Tutorial 7: A PCB-Aware Enclosure

Goal#

Build a design where the printed circuit board and its enclosure are linked. You will create a small 50 mm x 35 mm board with a microcontroller header, a USB-C connector, an LED and a pushbutton; switch it to a 3D PCB; use the board outline and connector positions to create an enclosure that automatically follows; then move a part on the board and watch the enclosure cutouts update. This is the core promise of having ECAD and MCAD in one tool.

The project is deliberately modest electrically so that the focus stays on the mechanical-electrical interface: board outline, mounting holes, keep-out zones, component heights and connector openings. It builds on Tutorial 2 (the snap-fit enclosure) but replaces manually typed board dimensions with references to the real board.

What you'll learn#

• Creating an electronics design with schematic and board from Fusion's Electronics workspace.
• Making sure each part has a 3D package so the 3D PCB is not full of plain boxes.
• Switching the board to 3D PCB and opening the resulting PCB design.
• Inserting the board into an enclosure design as an external reference.
• Deriving the board outline and mounting holes for the enclosure sketches.
• Placing connector cutouts using the connector's real position.
• Updating after changes and handling out-of-date references.

Prerequisites#

• Tutorial 2, and the Electronics section pages on schematics and board layout.
• A signed-in Fusion account. Electronics features have limits in the free Personal-use license (reported as 2 signal layers and 80 cm2 of board area; these figures are not in Autodesk's help, see Personal-Use Limits). A 50 x 35 mm (17.5 cm2) two-layer board is inside them.
• Roughly 60 to 90 minutes. If you only care about the mechanical side, you can use a pre-made board from the library and skip the routing steps.

Plan of the system#

Steps#

Part A: The electronics design#

1. Create the electronics design. Choose New > Electronics Design > Create New (Common tab). Save it as Sensor Board in your project.
2. Schematic. In the schematic editor, choose Place > Place Components and place: a USB-C receptacle (for example a 16-pin power-only receptacle from the library), a 2x5 pin header, a resistor, an LED, and a tactile switch. Wire them with the Net tool (Connect > Net): VBUS to the header, a 330 ohm resistor from header pin 1 through the LED to ground, the switch from header pin 3 to ground. Name the nets VBUS, GND, LED_A, BTN.
3. Run ERC. Run ERC from the Validate toolbar of the schematic and resolve warnings. Details are in the ERC and DRC page.
4. Switch to board. Choose Switch > 2D PCB. All components appear beside the board outline.
5. Set the outline. A new 2D PCB already has a default rectangular outline on the BoardOutline layer (formerly Dimension, layer 20). Edit it with the Board Shape tools (Outline Polyline, Outline Arc and so on) so it is a single closed 50 x 35 mm shape with 3 mm corner radii.
6. Place the parts. Use Modify > Move and place the USB-C at the left edge center (X = 2, Y = 17.5), the button at X = 42, Y = 17.5, the LED at X = 36, Y = 28 and the header at X = 25, Y = 6 (centered 6 mm from the long edge). Position values can be checked in the part properties.
7. Mounting holes. Use Place > Hole (NPTH) to place four 3.2 mm holes at (3.5, 3.5), (46.5, 3.5), (3.5, 31.5) and (46.5, 31.5).
8. Route. Use Route Manual or QuickRoute > Autorouter on a two-layer board. Add a ground pour on the bottom layer with Copper Pour. Run DRC and fix errors. For more on routing, see Routing and Autorouter.

Part B: 3D packages#

9. Check 3D models. Every component needs a footprint with a 3D model; you will see this in the 3D PCB (step 11). If a part shows as a plain box, its package has no 3D model; choose a different library part or attach one in the Content Manager (see Libraries page).
10. Component heights. Typical heights (check your actual parts): USB-C connector about 3.3 mm, button about 4.3 mm, 2 x 5 header about 8.5 mm. Confirm them in the 3D PCB later.

Part C: Switch to 3D PCB#

11. Create the 3D PCB. In the 2D PCB toolbar choose Switch > 3D PCB. If no 3D PCB exists, Fusion creates and links one (this replaces the old Push to 3D PCB workflow). Generation options are under PCB > 3D PCB Settings.
12. Open it. The 3D PCB opens as a separate design. Rotate it: you should see solder mask, copper, component bodies and mounting holes. Use the ViewCube to look at the top.
13. Save. Save the 3D PCB design so the project has a version.

