (groove cut 3mm deep)
         │                │
         │                │
    ─ ─ ─│  ┌──┐    ┌──┐ │
         │  │  │    │  │  │  ← 20×20mm legs
         │  │  │    │  │  │     70mm tall
         │  │  │    │  │  │
         │  └──┘    └──┘  │
         └────────────────┘  ← Fillets: 5mm at joints,
                                2mm at feet, 1.5mm on top

         ┌────────────────┐  ← Plate on build plate (smooth top surface)
         │  ████████████  │     Groove faces UP = easy bridge
         │                │
         │  ┌──┐    ┌──┐  │
         │  │  │    │  │  │  ← Legs grow upward
         │  │  │    │  │  │     Zero overhangs
         │  │  │    │  │  │
         │  └──┘    └──┘  │
         └────────────────┘
    ═══════════════════════════  Build plate

Steps 3–10: Building It

Export

Test Fit Strategy

Before printing the full stand (which might take 2–4 hours depending on size), print a quick test piece:

🖨️ Printing This Design

You've exported an STL — now comes the part most Fusion guides skip entirely. The air purifier stand looks simple, but it has real printing challenges depending on which way you orient it. Let's think through it.

Orientation Analysis

Option A — Right-side-up (legs on bed, plate on top): The legs print fine as vertical pillars growing from the bed. But the top plate is a flat ceiling spanning the empty space between the legs — a massive unsupported overhang. The printer would be trying to print a 200mm flat surface in mid-air, with nothing underneath except the four small leg tops. Without supports, the filament sags and droops. With supports, you'd fill the entire interior with support material — wasteful and messy to remove.

Option B — Upside-down (plate on bed, legs pointing up) ← BEST: The top plate sits flat on the build plate = perfectly smooth surface (this is the side everyone sees). The legs grow upward as vertical extrusions from the plate = zero overhangs. The groove on what's now the bottom? It's only 3mm deep. PLA can easily bridge across the groove diameter without any support — it's a gradual circular channel, not a sudden flat ceiling. The printer handles shallow grooves like this effortlessly.

The winner: Upside-down, every time. You get the smoothest surface on the visible top, zero supports for the legs, and the groove bridges itself.

Support Strategy

If your groove is narrow (under ~25mm diameter): No supports at all. The printer bridges across the shallow groove in a single pass. You'll see a slightly rough surface inside the groove — that's fine, the purifier base covers it.

If your groove is wider (25–50mm): The bridge might sag slightly in the center. Two options:

• Tree supports inside the groove only: In Bambu Studio: Print Settings → Support → enable supports, set Type to Tree, and set Threshold Angle to 30°. Tree supports are easy to peel out of the shallow groove. Set Support Interface to 2–3 layers for a smoother surface where the support meets the part.
• Paint-on supports: Right-click model → Support Painting. Paint green ONLY on the groove ceiling. This puts supports exactly where needed and nowhere else. Much cleaner than global supports.

If your groove is very wide (50mm+): Consider splitting the design. In Fusion: Design > Solid > Modify > Split Body → select a construction plane at the plate-leg junction. Print the plate flat (groove bridges easily when it's a thin disc), print the legs separately, then glue with CA (super glue) or epoxy. Add alignment pins in Fusion for precise assembly: small cylinders on one half, matching holes on the other.

Recommended Print Settings

• Material: PLA for purifiers under ~2kg. PETG for heavier units (better layer adhesion = legs won't delaminate under sustained load).
• Layer height: 0.2mm — standard quality, good balance of speed and detail.
• Walls: 3 perimeters. The legs get their strength from walls, not infill — 3 walls on a 20mm square leg gives 2.4mm of solid wall on each side, which is more than enough.
• Infill: 20% gyroid. Gyroid distributes strength evenly in all directions — ideal for a stand that takes vertical load from the purifier. Don't go higher; the plate and legs are solid enough at 3 walls.
• Supports: None when printing upside-down (unless the groove is wide — see above).
• Speed: 50mm/s default is fine. No speed-critical features.

Dimensions & Planning

Standard keycards/credit cards follow the ISO/IEC 7810 ID-1 size: 85.6mm × 54mm × 0.76mm. We'll design the holder with tolerances:

• Inner pocket: 88mm × 57mm (card + 1.2mm tolerance per side for easy insertion)
• Pocket depth: 4mm (holds the card securely without being too tight)
• Wall height: 2mm above the pocket (keeps card from sliding out sideways)
• Wall thickness: 2mm all around
• Thumb slot: U-shaped cutout on one short side so you can push the card out with your thumb
• Lanyard hole: 4mm diameter in one corner

Step-by-Step Build

🖨️ Printing This Design

The keycard holder is one of the most print-friendly designs in this guide — almost no printing challenges. But the details still matter if you want a smooth pocket interior.

Orientation Analysis

Best orientation: Open-side up (the card slot opening faces the ceiling). This puts the pocket base flat on the build plate. The walls grow vertically = zero overhangs. The thumb slot on one side creates a small overhang where the U-shape bridges across — but at only ~20mm wide, PLA bridges this gap cleanly without any sag.

Why not upside-down? You'd need supports inside the pocket to print the floor, and those supports would leave marks on the pocket interior. Since the card slides in and out of that pocket, you want the interior as smooth as possible. Printing open-side-up gives you clean vertical walls with no support artifacts.

Why not on its side? The pocket walls would become overhangs, and the small size makes bed adhesion tricky. Not worth it.

Support Strategy

No supports needed. The design is inherently print-friendly:

• Pocket walls grow vertically — no overhangs.
• Thumb slot bridge is under 20mm — PLA handles this easily.
• Lanyard hole is a through-hole cut with Extrude All — the slicer bridges the circular hole automatically (4mm diameter = trivial bridge).

If you see the slicer adding supports inside the thumb slot cutout, you can safely disable them. Or use Paint-on supports (right-click model → Support Painting) and paint red (block supports) over the thumb slot area.

Recommended Print Settings

• Material: PLA for desk/home use. PETG if it's going in a backpack, on a lanyard, or anywhere it'll take daily abuse — PETG is more impact-resistant and won't crack from repeated flexing.
• Layer height: 0.16mm — finer than the usual 0.2mm. The card slides in and out of the pocket, and layer lines create tiny ridges. At 0.16mm, those ridges are smaller = smoother pocket interior = the card doesn't catch. If you don't care about smoothness, 0.2mm works fine.
• Walls: 3 perimeters. The walls ARE the pocket — they need to be solid and smooth.
• Infill: 15%. The part is small enough that infill barely matters — the floor and walls are mostly solid perimeters anyway.
• Supports: None.
• Speed: 40mm/s for the inner walls (slower = smoother interior surface). Outer walls and infill can run at default 50mm/s.
• Print time: ~30–45 minutes.

Sizing Your Clip

First, measure the cable you want to organize:

• USB-C cable: ~3.5mm diameter → clip inner diameter = 4.5mm (+ 1mm tolerance)
• Lightning cable: ~3.2mm → clip inner diameter = 4.2mm
• Ethernet cable: ~6mm → clip inner diameter = 7mm
• Power cord: ~7–8mm → clip inner diameter = 9mm

We'll use 7mm inner diameter as our example (fits most common cables with some flexibility).

Step-by-Step Build

🖨️ Printing This Design

Cable clips are tiny, simple, and fast to print — but material choice matters more than you'd expect because the clip has to flex without snapping every time you insert a cable.

Orientation Analysis

Best orientation: C-opening facing up, flat mounting tab on the bed. The tab gives a large, stable first-layer footprint. The C-shaped clip body grows upward from the tab. The C-curve is a gradual arc — there's no sharp overhang at any point. The printer traces the curve layer by layer, each one offset slightly inward, and it handles this perfectly without supports.

Why not C-opening facing down? The tab would be on top, and the C-opening against the bed. This creates a worse first layer (the thin C walls don't give great adhesion) and the tab would need supports. No benefit.

Why not on its side? You'd lose the snap-fit flexibility. FDM layers are weakest at the layer boundaries — if layers run horizontally across the C-opening, the clip cracks along a layer line when you flex it. With the C-opening up, layers stack vertically along the curve, maximizing flex life.

Support Strategy

No supports needed. The C-shape has no true overhang — every layer is a gradual shift from the previous one. Even the inner surface of the C-curve prints cleanly because it's a continuous arc, not a sudden flat ceiling. If you're printing 5 clips via Rectangular Pattern, make sure the slicer isn't adding supports between the clips (it shouldn't, but check the preview).

