Tutorial 1: A Simple L-Bracket

Goal#

Build a sturdy L-shaped mounting bracket that holds a small panel or sensor to a wall. The finished part is 60 mm wide, with a 50 mm base leg and a 40 mm upright leg, both 4 mm thick, a triangular gusset for stiffness, two slotted holes in the base and two round holes in the upright. You will drive every important size from named parameters so you can resize the bracket in seconds.

This is the first tutorial in the section because almost every other project reuses its moves: sketch on a plane, constrain, extrude, add holes, fillet, and check the result. Work through it slowly, even if you have used CAD before, because the habits you form here (fully constrained sketches, parameters, a clean timeline) make the later tutorials faster.

What you'll learn#

• Starting a design with units and a named component.
• Creating user parameters for thickness, width and hole sizes.
• Sketching and fully constraining a profile with dimensions tied to parameters.
• Extruding a symmetric profile, then adding a gusset as a second feature.
• Placing holes with the Hole command and slots with a sketch cut.
• Applying fillets in the right order so they do not fail.
• Using the Inspect tools to check wall thickness and mass.
• Exporting STL (3D printing) and DXF (laser or waterjet cutting of a flat blank).

Prerequisites#

• Fusion installed and signed in (the free Personal-use license is enough).
• Comfort with orbiting, panning and zooming. See the ViewCube page in Getting Started.
• Awareness of the browser tree and timeline. If the timeline is hidden, enable it from the View menu or from the bottom bar.
• Roughly 30 to 40 minutes.

Set the document units to millimeters before you begin. Open the Browser, expand Document Settings, then Units, and confirm the unit is Millimeter. You can also set the default unit under Preferences > General > Default Units > Design.

Design intent#

Write down what the part must do before you click anything:

A 5.5 mm hole clears an M5 screw. Slots give you adjustment of about 8.5 mm along the leg after tightening.

Steps#

Part A: Parameters and the L profile#

1. Create a new design. Choose File > New Design. Press Ctrl+S and save it as L-Bracket in a project.
2. Open the Parameters dialog. Go to Modify > Change Parameters. Under User Parameters click the plus icon.
3. Add the first parameter. Name t, unit mm, expression 4, comment Material thickness. Click OK on the row.
4. Add the rest the same way. w = 60 mm; base_len = 50 mm; up_len = 40 mm; hole_d = 5.5 mm; slot_len = 14 mm; bend_r = t. Close the dialog.
5. Rename the root. In the Browser, right-click the top component name and rename it L-Bracket. Leaving this named keeps your later export file names tidy.
6. Start a sketch on the side plane. Click Create Sketch, then pick the XY plane in the origin folder. The profile of an L lies in a plane and the bracket's width runs along Z, so this is the right orientation.
7. Draw the outer outline. Press L for Line. Start at the origin and draw: right along X to about 50, up along Y to about 4, left to about 4 along X from the vertical, up to about 40, left, and back down to close the polyline. You are drawing six lines forming an L. Ignore exact lengths for now.
8. Add constraints. Fusion usually auto-adds horizontal and vertical constraints. Check that the first segment starts exactly on the origin (a coincident constraint at the origin point). If the origin point is not locked, drag nothing; use Constrain > Coincident and pick the corner and the origin.
9. Dimension the profile. Press D for Sketch Dimension. Click the bottom line and in the value box type base_len, then Enter. Click the left vertical line (the full height of the L) and type up_len. Click the short vertical edge at the right end of the base and type t. Click the short horizontal edge at the top of the upright and type t. Everything should turn black (fully constrained). If lines remain blue, add the missing dimension; see the Fully Constrained Sketches page for diagnosing which ones.
10. Check the thickness consistency. Both leg thicknesses are now t. Finish the sketch with the green check or press Enter on the Finish Sketch button.

Part B: Extrude the width#

11. Extrude. Press E. Select the L profile. Set Direction to Symmetric, Measure to Whole Length, and type w in the Distance field. The preview should be an L-shaped solid, 60 mm wide, centered on the XY plane.
12. Name the body. Operation is New Body. Click OK and rename the body Bracket in the browser.

Part C: Bend radii (fillets)#

13. Select inside corner. Press F for Fillet. Click the inside corner edge where the base meets the upright. In the radius box type bend_r.
14. Add the outside corner to the same fillet. Hold Ctrl or just click on the outside corner edge as well. Fusion lets you use multiple radius groups; click the plus to add a second group if you want a different value. Set the outside radius to bend_r + t so the two surfaces stay concentric. Click OK.
15. Fillet the free end corners. Press F again. Pick the four corner edges at the free ends of the legs (the edges that run through the 4 mm thickness at the left and right sides of the base end and of the upright top). Use a radius of 1.5 mm (less than half the 4 mm thickness, otherwise the two fillets on one end overlap and fail). These round the corners that would otherwise catch fingers.