Part D: The enclosure design#

14. New mechanical design. File > New Design, name it Sensor Enclosure.
15. Insert the board. In the Data Panel, right-click the Sensor Board 3D PCB and choose Insert into Current Design. The board is inserted as a linked component with a link icon in the browser. See External References.
16. Ground the board. Right-click the PCB component > Ground to Parent. Move the board so its bottom face is at Z = 5 mm above the origin XY plane (Move/Copy with Z = 5 mm), leaving room for 5 mm standoffs; the top of the standoffs' floor is then Z = 0 and a 2 mm floor lies below it.
17. Check orientation. The USB-C should point toward -X. If not, rotate the component in the enclosure design with Move/Copy.

Part E: Derive the outline#

18. Create the base component. New Component Base.
19. Sketch from the board. Create a sketch on an offset plane at the board bottom (Z = 5 mm), and use Project to project the board outline edges. The projection is associative: if the board gets longer, the sketch follows after the update.
20. Offset. Using Offset (O), offset the outline outward by 0.4 mm (clearance) then another 2 mm (wall). Result: two loops. If you prefer a parametric offset, define clear and wall as user parameters in the enclosure design and use clear + wall.
21. Extrude the walls. Select the area between the outer loop and the inner offset loop; extrude with Direction Two Sides: 12 mm up (board 1.6 + header 8.5 + about 2 mm margin) and 5 mm down to Z = 0. Then sketch the outer loop on the Z = 0 plane and extrude it 2 mm downward as the floor, Operation Join.
22. Standoffs. Use the projected mounting hole circles. Sketch circles of diameter 7 mm on the Z = 0 plane at the projected mounting hole centers and extrude them up to the board bottom (To Object, select the board's bottom face; 5 mm). Then use Hole with diameter 2.5 mm for M3 screws, depth 8 mm.

Part F: Connector cutouts that follow the board#

23. Cut the USB-C opening. Sketch on the outside face of the short wall (-X end). Project the USB-C body edges from the PCB (you can project a component's silhouette if the component is visible and not in a hidden state). Offset the projected rectangle by 0.5 mm outward for clearance. Extrude Cut through the wall.
24. Button hole. (Do steps 24 and 25 after creating the Lid in step 26.) On the lid, project the center point of the button from the PCB, add a 4.5 mm hole (or a 3.2 mm hole for a button cap). Because the point is projected, moving the button on the PCB later moves the hole after the lid regenerates.
25. LED light pipe. Project the LED center to the lid and cut a 3.2 mm hole; add a 1 mm counterbore on the inside.

Part G: The lid#

26. Lid. New Component Lid and use the Tutorial 2 approach: plate with a rim and either snap hooks or four screws to bosses. Use the base's inner loop for the rim projection.

Part H: Round trip#

27. Change the board. Return to the electronics design and move the button 5 mm to X = 37. Re-run DRC, then choose Switch > 3D PCB again; an Out-Of-Date indicator marks the documents that need updating.
28. Update the reference. In the enclosure design an Out-Of-Date icon appears in the Application bar; click it and review the update (synchronization is a pull). The projected button hole follows.
29. Change the outline from the mechanical side. If you decide to widen the board, edit the outline in the electronics design and update. Push to 2D PCB (3D PCB > Modify) also exists for changes made from the mechanical side; see the 3D PCB page.

Checkpoints#

• Inspect > Interference between the PCB component and Base reports none; the header is fully inside.
• The gap between the board edge and the inner wall measures 0.4 mm on all sides.
• Moving the button on the PCB and updating moves the button hole in the lid.
• The timeline has no red icons after update.
• A section through the USB-C connector shows the opening 0.5 mm larger than the plug body all around.

Variations#

1. Add a second board (a stacked sensor board) and compute standoff heights from the connector.
2. Create a sheet metal version of the base with the Sheet Metal workspace.
3. Add a clear light pipe body printed in transparent PETG.
4. Use configurations to switch between with-header and no-header builds.
5. Add a vent area above hot components after running a thermal check (see Simulation section).

Troubleshooting#

Related#

• 3D PCB and ECAD-MCAD Sync gives all push and pull options.
• Board Layout, Schematic Capture, Libraries pages for the electronic steps.
• Derive and External References explain linked geometry.
• Tutorial 2 for the snap fit details.