Recommended Print Settings

• Material: PETG is ideal. Clips need to flex slightly every time a cable snaps in — PLA can do this a few times, but eventually the repeated flex causes a stress fracture at the C-opening. PETG flexes and returns without fatiguing. If you only need the clips to work for a few months, PLA is fine. For long-term use, go PETG.
• Layer height: 0.2mm — standard. These are functional parts, not display pieces.
• Walls: 3 perimeters. The clip is small enough that 3 walls makes the C-section nearly solid, which is what you want — the flex comes from the geometry (the gap in the C), not from thin walls.
• Infill: 100% — the clips are tiny (maybe 3–5g each). At this size, the difference between 30% and 100% infill is fractions of a gram and a few seconds of print time. Solid = maximum snap strength.
• Supports: None.
• Print time: ~20 minutes for 5 clips.

Why This Design Is Different

The air purifier stand (Chapter 10) was a flat platform — weight pushes straight down, simple. This one fights lateral forces. Every time you grab the hose and pull, that force at the top of a tall object creates a tipping moment. The engineering here is about stability, not just holding weight.

• Bottom exhaust — the vacuum can't sit flat on a surface. It needs to be raised with air gaps underneath.
• Top-heavy — tall cylinder, motor at the top. Wants to tip over.
• Lateral pull — the hose gets yanked sideways. The stand must resist that torque.
• Tape adhesion — legs need big, flat contact patches for double-sided tape.

Step 1: Measure Everything

Grab your calipers. This project needs more measurements than the previous ones because the design has to match the vacuum precisely and resist specific forces.

Step 2: Plan the Dimensions

Work these out on paper before opening Fusion. Every dimension ties to a physics reason — this isn't guesswork.

• Ring inner diameter: vacuum diameter + 0.5mm tolerance = 72.5mm (snug but removable)
• Ring wall thickness: 3mm per side → outer diameter = 78.5mm
• Ring height: 30–50% of vacuum height for good grip. For a 220mm vacuum: 40mm ring (about 18% feels low, but 40mm gives solid lateral support without making insertion difficult)
• Leg spread: tip-to-tip distance should be at least as wide as the vacuum is tall. Vacuum is 220mm tall → legs should reach at least 110mm from center (220mm tip-to-tip diameter). Example: each leg extends 70mm outward from the ring's outer edge.
• Leg height: 18mm — this is the airflow gap. Enough for the bottom exhaust to breathe, not so tall that it raises the center of gravity more.
• Leg shape: Trapezoid — 20mm wide at the ring, 30mm wide at the tip. Wider tip = more tape area + more stability.
• Number of legs: 4 (quadpod). Three works too, but four gives better stability in all directions when the hose pull direction is unpredictable.

Step 3: Create the Collar Ring

Step 4: Create One Leg

Step 5: Circular Pattern the Legs

Step 6: Add Gussets for Strength

This is the step most beginners skip, and it's the one that prevents your legs from snapping off. Where each leg meets the ring, there's a sharp 90° joint — that's a stress concentration point. Every time you bump the stand or pull the hose, force concentrates right at that corner. Gussets are triangular ribs that distribute that stress over a larger area.

Step 7: Add Airflow Gaps

The vacuum's air exhaust is at the bottom. If the ring sits flush against the legs with no openings, air can't escape and the motor overheats. You need gaps between the ring and the desk surface.

Step 8: Tape Recesses on Leg Bottoms

Step 9: Add an Anti-Tip Lip (Optional)

When you yank the hose sideways, the vacuum doesn't just tip — it can also lift slightly and pop out of the ring upward. A small inward lip at the top of the ring prevents this. Think of it like the rim of a cup.

Step 10: Fillet Everything

Step 11: Section Analysis — Verify Before Printing

Step 12: Export and Print

🖨️ Printing This Design

The vacuum cradle is more complex than the air purifier stand — it has a tall ring, splayed legs, gussets, and optional lip. The orientation choice is less obvious than you'd think.

Orientation Analysis

Option A — Right-side-up (legs on bed, ring pointing up) ← BEST: The leg tips sit flat on the bed = excellent first-layer adhesion (those wide trapezoid tips are perfect). The ring grows upward as a vertical cylinder — zero overhangs on the ring walls. The gussets (triangular ribs between legs and ring) grow upward from the bed as angled surfaces, but they're triangles growing from a wide base to a narrow top — the overhang is gradual and well within the 45° rule. Everything prints clean.

Option B — Upside-down (ring on bed, legs pointing up): The ring's flat bottom gives good bed contact — but the gussets are now upside-down triangles. They'd need to print with wide tops and narrow bases, creating unsupported overhangs at every gusset-to-ring junction. You'd need supports under every gusset, and removing them between the legs without damaging the gussets is messy. Worse option.

The winner: Right-side-up. Legs on bed, ring growing upward.

Support Strategy

Without the anti-tip lip: No supports needed at all. The ring is a vertical cylinder, legs are vertical extrusions, and gussets are gradual triangles — all self-supporting.

With the anti-tip lip: The lip creates an inward overhang at the top of the ring (1.5mm projecting inward). This is a small overhang but it runs around the entire inner circumference. Two approaches:

• Tree supports inside the ring: In Bambu Studio: Print Settings → Support → enable, Type: Tree, Threshold Angle: 40°. Trees grow up inside the ring and support just the lip overhang. Peel them out after printing — they come out easily from the open top. Set Support Interface Layers to 2 for a smoother finish on the lip's underside.
• Paint-on supports: Right-click model → Support Painting. Paint green ONLY on the lip's inner ceiling surface. This is more precise than global supports and avoids any support material touching the ring's inner wall (which needs to be smooth for the vacuum to slide in).

Splitting Strategy

If your stand is very tall (legs over 100mm), consider printing the ring and legs separately. In Fusion: Design > Solid > Modify > Split Body → place a construction plane at the ring-to-leg junction. Print the ring vertically, print the legs with wide tips on the bed, then join with CA glue or epoxy. This avoids the stability issues of tall prints and lets you orient each piece optimally.

Recommended Print Settings

• Material: PETG strongly recommended. This stand takes repeated lateral force every time you pull the vacuum hose. PLA is stiffer but brittle — it'll crack at the gusset-to-ring joints after weeks of daily use. PETG has better layer adhesion, slight flex before failure, and bonds better to VHB tape.
• Layer height: 0.2mm — standard quality.
• Walls: 4 perimeters — wall strength matters more than infill for resisting bending forces. The gussets and ring walls need solid perimeters to distribute stress.
• Infill: 25% cubic. Cubic provides uniform strength in all directions including lateral — better than grid for resisting bending. Higher than the air purifier stand because this part takes dynamic loads (repeated pulling), not just static weight.
• Supports: Only if you added the anti-tip lip. Otherwise support-free.
• Speed: 40mm/s for outer walls (clean surface inside the ring = vacuum slides smoothly), 50mm/s for everything else.
• Estimated print time: 2–3 hours depending on leg spread.

Engineering Breakdown

This section is the "why" behind every dimension. Skip it if you just want to build — come back to it when you design your next functional part.

Center of Gravity & Tipping

The vacuum is tall (220mm) and its motor/battery is near the top — the center of gravity is high. For the assembly (vacuum + stand) to resist tipping, the combined center of gravity must stay inside the polygon formed by the leg tips, even when a lateral force is applied at the top. Wider legs = larger stability polygon = harder to tip.

Moment Arms

Pulling the hose at the top creates a torque (rotational force) around the tipping edge. Torque = Force × Distance. The "distance" is the vacuum's height. Your stand fights back with: (vacuum weight × distance from center to leg tip) + (tape holding force). The tape is your primary anti-tip mechanism — the weight alone isn't enough for a light desk vacuum.

Tape Contact Area

VHB tape's holding strength scales with contact area. Each leg tip at 30mm × 20mm = 600mm². Four legs = 2,400mm² total. 3M VHB 5952 holds roughly 1.1 MPa in shear — at 2,400mm², that's theoretically over 2,600N (265kg) of force before the tape fails. Real-world performance is lower (surface prep, temperature, peel vs shear), but you have massive safety margin.

Why PETG Over PLA

PLA has higher stiffness (tensile modulus ~3.5 GPa vs PETG ~2.0 GPa), which sounds better. But stiffness isn't strength. PLA is brittle — it snaps without warning when it fails. PETG yields — it bends and deforms before breaking, giving you warning. For a part that takes repeated lateral loading every day (pulling the hose), PETG's ductility is worth the lower stiffness. It also has better layer adhesion, meaning the legs are less likely to delaminate at layer boundaries under bending stress.