Pause and name this feature "Bend Fillets" by right-clicking its timeline icon and choosing Rename. Naming features in the timeline pays off when you revisit the file.

Part D: Holes in the upright#

16. Hole command. Press H. Click the face of the upright that points in the +X direction (the inside face, on the same side as the base).
17. Plan the placement. Rather than dropping holes by eye, locate them with a sketch.
18. Use "From Sketch" placement. Cancel the Hole dialog, create a sketch on the same face, and add two points using Create > Point. Constrain each point: horizontal distance from the center line is 15 mm (so they sit 30 mm apart), vertical distance from the bottom outside edge of the upright is 18 mm. For a symmetric layout, draw a construction centerline first, then constrain the two points as Symmetric about it.
19. Hole parameters. Start Hole again. With Placement at From Sketch, select the two points. Set Hole Type to Simple, Diameter to hole_d, Depth to All or t. Confirm that the preview goes through the 4 mm wall only.
20. Finish. Click OK. The holes appear as one timeline feature.

Part E: Slots in the base#

21. New sketch on the base top face. Select the upper surface of the base leg and create a sketch.
22. Draw a slot. In Sketch > Slot choose Center to Center Slot. Click the first center, the second center, then drag to set the width, and type hole_d.
23. Dimension the slot. The center-to-center distance is slot_len - hole_d which gives an overall length of slot_len. Type that expression for the distance. Orient the slot's long axis along X. Locate the first slot with its center 20 mm from the upright's outer face (so it clears the 4 mm inside bend radius) and 12 mm from the side edge, then place the second slot symmetrically by mirroring about the width center line.
24. Cut. Press E, select both slot profiles, choose Operation Cut, set Extent to All (or 5 mm). OK.

Part F: Gusset#

25. Choose the sketch plane. The gusset lies in the same plane as the L profile, so no offset plane is needed; sketch directly on the XY origin plane.
26. Gusset sketch. Create a sketch on XY. Draw a triangle with one vertex at the inside corner of the L (point A, at X = 4, Y = 4), a second vertex 25 mm up the inside face of the upright (point B) and a third vertex 30 mm along the top of the base (point C), joined by a diagonal. Dimension: leg on base 30 mm, leg on upright 25 mm. Because the fillet sits in the corner, use Project (P) to bring in the inside edges and the fillet so the triangle meets them cleanly.
27. Extrude the gusset. Press E, select the triangle profile, set Direction to Symmetric, Whole Length 3 mm, Operation Join. The gusset is now a rib exactly at the center of the width.
28. Fillet the gusset. Apply a 1 mm fillet to the sharp end edges for printing quality.

Checkpoints#

Before moving on, check each of the following:

• The timeline holds about eleven items: Sketch, Extrude, Fillet, Fillet, Sketch, Hole, Sketch, Extrude (slots), Sketch, Extrude (gusset), Fillet. No yellow or red icons.
• In Modify > Change Parameters, editing t to 5 mm should regenerate the bracket without errors. If a feature fails, note which one; it tells you which dimension was not parameter-driven.
• Use Inspect > Measure on the slot: the width reads 5.5 mm and the length 14 mm.
• Inspect > Section Analysis cut through the center plane: the wall should read 4 mm everywhere except the gusset.
• Right-click the body > Properties shows the volume; the hand-calculated volume is about 20.4 cm3, so with aluminum 6061 (2.70 g/cm3) the mass is about 55 g. The exact value depends on the material you assign.

Variations#

1. Sheet-metal version. Replace the extruded L with a flange-based sheet-metal body. Use the Sheet Metal workspace and compare the flat pattern. See the sheet metal section of this guide.
2. Two-way gusset. Add a second gusset at 10 mm from each edge instead of one at center.
3. Countersunk holes. In the Hole dialog switch the hole type to Countersink with 90 degrees included angle.
4. Parametric family. Use configurations to create 40 / 50 / 60 mm widths in one file.
5. Print optimization. Rotate the part so the L lies flat on the bed; the gusset will print without support, and the holes remain accurate.

Troubleshooting#

Export#

• STL for printing. Right-click the body > Save as Mesh, choose STL (Binary), refinement Medium. Alternatively use the 3D Print command (see 3D print a design).
• DXF for cutting. For a flat blank of an aluminum bracket you need a flat pattern. In the Solid workspace you can approximate it: the developed length is base_len + up_len - 2*(t + bend_r) + bend allowance. Do it properly with sheet metal tools instead of hand-calculating.

Related#

• Sketch Basics and Dimensions in the Sketching section explain the constraint colors you used.
• Extrude and Fillet pages describe each option you toggled.
• Hole and Thread covers tapped holes in case you want M5 threads instead of clearance.
• Parameters Dialog covers favorites and expression syntax.
• Next in this section: the electronics enclosure.