New Skills in This Project

• Print-in-place design — designing a part that prints flat on the bed but functions as a complete assembly. No separate clips, no glue, no post-print assembly.
• Snap-fit cantilevers — a flexible tab that deflects when the Dot pushes past, then springs back to lock it in. This is the core of print-in-place: the "mechanism" is built into the geometry.
• Clearance for round objects — designing a cradle that's a specific arc angle (not a full circle), with precisely calculated clearance so the Dot fits snugly without jamming.
• VHB tape mounting — recessed pockets on the back face that keep tape edges from peeling and give a flush surface against the wall.

Echo Dot Dimensions (4th/5th Gen)

The "round puck" Echo Dot. Verify yours with calipers — Amazon's tolerances vary slightly between batches.

Step 1: Create the Wall Plate

The plate is the mounting surface. Flat back for tape, flat front for the cradle to extend from. Simple box — just like Chapter 7, but with real dimensions.

Step 2: Sketch the Cradle Profile

The cradle is a C-shaped half-pipe that wraps around the Echo Dot. We'll sketch it as two concentric circles, then trim away the top to leave an opening for sliding the Dot in.

Step 3: Extrude the Cradle

Step 4: Add the Retaining Lip

Without a lip, the Dot would just slide out the top of the cradle. We need a small overhang at the opening that catches the Dot once it's pushed in. This lip is the key to the snap-fit — it deflects outward as the Dot passes, then springs back.

Step 5: Add Snap-Fit Flexibility

Right now the lip is rigid — you'd have to force the Dot past it, and it might crack. We need the lip to flex outward when the Dot pushes against it, then snap back. The trick: cut a thin slot behind the lip to create a flexible cantilever beam.

Step 6: Add Tape Recesses on the Back

VHB tape sticks better when the edges are recessed slightly into the surface. This prevents peeling at the corners — the most common failure mode for tape-mounted prints.

Step 7: Add Cable Routing

The Echo Dot needs power. With the Dot sitting sideways in the cradle, the power cable should exit from the bottom. Cut a slot through the cradle wall at the bottom for the cable to pass through.

Step 8: Fillet Everything

Fillets serve two purposes here: structural (reducing stress concentrations at joints) and aesthetic (making the mount look intentional, not hacked together).

Step 9: Export & Print Settings

🖨️ Printing This Design

The Echo Dot mount has the most challenging print geometry so far — a concave cradle (overhangs inside a curve), snap-fit lips (precision features), and a flat plate (warping risk). Here's how to handle it.

Orientation Analysis

Best orientation: Plate flat on bed, cradle pointing upward. The plate gives a large, stable first layer (120 × 80mm = excellent adhesion). The cradle walls grow upward from the plate as a half-pipe shape. The outer walls of the cradle are vertical — no issues. The problem is the inner curve of the cradle: it's concave, meaning as the walls curve inward toward the top, the inner surface becomes an overhang. Think of it like printing the inside of a bowl — the bottom half is fine, but as the curve goes past 45° from vertical, you need supports.

Why not upside-down (cradle on bed)? The cradle's curved outer surface would be on the build plate — poor adhesion, weird geometry contact, and the plate would be floating in the air needing full support. Terrible option.

Why not sideways? Layer lines would run across the snap-fit lips instead of along them. The lips need layers along their length for flex — sideways printing makes them brittle across the layer boundaries.

Support Strategy

This design needs supports — there's no avoiding it. The inner curve of the cradle creates overhangs past 45° as it wraps around to form the half-pipe. Here's how to do it cleanly:

• Support type: Tree supports (Bambu Studio: Print Settings → Support → Type: Tree). Tree supports navigate around the cradle geometry better than grid supports, and they're dramatically easier to remove from the curved interior. Normal grid supports inside a curved cradle are a nightmare to clean.
• Threshold angle: 40° — this catches the inner curve overhangs while leaving the outer walls alone.
• Support interface: 3 layers — the inner cradle surface needs to be reasonably smooth (the Echo Dot sits against it). More interface layers = smoother surface where supports contact the part.
• Paint-on alternative: For maximum control, right-click model → Support Painting. Paint green only on the inner curve's ceiling areas (the parts that are clearly overhanging). Paint red on the snap-fit lips and relief slots — you do NOT want supports inside those delicate features.

Splitting Strategy (Alternative)

If you want to avoid supports entirely: split the cradle from the plate. In Fusion: Design > Solid > Modify > Split Body at the plate-to-cradle junction. Print the plate flat (trivial — no overhangs). Print the cradle halves laid flat on their sides (the half-pipe becomes a simple curved wall with no overhangs). Glue the cradle to the plate with CA glue. This eliminates supports completely, but requires assembly and precise alignment.

Recommended Print Settings

• Material: PETG — mandatory. The snap-fit cantilevers flex every time you insert/remove the Echo Dot. PLA is too brittle — the lip will crack after 3–5 insertions. PETG flexes and returns without permanent deformation. Print at 240°C nozzle / 80°C bed for maximum layer adhesion.
• Layer height: 0.2mm — good balance of speed and detail for the cradle curves.
• Walls: 4 perimeters — the cradle and lips are structural, and wall count directly affects snap-fit strength.
• Infill: 25% — the plate needs rigidity to hold the cradle against the wall without flexing under the Dot's 328g weight.
• Supports: Tree supports, 40° threshold, 3-layer interface. Or paint-on supports targeting only the inner cradle curve.
• Speed: 35mm/s for the snap-fit lip area (precision matters), 50mm/s elsewhere.

Design Breakdown

Why Print-in-Place Works Here

Traditional approach: print the mount, print a clip, assemble with a screw. Print-in-place eliminates the assembly step by building the mechanism directly into the geometry. The snap-fit cantilever (lip + relief slot) is a compliant mechanism — it gets its motion from material flex, not from separate moving parts. This only works because:

• PETG flexes before breaking — PLA would snap. The lip needs to deflect 2-3mm without permanent deformation.
• The relief slot creates a controlled weak point — without it, the entire cradle wall would need to flex (impossible).
• The geometry prints without trapped supports — the slot is open, not enclosed. Supports can be removed easily.

Clearance Math

Echo Dot diameter: 100mm. Cradle inner diameter: 102mm. That's 1mm clearance per side. Why 1mm?

• Too tight (0.3mm or less): Manufacturing variance + printer tolerance = the Dot won't fit. You'll sand, swear, and reprint.
• Too loose (2mm+): The Dot rattles in the cradle. The lip can't catch it because there's too much play.
• 1mm is the sweet spot: Accounts for printer accuracy (~0.2mm), Echo Dot tolerance (~0.5mm), and still snug enough for the lip to engage.

VHB Tape vs. Screws

3M VHB 5952 holds ~1.1 MPa in shear. Two 60mm × 15mm strips = 1,800mm² of contact. That's theoretically ~1,980N (200kg) of shear strength. The Echo Dot weighs 328g. You have a 600:1 safety margin. VHB easily outperforms two drywall screws for this application, and you don't drill holes in your wall.

New Skills in This Project

• Ultra-thin wall design — designing parts at or near nozzle width (0.4mm). You'll learn why wall thickness must be a multiple of your nozzle diameter.
• Sheet-like 3D printing — parts that are essentially 2D sheets with a tiny Z dimension. Different rules apply: no infill, all perimeter walls, slow speeds.
• Precise measurement of existing objects — using calipers to measure the chute interior and designing a part that fits inside with clearance.
• Material selection reasoning — why PETG is the right material: slippery surface (low friction coefficient), heat-resistant (purge blobs are 200°C+), and slightly flexible so it can bend into the chute.

Waste Chute Dimensions (P1S)

Grab your calipers. Open the P1S front panel, locate the waste chute on the right side, and measure the interior.

Understanding Nozzle-Width Constraints

Before we sketch, let's talk about why this part is special. Your nozzle is 0.4mm wide. That means the thinnest wall you can print is 0.4mm — one pass of the nozzle. Two passes = 0.8mm. Three = 1.2mm. You can't print a 0.6mm wall because the slicer can't fit 1.5 nozzle passes.

We'll use 0.8mm — exactly 2 perimeter walls. This gives us a solid, gap-free sheet that's still thin enough to flex slightly when inserting into the chute.

Step 1: Sketch the Liner Profile

This is as simple as sketching gets — a rectangle. But the dimensions matter precisely.

Step 2: Extrude to 0.8mm

Here's where the nozzle-width constraint comes in. We're extruding to exactly 2× the nozzle width.

Step 3: Add the Retention Lip

The lip hooks over the top rim of the chute. It's an L-shaped extension — the liner goes up, then bends forward over the rim. Without this, the liner would just slide down into the chute.

Step 4: Fillet the Bottom Edge

A small fillet on the bottom edge helps purge blobs roll off instead of catching on a sharp corner.

Step 5 (Optional): Add Air-Channel Ribs

These are barely-there raised lines on the inner surface that create tiny air gaps. When a hot purge blob lands on the liner, the ribs prevent full-surface contact — less contact = less sticking.

Step 6: Export as STL

🖨️ Printing This Design

The chute liner is geometrically trivial — it's a flat sheet. But ultra-thin parts have their own printing challenges that don't apply to thicker designs. The enemies here are warping, adhesion, and speed.

Orientation Analysis

Best orientation: Flat on the bed. Lay the 41mm × 115mm face flat on the build plate. The 0.8mm thickness builds up in just 4 layers at 0.2mm layer height. The retention lip at the top is an L-shaped extension — the vertical part (3mm tall) grows upward from the sheet, then the horizontal hook (5mm) creates a small overhang. At only 5mm wide and 0.8mm thick, the hook bridges effortlessly.

Why not on its edge? Standing the liner on its 0.8mm edge would be absurd — the contact area is too small for adhesion, and a 115mm tall, 0.8mm thick wall would wobble and fail almost immediately. Never print sheet-like parts on their edge.

Why not angled? No benefit. The part is flat. Angling it just wastes bed space and adds complexity.

Support Strategy

No supports needed. There are zero overhangs — the sheet is flat, the lip hook is a tiny bridge the printer handles automatically. The optional ribs on the inner surface are just 0.4mm bumps on a flat surface — no overhang there either.

The Real Challenge: Warping & Adhesion

Thin, wide PETG sheets love to warp. The edges cool faster than the center, creating internal stress that curls the corners up off the bed. This is the #1 failure mode for this part. Countermeasures:

• Brim: In Bambu Studio: Plate Adhesion → Brim Width: 5mm. The brim adds extra first-layer material around the part's perimeter, anchoring the edges. Peel it off after printing — it snaps away cleanly from PETG.
• Bed temperature: 80°C for PETG (standard). If warping persists, try 85°C for the first 5 layers, then drop to 75°C. In Bambu Studio: Filament Settings → Bed Temperature → First Layer / Other Layers.
• First layer speed: 20mm/s (slower = better adhesion). The first layer is everything for thin parts.
• Enclosure: If you have a P1S (you probably do — you're printing a liner for it), keep the enclosure closed. Even airflow prevents uneven cooling that causes warping.

Recommended Print Settings

• Material: PETG — non-negotiable. It's slippery (purge blobs slide off), heat-resistant (survives 200°C+ blob contact), and flexible enough to bend into the chute without cracking. PLA would work geometrically but melts/deforms when hot purge blobs hit it.
• Layer height: 0.2mm — at 0.8mm total thickness, that's exactly 4 layers. Each layer matters.
• Walls: 2 perimeters (2 × 0.4mm nozzle = 0.8mm). This IS the entire part — there's no interior space for infill.
• Infill: 0% — irrelevant. The part is all wall.
• Speed: 30mm/s max. Thin parts oscillate at higher speeds — the nozzle pushes the flimsy sheet around. Slow and steady.
• Supports: None.
• Bed adhesion: Brim, 5mm width.
• Print time: ~15 minutes.

Dimension Validation

New Skills in This Project

• The Sweep tool — creating a 3D shape by moving a 2D profile along a curved path. Think of it like squeezing toothpaste along a curved line — the tube shape follows the path.
• Spline curves — organic, flowing curves defined by control points. Unlike arcs (which are parts of circles), splines can create any smooth curve.
• Countersink holes — screw holes where the head sits flush with or below the surface. Combines a through-hole with a chamfered cone at the top.
• Load-bearing design — headphones weigh 250–400g and pull straight down. The mount pushes up against the desk. The hook arm acts as a cantilever — stress concentrates where it meets the plate.

Step 1: Create the Mounting Plate

Step 2: Add Countersink Screw Holes

Countersink holes let screw heads sit flush so the plate lies flat against the desk. We'll make them in two steps: drill the through-hole, then chamfer the top.

Step 3: Draw the Hook Path (Spline)

This is the big new concept. We'll draw the J-shaped hook path as a spline — a smooth curve that Fusion will use as the "track" for the Sweep tool.

Step 4: Draw the Hook Profile (Circle)

The Sweep tool needs two things: a PATH (the spline we just drew) and a PROFILE (the cross-section shape). Our hook has a round cross-section — a circle.

Step 5: Sweep!

This is the payoff. One click creates the entire 3D hook from the path and profile.

Step 6: Join Hook to Plate

Right now the hook and plate are separate bodies. We need to merge them.

Step 7: Export as STL

🖨️ Printing This Design

The headphone hanger is the most orientation-sensitive project in this guide. Print it the wrong way and it snaps under the weight of headphones. Print it the right way and it'll hold for years.

Orientation Analysis

Option A — Plate flat on bed, hook pointing down ← WRONG: The plate prints beautifully flat. But the hook's J-curve extends straight down from the plate. Layer lines run horizontally through the hook — perpendicular to the bending force. When headphones (250–400g) hang on the hook, they pull straight down, trying to peel the layers apart at the weakest point: the junction where the hook meets the plate. The hook will eventually snap along a layer line. Don't do this.

Option B — Sideways (plate vertical, hook extending horizontally) ← BEST: Lay the entire part on its side so the plate is vertical and the J-hook extends horizontally from it. Now layer lines run along the hook's length — parallel to the bending force. Each layer wraps around the full cross-section of the hook, creating a continuous tube of material along the entire curve. Bending force is now fought by the layer bonds across the full 10mm diameter, not by trying to separate individual layers. Vastly stronger.

Option C — Split and print flat (strongest option): In Fusion, use Design > Solid > Modify > Split Body to separate the plate from the hook at their junction. Print the plate flat on the bed (trivial). Print the hook lying on its side with the J-curve flat on the bed (the 10mm round cross-section becomes a long sausage shape on the bed). Glue together with CA glue or epoxy. Each piece prints in its optimal orientation, and the epoxy joint at the junction is actually stronger than the FDM layer bond.

Support Strategy (for sideways orientation)

Printing sideways means the underside of the J-curve becomes an overhang. The hook curves from vertical to horizontal to curving back up — the bottom of that curve needs support.

• Support type: Tree supports — the J-curve is an organic shape, and tree supports follow organic surfaces better than grid supports. They also leave a cleaner surface on the round hook (you don't want rough support marks where the headphone band rests).
• Threshold angle: 35° — catches the curve underside while leaving the straight sections alone.
• Support interface: 3 layers — the hook's outer surface should be smooth where headphones rest. More interface layers = smoother contact surface.
• Paint-on supports: Right-click model → Support Painting. Paint green only on the J-curve's underside. Paint red on the plate's face and the hook's top surface. This gives you supports exactly where needed and keeps the rest clean.

Support removal: PETG tree supports snap off cleanly with needle-nose pliers. The curved surface may have minor marks where supports attached — sand with 220-grit sandpaper for a smooth finish, or leave as-is (it's under a desk, nobody sees it).

Recommended Print Settings

• Material: PETG — mandatory for this design. Headphones hang 24/7, creating sustained bending stress. PLA creeps under sustained load (slowly deforms over weeks/months). PETG doesn't. PLA is also brittle — one bump knocks the headphones sideways and the PLA hook snaps. PETG absorbs that impact and springs back.
• Layer height: 0.2mm — standard quality.
• Walls: 4 perimeters — the hook's 10mm circular cross-section is almost entirely walls at 4 perimeters (4 × 0.4mm × 2 sides = 3.2mm of solid wall out of 10mm diameter). This is what gives the hook its strength.
• Infill: 40% — higher than most projects because this is load-bearing. The hook arm acts as a cantilever beam under constant bending stress. More infill = more internal structure resisting that bend.
• Supports: Yes — tree supports under the J-curve (sideways orientation). None needed if using the split-and-glue approach.
• Speed: 40mm/s — moderate. Not a rush job, and slower speeds give better layer adhesion on PETG.

Dimension Validation

New Skills in This Project

• Components — Fusion's way of organizing multi-part designs. The box and lid are separate components in the same file, each with their own body, sketches, and timeline. This is how real products are designed.
• Text embossing/debossing — putting actual text on your parts. Emboss (raised) or deboss (recessed) — both use the same Sketch Text + Extrude workflow.
• Snap-fit tolerances — designing bumps and catches that click together. This requires understanding interference fits: the catch must be slightly deeper than the bump is tall.
• Ventilation holes — rectangular pattern of small holes for airflow. Chargers generate heat inside a closed box — vents prevent overheating.
• Oval/ellipse sketching — cable entry holes aren't circles, they're ovals. Fusion has a dedicated Ellipse tool for this.

Step 1: Create Component Structure

Before we draw anything, let's set up the component tree. This keeps box and lid bodies organized and exportable separately.

Step 2: Design the Box

Activate the Box component (double-click it in the Browser). We'll build the open-top box using the same sketch-extrude-shell workflow from earlier chapters, but bigger.

Step 3: Add Cable Entry Holes

Cables enter through oval holes on both short sides. Ovals are better than circles for cables — they accommodate flat USB-C and round barrel connectors alike.

Step 4: Add Ventilation Grid

Chargers inside the box generate heat. A grid of small holes on the back face allows airflow. We'll use Rectangular Pattern to create the grid efficiently.

Step 5: Add Snap-Fit Bumps

Small protrusions near the top rim of each long wall. The lid's catches will grab onto these bumps — click in, click out. The critical dimension: bump height vs. catch depth.

Step 6: Design the Lid

Now activate the Lid component (double-click "Lid" in the Browser). The lid is a flat plate with matching snap catches and a text label.

Step 7: Add Text Label

The final touch — emboss or deboss a text label on the lid surface. This is your first time using Fusion's Text tool in a sketch.

Step 8: Export Both Components

Since box and lid are separate components, they export separately — and they should, because they print in different orientations.

🖨️ Printing This Design

The cable organizer is a two-part design — box and lid print separately with different orientations. The box is straightforward; the lid has some nuances around the inner lip and text embossing.

Orientation Analysis

Box — Open-side up (upright): The obvious choice, and it's correct. Place the box flat on the bed with the opening facing the ceiling. The walls grow vertically — zero overhangs, zero supports. The snap-fit bumps on the outer walls are tiny (1mm) protrusions that the printer handles as slight outward steps — well within the overhang tolerance. The ventilation holes on the back face are through-holes in a vertical wall — the slicer bridges across each 5mm hole automatically. The oval cable entry holes are slightly bigger bridges (~15mm minor axis) but still bridge fine since they're in a vertical wall and the bridge is circular (not a flat ceiling).

Lid — Flat, text side up: The lid is a flat plate with a downward-extending inner lip. Print it with the TOP surface (with text) facing up. The inner lip extends 3mm downward, but since it prints on the bed, you actually flip it: inner lip facing up, text on the bed. Wait — that would damage the text. Better approach: print with text side up. The inner lip extends downward from the bottom = it's printing downward from the plate, but since the plate is on the bed, the lip is really just a step on the bottom surface. No overhang — the lip is vertical walls extending below the plate's outer edge. The snap catches are small cutouts in the lip — through-holes, no overhangs.

Support Strategy

Box: No supports needed. Everything is vertical walls growing from a flat base. The vent holes and cable ovals are circular/oval through-holes in vertical surfaces — the slicer bridges the top arc of each hole. At 5mm diameter (vents) and 15mm minor axis (ovals), these bridge cleanly in PLA.

Lid: No supports needed. The inner lip is a vertical extension below the plate. The text embossing is either raised (extrude upward = just a bump, no overhang) or recessed (extrude downward = a pocket, no overhang). Neither requires supports.

One exception: If your embossed text uses a font with enclosed counters (the inside of letters like "O", "A", "D"), the slicer needs to bridge across those tiny enclosed areas. At 12mm text height, these counters are tiny — they bridge automatically. But if you see missing counter fills in the slicer preview, enable Detect Thin Walls in Bambu Studio (Print Settings → Quality → Detect thin walls).

Recommended Print Settings

Dimension Validation

New Skills in This Project

• User Parameters — named variables that drive dimensions throughout your design. Instead of typing "70" for the angle, you type stand_angle. Change the parameter → the entire model updates. This is the defining feature of parametric CAD.
• Construction Planes at angles — creating a tilted sketch plane at an arbitrary angle to an existing face. You'll sketch on a 70° plane as easily as sketching on a flat one.
• Revolve tool — spinning a 2D profile around an axis to create a round 3D shape. We'll use it for optional rounded feet on the base.
• Parameter-driven design thinking — deciding which dimensions should be parameters and which can be hard-coded. Not everything needs to be a variable.

Step 1: Define User Parameters

Before we sketch a single line, we'll define the variables that control the design. This is backwards from how we've worked in every previous project — and that's the point. Parameters-first is how professionals design.

Step 2: Create the Base Plate

Step 3: Create a Construction Plane at an Angle

The back support rises at 70° from horizontal. To sketch on a 70° plane, we first need to create one.

Step 4: Create the Back Support

Step 5: Add the Phone Lip

The lip is a small shelf at the front of the base that stops the phone from sliding off. It's just a rectangle extruded upward from the base's front edge.

Step 6: Fillet the Edges

Step 7 (Optional): Revolve — Add Rounded Feet

Optional but teaches the Revolve tool. We'll add small hemispherical rubber-bumper-style feet at the base corners to prevent desk scratching and add grip.

Step 8: Test the Parameters

This is the most satisfying step. Let's prove that parameters actually work.

Step 9: Export as STL

🖨️ Printing This Design

The phone stand is parametric — the printing challenges change depending on what angle you chose for stand_angle. This makes it a great real-world lesson: your design decisions in Fusion directly affect how printable the result is.

Orientation Analysis

Best orientation: Base flat on bed, angled support rising upward. The base plate sits flat = great first-layer adhesion over the full 80 × 100mm footprint. The back support panel grows at an angle from the base's back edge. The phone lip at the front is a small vertical extrusion from the base = no issues.

The key question is whether the angled back support creates a problematic overhang — and that depends entirely on your stand_angle parameter:

• stand_angle = 70° (default): 70° from horizontal = only 20° from vertical. Well within the 45° overhang limit. No supports needed. The printer traces each layer with a slight offset, and the 20° lean is imperceptible to the printer.
• stand_angle = 60°: 30° from vertical. Still safe. No supports.
• stand_angle = 50°: 40° from vertical. Getting close to the limit. PLA can handle this, but you might see slight roughness on the underside of the support panel. PETG starts needing supports here.
• stand_angle = 45°: Exactly 45° from vertical = the theoretical limit. It'll print, but the underside will be rough. Add supports if you want a clean surface underneath.
• stand_angle < 45°: More than 45° overhang. You need supports.

The parametric lesson: At 70° (default), this is a support-free, easy print. But if someone changes the parameter to 35° for a more reclined tablet angle, suddenly supports are mandatory. Your design parameter affects manufacturing. Real engineering.

Support Strategy (when stand_angle < 50°)

If you've set a low angle and need supports:

• Support type: Normal (grid) supports work best here. The back support panel's underside is a flat, regular surface — not organic or curved. Grid supports give a flatter interface on this kind of geometry than tree supports.
• Threshold angle: 45° — this catches the angled panel while leaving the base and lip alone.
• Support interface: 2 layers — the underside of the back panel isn't a critical surface (nobody sees it when the phone is in place).
• Paint-on alternative: Right-click → Support Painting. Paint green on ONLY the underside of the angled panel. This is cleaner than global supports, which might try to add material under the lip or inside corners.

No Splitting Needed

The phone stand doesn't benefit from splitting. It's a simple one-piece design at any angle, and all the geometry grows from the base plate. If you did split the back support from the base, you'd create a weak glue joint at the highest-stress point (where the phone's weight pushes against the support). Keep it as one piece — the Fusion fillet at the base-to-support junction distributes stress, and FDM's layer continuity through that junction is stronger than any glue.

Recommended Print Settings

• Material: PLA — a desk stand doesn't take abuse. It holds a phone at an angle, that's it. PLA is stiffer than PETG, which means less flex in the back support = the phone sits more stably. If you want a premium feel, try Silk PLA (metallic sheen) or Matte PLA (soft texture).
• Layer height: 0.2mm — standard. The angled back panel will show layer lines as visible stepped ridges. If this bothers you, drop to 0.12mm — the steps become almost invisible, but print time nearly doubles.
• Walls: 3 perimeters — the 4mm back support panel is almost entirely walls at 3 × 0.4mm per side = 2.4mm of solid wall. Adequate for holding a 200g phone.
• Infill: 20% — the base needs some weight for stability (prevents tipping when you tap the phone screen), and 20% provides that without wasting material.
• Supports: None at stand_angle ≥ 50°. Normal supports at lower angles.
• Speed: 50mm/s — no sensitive features.

Dimension Validation

Why Split a Model?

You've been designing single-body prints for every project so far. That works great when the shape is simple. But some geometries fight you no matter what:

• Internal overhangs and ceilings — supports inside enclosed spaces are impossible to remove
• Tall thin features — wobbly during printing, prone to layer shifts
• Multi-material designs — legs in PETG for strength, plate in PLA for aesthetics
• Larger than the build plate — the only option is splitting
• Reprint efficiency — if one leg fails, reprint just the legs instead of the whole stand

The Air Purifier Stand is the perfect example. In Chapter 10, we printed it upside-down — the groove bridged across open air (sometimes saggy), and the leg-to-plate junctions needed support material. Splitting the plate from the legs solves both problems.

Five Assembly Methods

Before we split anything, you need to know how the pieces will go back together. Here are five approaches — from dead-simple to mechanically satisfying — each with full Fusion walkthroughs using our Air Purifier Stand as the example.

Method 1: Super Glue Joint — ⭐ Easiest

Difficulty: ⭐ Beginner  |  Permanent? Yes  |  Tools needed: CA glue, 220-grit sandpaper

The simplest assembly. Split your model with a flat cut → print both halves → glue them together. No alignment features, no pins, no extra geometry in Fusion. Just two flat faces bonded with cyanoacrylate (CA / super glue).

Fusion Steps

1. Open your completed Air Purifier Stand from Chapter 10
2. Go to Design > Solid > Modify > Split Body
3. Select the stand body → select the bottom face of the plate as the splitting tool
4. Click OK — two bodies appear in the Browser panel
5. Rename them TopPlate and Legs
6. Right-click each → Save as Mesh → export as STL (Binary, High refinement)

That's it for the Fusion work. No pins, no holes, no alignment features. The flat mating surfaces are the alignment — press them together on a flat table and they self-align.

Assembly Process

1. Sand both mating faces lightly with 220-grit sandpaper — this roughens the surface for better glue adhesion. Don't sand aggressively; 10-15 seconds of light passes per face is enough
2. Dry-fit first — press the pieces together without glue to verify they sit flush
3. Apply thin CA glue to ONE face only — a thin, even layer across the surface. Don't use blobs; excess glue squeezes out and makes a mess
4. Press together firmly for 30 seconds — apply even pressure across the whole joint
5. Wipe excess glue immediately with a dry paper towel before it cures
6. Optional: spray CA accelerator on the outside of the joint for an instant bond (otherwise full cure takes 10-15 minutes)

When to use: When you don't need to disassemble, and alignment isn't critical. Perfect for cosmetic parts, prototypes, or oversized models split purely to fit the build plate. If your purifier stand is permanent furniture, glue is all you need.

Method 2: Pin & Hole Push-Fit — ⭐⭐ Recommended

Difficulty: ⭐⭐ Intermediate  |  Permanent? Optional (friction or glue)  |  Tools needed: None (optionally CA glue)

Split the body AND add cylindrical pins on one half with matching holes on the other. The pins self-align the pieces during assembly, prevent lateral sliding, and friction-fit holds them together. Add glue if you want permanent. This is the method we'll walk through in the step-by-step below.

Pin Sizing Guide

Multiple Pins Per Connection

A single pin prevents lateral movement but can't prevent rotation. For our purifier stand (round plate, round legs), one pin per leg is fine because the leg position relative to the plate is already constrained by the socket shape. But for flat mating surfaces (like a rectangular box split in half), use 2–3 pins per connection:

• 2 pins: Prevents rotation completely. Place them as far apart as possible along the joint.
• 3 pins: Adds redundancy. If one pin is slightly off-tolerance, the other two still hold alignment. Use a triangle arrangement, not a line.
• Asymmetric placement: Put pins in a non-symmetric pattern so the parts can only assemble one way — prevents accidental 180° rotation.

Stepped Pins (Advanced Variant)

A stepped pin has two diameters: a 4mm shaft that fits into the hole, topped by a 6mm shoulder/flange that acts as a depth stop. The shoulder rests on the mating surface when fully inserted, preventing the pin from going too deep.

Fusion steps for a stepped pin:

1. Create a sketch on the leg top face → draw a 4mm diameter circle centered on the leg
2. Extrude 4mm upward, Operation: Join — this is the shaft
3. Create a new sketch on the top face of the pin you just made
4. Draw a 6mm diameter circle, concentric with the shaft
5. Extrude 1.5mm downward (into the shaft), Operation: Join — this creates the flange/shoulder
6. The matching hole stays at 4.3mm diameter — the 6mm shoulder sits on the surface and stops insertion at the right depth

When to use: Functional parts, things you might want to disassemble, anything where precise alignment matters. The purifier stand's default method. Pins + glue gives you the strongest permanent joint with perfect alignment.

Method 3: Snap-Fit / Mechanical Retention — ⭐⭐⭐ Advanced

Difficulty: ⭐⭐⭐ Advanced  |  Permanent? No — tool-free assembly and disassembly  |  Tools needed: None  |  Material: PETG or TPU required (PLA will crack)

This is the satisfying one. Design legs that snap into the plate and are held by a mechanical catch. Push in → hear a click → done. No glue, no tools, no hardware. To remove: squeeze the leg slightly and pull down.

The Concept

• Each leg has a small bump/hook near the top — a rectangular protrusion on the outer face
• The plate has matching sockets with a slight undercut — the bump snaps past the socket entry and rests in a recessed pocket
• A relief slot behind the bump allows the leg wall to flex inward during insertion
• Chamfers on both the bump and socket entry create a ramp that guides the parts together
• Push the leg up into the socket → the bump deflects inward (using the flex from the relief slot) → clears the undercut → springs back outward into the pocket → click

Fusion Step-by-Step: Snap-Fit Purifier Stand

Part A — The Snap Bump (on the leg, top end):

1. In the Browser panel, select the Legs body. Hide the TopPlate.
2. Go to Design > Sketch > Create Sketch — select the outer face of one leg, near the top
3. Use the Rectangle → Center Rectangle tool (R)
4. Draw a rectangle: 3mm wide × 1.5mm tall, positioned 2mm from the top edge of the leg
5. Use Sketch > Constrain > Dimension (D) to lock all measurements
6. Click Finish Sketch
7. Press E for Extrude → select the rectangle profile → type 1 mm outward (away from the leg center)
8. Operation: Join → click OK
9. Now add the lead-in ramp: go to Design > Solid > Modify > Chamfer
10. Select the TOP edge of the bump (the edge closest to the leg top) → distance: 0.8mm at 45°
11. Click OK — this creates the lead-in ramp that lets the bump slide past the socket entry
12. Leave the BOTTOM edge sharp — this is the catch that holds. The sharp edge hooks behind the undercut pocket.

Part B — The Relief Slot (critical for flex):

1. Go to Design > Sketch > Create Sketch — select the same outer face of the leg
2. Draw a rectangle directly behind the bump (between the bump and the leg center): 1mm wide × extending from the bump to 5mm below it
3. Finish Sketch
4. Press E for Extrude → select the slot profile → extrude through the leg wall as a cut
5. Operation: Cut → click OK

This slot creates a thin section of wall behind the bump that can flex inward when the leg is pushed into the socket. Without it, the leg is too rigid — the bump can't deflect and won't clear the socket entry. Think of it like the relief slot in the Echo Dot mount from Chapter 14.

Part C — The Socket Pocket (on the plate):

1. Show the TopPlate body. Hide the Legs body for easier selection.
2. Go to Design > Sketch > Create Sketch — select the inner wall of the leg socket (the cylindrical hole inside the plate where the leg inserts)
3. Draw a rectangle matching the bump location: 3.2mm wide × 1.7mm tall (that's 0.2mm clearance on each dimension for manufacturing tolerance)
4. Position it to align with where the bump will sit when the leg is fully inserted
5. Finish Sketch
6. Press E for Extrude → select the pocket profile → extrude 1.2mm into the plate wall (away from the socket center)
7. Operation: Cut → click OK

This pocket is slightly deeper than the bump (1.2mm vs 1mm). The extra 0.2mm means the bump fully seats inside the pocket, giving you that satisfying "click" when it snaps into place.

Part D — Draft Angle on Socket Entry:

1. Go to Design > Solid > Modify > Chamfer
2. Select the TOP edge of the socket opening (the entry where the leg slides in)
3. Distance: 0.8mm at 45° — this matches the bump's lead-in chamfer
4. Click OK

Together, the two chamfers (bump top + socket entry) create a smooth ramp. When you push the leg upward, the bump's chamfer rides against the socket's chamfer, gradually deflecting the wall inward through the relief slot. Once the bump clears the entry edge, it springs outward into the pocket.

Part E — Replicate to All Four Legs:

1. Select all the features you just created (bump extrude, chamfer, relief slot cut) in the Timeline
2. Go to Design > Solid > Create > Pattern > Circular Pattern
3. Pattern Type: Features → select the snap-fit features
4. Axis: Z axis (vertical center)
5. Quantity: 4
6. Click OK — repeat the same pattern for the socket pockets and entry chamfers on the plate

Design Parameters Reference

When to use: When you want tool-free, reversible assembly with no hardware. Battery covers, enclosures, modular furniture, anything opened occasionally. For the purifier stand: if you want to swap legs (different heights, colors, or materials) without glue or tools, snap-fit is the move.

Method 4: Threaded / Heat-Set Inserts — ⭐⭐⭐ Advanced

Difficulty: ⭐⭐⭐ Advanced  |  Permanent? No — bolted, fully removable  |  Tools needed: Soldering iron, hex key/screwdriver  |  Hardware: M3 or M4 brass inserts + matching bolts

The strongest removable connection. Brass heat-set inserts melt into the plastic with a soldering iron tip, creating permanent threaded sockets. Then you bolt the pieces together with machine screws. Industrial-grade, designed for hundreds of assembly/disassembly cycles under load.

Fusion Steps for the Purifier Stand

Part A — Insert Holes in the Plate:

1. Select the TopPlate body
2. Go to Design > Sketch > Create Sketch on the bottom face of the plate (where each leg meets the plate)
3. Press C → draw a circle centered on each leg position: 4.5mm diameter for M3 inserts (check your specific insert's datasheet — common brands like CNC Kitchen or Ruthex specify the hole size)
4. Finish Sketch
5. Press E for Extrude → -6mm (into the plate, from the bottom face). This should be ≥ the insert length (most M3 inserts are 4–5mm long). Leave at least 1mm of material above the insert.
6. Operation: Cut → click OK
7. Use Circular Pattern to replicate to all 4 leg positions

Part B — Bolt Through-Holes in the Legs:

1. Select the Legs body
2. Go to Design > Sketch > Create Sketch on the bottom face of one leg (the foot that sits on the ground)
3. Press C → draw a circle: 3.2mm diameter for M3 bolts (3mm bolt + 0.2mm clearance)
4. Center it on the leg
5. Finish Sketch → Press E → Extrude through the entire leg (use "To Object" and select the top face, or extrude a large value with "Cut" through all)
6. Operation: Cut → click OK

Part C — Countersink for Flush Bolt Heads:

1. Go to Design > Solid > Modify > Chamfer
2. Select the bottom entry edge of each bolt hole (on the foot of the leg)
3. Distance: 3mm — this creates a conical recess where the bolt head sits flush with (or slightly below) the leg bottom
4. Click OK
5. Replicate with Circular Pattern to all 4 legs

Insert Installation

1. Set your soldering iron to 200–220°C (for PLA) or 240–260°C (for PETG)
2. Place a brass insert on the hole opening, threaded end up
3. Press the soldering iron tip into the insert's threaded hole — apply gentle, steady downward pressure
4. The insert melts into the surrounding plastic in ~5 seconds. Stop when the insert flange is flush with the surface.
5. Wait 30 seconds for cooling before touching
6. Thread an M3 bolt through the leg's through-hole and into the insert → tighten with a hex key

When to use: Heavy loads, vibration environments, parts you'll disassemble many times. The purifier stand sitting on a table next to a running 3D printer (constant vibration) is a perfect candidate. Also great when you want to swap parts — print legs in different colors or lengths and bolt on whichever set you want.

Method 5: Dovetail / Slide-In Joint — ⭐⭐ Intermediate

Difficulty: ⭐⭐ Intermediate  |  Permanent? Semi-permanent (locked by geometry)  |  Tools needed: None  |  Cool factor: High

Parts slide together from one direction and lock mechanically in all other directions. One piece has a trapezoidal rail (wider at the base, narrower at the top — like a traditional woodworking dovetail). The other piece has a matching channel. Slide together from the side → locked everywhere except the slide axis. Add a pin, clip, or friction bump at the end to prevent sliding back out.

Fusion Steps for the Purifier Stand

Part A — Dovetail Rail on the Leg Top:

1. Select the Legs body. Go to Design > Sketch > Create Sketch on the end face (the side of the leg top, perpendicular to the slide direction)
2. Use the Line tool (L) to draw a trapezoid profile:
   • Bottom edge (wider): 6mm
   • Top edge (narrower): 4mm
   • Height: 3mm
   • The angled sides create the dovetail — roughly 75° from horizontal (15° draft)
3. Position the trapezoid centered on the leg top face
4. Use Sketch > Constrain > Dimension (D) to lock all measurements
5. Finish Sketch
6. Press E for Extrude → select the trapezoid → extrude along the slide direction for the full width of the connection (e.g., 15mm)
7. Operation: Join → click OK

Part B — Matching Channel in the Plate:

1. Select the TopPlate body
2. Go to Design > Sketch > Create Sketch on the corresponding face of the plate (same orientation as the rail sketch)
3. Draw the same trapezoid shape, but larger by the clearance tolerance:
   • Bottom edge: 6.5mm (+0.25mm per side)
   • Top edge: 4.5mm (+0.25mm per side)
   • Height: 3.3mm (+0.3mm)
4. Finish Sketch
5. Press E for Extrude → extrude as a Cut through the plate, along the slide direction
6. Operation: Cut → click OK

Part C — End Stop (prevents sliding back out):

1. At the closed end of the dovetail channel, the rail simply bottoms out against a wall — the extrude-cut doesn't go all the way through
2. Alternatively, add a small pin or friction bump near the open end: sketch a 1mm semicircle on the channel wall, extrude 0.5mm inward. This creates a slight interference that holds the rail in place after sliding fully in.

When to use: When you want that satisfying mechanical slide-together feel. Modular shelving, stackable organizers, decorative assemblies. For the purifier stand, a dovetail rail lets you slide legs onto the plate from the side — it's more work than pins but looks and feels premium.

Step-by-Step: Splitting the Air Purifier Stand

Open the Air Purifier Stand design from Chapter 10 (or create a copy first — File > Save As — so you keep the original). We're going to split it into two bodies, add alignment pins, and export each piece separately.

Step 1: Verify Your Starting Point

You should have a single body in the Browser panel: the complete Air Purifier Stand with a 200mm top plate, a 180.5mm groove, and 4 legs. If you don't have this, go back to Chapter 10 and build it first.

The key insight: always design as one body first, then split. It's much harder to modify a split design — dimensions, fillets, and features all reference the original body. Get the shape right, then cut it apart.

Step 2: Create a Construction Plane for the Split

We need to tell Fusion where to cut. The split goes right where the legs meet the plate — the underside of the top plate.

1. Go to Design > Construct > Offset Plane (or press S and search "Offset Plane")
2. Select the bottom face of the top plate — this is the flat surface where the legs connect
3. Set the offset to 0 mm (we want the plane right on that face)
4. Click OK

A translucent orange plane appears at the split location. This is a construction plane — it doesn't become part of the model, it's just a reference tool. You'll see it listed under "Construction" in the Browser panel.

Step 3: Split the Body

This is the moment of truth — one body becomes two.

1. Go to Design > Solid > Modify > Split Body (or press S and search "Split Body")
2. Body to Split: click on the Air Purifier Stand body
3. Splitting Tool(s): click the construction plane you just created (or the bottom face of the plate)
4. Click OK

Immediately you'll see two separate bodies appear in the Browser panel under "Bodies." They might have generic names like "Body1" and "Body2."

5. In the Browser panel, right-click the first body (the top plate) → Rename → type TopPlate
6. Right-click the second body (legs + base ring) → Rename → type Legs

You now have two bodies that together look identical to the original — but they're separate objects that can be exported independently.

Step 4: Add Alignment Pins to the Legs

We'll add cylindrical pins on top of each leg. These will push into matching holes in the plate during assembly.

1. Work on the "Legs" body — in the Browser panel, make sure the Legs body is visible (lightbulb on). You may want to temporarily hide the TopPlate body (click its lightbulb to toggle visibility) so you can easily click faces on the legs without accidentally selecting the plate
2. Create a new sketch on the top face of one leg — click the flat top surface of any one leg
3. Press C for the Circle tool → click the center of the leg face → type 4 for 4mm diameter → press Enter
4. Press Finish Sketch (or the green checkmark)
5. Press E for Extrude → the circle highlights → type 4 mm upward
6. Set Operation to Join (this merges the pin cylinder into the Legs body)
7. Click OK

You now have a single 4mm × 4mm pin sticking up from one leg. Now replicate it to all four legs:

8. Go to Design > Solid > Create > Pattern > Circular Pattern
9. Pattern Type: Features
10. Objects: select the Extrude feature you just made (click the pin, or select it in the Timeline)
11. Axis: select the Z axis (the vertical center axis of the stand)
12. Quantity: 4
13. Click OK

All four legs now have identical pins pointing upward. Each pin is 4mm in diameter and 4mm tall.

Step 5: Add Matching Holes to the Plate

The holes need to be slightly larger than the pins to allow assembly. We'll use 4.3mm diameter for a sliding fit (0.3mm total clearance).

1. Select the "TopPlate" body — in the Browser panel, make sure it's visible (lightbulb on). You may want to hide the Legs body temporarily so you can easily select the plate's faces
2. Create a new sketch on the bottom face of the plate
3. Press C → draw a circle at the same position as one pin: 4.3 mm diameter
4. Use Sketch > Project (shortcut P) to project the pin center points from the Legs body onto your sketch — this ensures exact alignment (turn the Legs body back on temporarily if you hid it)
5. Constrain each hole center to a projected pin center with Coincident
6. Finish Sketch
7. Press E → Extrude: -4 mm (negative = cutting into the plate, leaving 1mm of material on top)
8. Set Operation to Cut
9. Click OK

Repeat for all four holes, or use Circular Pattern again (same axis, same quantity of 4) to cut all four in one operation.

The plate now has four 4.3mm × 4mm deep blind holes that line up perfectly with the four 4mm pins on the legs. The remaining 1mm of plate material at the top keeps the surface clean — no visible holes on the groove side.

Step 6: Add Chamfers for Easy Alignment

Small chamfers on the pin tips and hole entries make assembly much easier — the tapered surfaces guide the parts together even if they're slightly misaligned.

1. Go to Design > Solid > Modify > Chamfer
2. Select the top edge of each pin (the circular edge at the tip) — hold Shift or ⌘ to multi-select all four
3. Set Distance to 0.5 mm
4. Click OK — each pin now has a tapered lead-in tip

5. Run Chamfer again
6. Select the entry edge of each hole (the circular edge on the bottom face of the plate)
7. Distance: 0.5 mm
8. Click OK — each hole now has a funnel-shaped lead-in

The chamfers create a self-centering effect: even if you're off by a fraction of a millimeter, the taper guides the pin into the hole.

Step 7: Test Fit Visually

Before exporting, verify everything lines up:

1. Press M for Move → select the TopPlate body
2. Move it 20 mm upward (Z axis) — this separates the two pieces visually
3. Orbit around and check: do the pins and holes line up? Do the chamfers look right?
4. For precision checking: go to Design > Inspect > Section Analysis → place a section plane that slices through a pin-hole pair → verify the clearance gap is visible
5. When satisfied, press ⌘Z to undo the move (or press M and move it back)

Step 8: Export Each Body Separately

Each body becomes its own STL file:

1. In the Browser panel, right-click "TopPlate" → Save as Mesh
2. Format: STL (Binary), Refinement: High
3. Save as TopPlate.stl
4. Right-click "Legs" → Save as Mesh
5. Save as Legs.stl

You now have two separate STL files, each ready to be sliced and printed in its optimal orientation.

Printing Strategy for Split Parts

This is where splitting pays off — each piece can now be oriented for perfect print quality.

The Top Plate (TopPlate.stl)

• Orientation: Print groove side UP — the flat bottom sits on the bed for a perfect surface finish
• The groove is now an upward-facing recess — no overhang, no bridging, no supports needed!
• The pin holes on the bottom face are on the bed — they print fine as simple circles
• Settings: 0.2mm layers, 3 walls, 20% infill

The Legs (Legs.stl)

• Orientation: Print legs pointing up (pins at the top)
• The base ring sits flat on the bed — great adhesion and stability
• Legs grow vertically — no overhangs whatsoever
• Pins are small cylinders on top of the legs — they print fine
• Settings: 0.2mm layers, 4 walls, 25% infill (legs need structural strength)

Assembly

1. Test fit: Push the pieces together. The pins should slide into the holes with slight resistance.
2. Too tight? Sand the pins lightly with 220-grit sandpaper, test again.
3. Too loose? Add a small drop of CA (super glue) into each hole before pushing the pieces together.
4. Press firmly until the plate sits flat on top of the legs — the chamfers will guide everything into alignment.
5. Done. The stand is assembled and ready to use.

Tolerance Reference

Tolerances are the clearance gap between mating parts. Here's a quick reference for pin-and-hole joints (assuming a 4mm pin):

When to Split vs. Print as One Piece

Not every model should be split. Splitting adds complexity — more design work, two print jobs, and an assembly step. Here's when it's worth it:

Assembly Method Decision Guide

Once you've decided to split, pick the right assembly method for your situation:

Design Dimensions

Every dimension in this project traces back to the ISO 7810 standard card size. Here's the full breakdown:

New Skills in This Project

• Shell tool — hollowing a solid body to create a pocket with uniform wall thickness. You used this before (Chapter 17), but here the shell depth matters more because the card is only 0.76mm thick.
• Snap-fit with relief slot — a flexible tab with a bump that catches the card edge. The relief slot behind the tab allows it to flex inward when the card pushes past. Same engineering principle as the Echo Dot mount (Chapter 14) and Cable Organizer lid (Chapter 17).
• Chamfers for usability — angled lead-ins at the card entry point so the card slides in smoothly without snagging. A small detail that makes the design feel professional.
• Multi-feature design — combining a pocket, snap lock, push-out window, thumb recess, and keychain hole into one compact body. Planning feature placement so nothing conflicts.

Step 1: Create the Outer Body

Start with a solid rectangular block at the corrected dimensions. Every measurement traces from the card size + clearance + wall thickness.

Step 2: Shell It Out

The Shell tool removes the interior of a solid body, leaving a uniform wall thickness. By selecting the top face, we create an open-top pocket — the card slot.

Step 3: Cut the Push-Out Window

A rectangular window on the back (bottom face) of the holder lets you push the card out with your thumb from behind. Without this, you'd need tweezers to extract a flush-sitting card.

Step 4: Create the Snap-Lock Tab

This is the functional heart of the design — a small flexible tab on the inner right wall with a tiny bump that catches the top edge of the card when fully inserted. The card pushes past the bump going in (click!), and the bump prevents it from sliding back out.

Step 5: Cut the Relief Slot

The snap tab won't flex without a relief slot behind it. This is the critical engineering detail — a narrow slot cut through the wall, directly behind the tab, that lets it deflect inward when the card pushes past.

Step 6: Add the Release Button Recess

To release the card, you need to press the snap tab inward from the outside. A small thumb recess on the outer wall — aligned with the tab — gives you a target to press.

Step 7: Add the Keychain Hole

A small hole in one corner lets you attach the holder to a keyring or lanyard. We'll reinforce the area around the hole to prevent stress cracking.

Step 8: Fillet All Outer Edges

Rounding the outer edges makes the holder comfortable in your pocket and pleasant to grip. Inner edges get a smaller fillet to help the card slide smoothly.

Step 9: Add Card-Guide Chamfers

The final usability touch — chamfered lead-ins at the top opening of the pocket. These create a funnel effect so the card enters smoothly even when you're not looking.

Step 10: Export for Printing

🖨️ Printing This Design

This is a single-body print with no supports required — if you orient it correctly. The snap-lock mechanism is the only tricky feature, and it prints fine with the right material.

Orientation

Open side UP — place the holder on the build plate with the pocket opening facing the ceiling. The bottom wall sits flat on the bed. All four side walls grow vertically — zero overhangs. The snap tab is a small feature on the inner wall that prints as part of the vertical wall growth. The relief slot is a 1mm gap in a vertical wall — the slicer bridges across it cleanly (it's only 1mm, well within any printer's bridging capability).

The push-out window on the back is now on the build plate surface. Since we cut it as a through-hole, the slicer simply doesn't print material there — the bed IS the bottom of the window. Clean first-layer finish.

Support Strategy

No supports needed. Every feature is either a vertical wall, a through-cut, or a surface detail on a flat face. The relief slot (1mm bridge) and keychain hole (5mm vertical through-hole) are the only potential bridge points — both are trivial for any FDM printer.

Recommended Print Settings

Dimension Validation

How It Works

Keep Going with Parameters

You used User Parameters in Chapter 18 to drive the phone stand's angle and width. Apply the same approach to every future design. Name your variables well (purifier_base, not d1), and use expressions like purifier_base + 0.5 in dimension fields. One parameter change → entire model updates.

Advanced Topics to Explore

Learning Resources

• Product Design Online (YouTube) — Best structured Fusion tutorial series, perfect next step after this guide
• Maker's Muse (YouTube) — Practical 3D printing design tips, tolerance guides, real projects
• r/Fusion360 — Active community, post your designs for feedback
• Autodesk Forums — Official support, answered by Autodesk staff
• Official Shortcuts Guide — Complete keyboard shortcut reference from Autodesk

More Practice Projects

Ideas, roughly ordered by difficulty: