How would you model this?

Tackling a tricky 3D model from a flat drawing can feel overwhelming, like piecing together a puzzle without all the edges. But what if you broke it down into bite-sized parts? In this guide, we'll model a flange mount step by step in Fusion. You'll see how to turn dimensions into a solid part, using smart tricks to keep things simple and editable. By the end, you'll learn how to handle complex shapes with ease.

Establishing the Foundation – The Revolving Base Feature

Start with the core of your flange mount: the cylindrical body. This sets the stage for everything else. Pull dimensions straight from the drawing, like diameters of 68 mm and heights of 23 mm. It's smart to build this first because it anchors the whole design.

Modeling the Initial Profile and Revolve Command

Create a new file and check your units are set to millimeters. Pick the front plane for your sketch. Draw a centerline from the origin at 0,0 to act as your revolve axis. Sketch a rough profile of the cylinder, ignoring small extras for now.

Make that bottom line horizontal with a quick constraint. Reference the profile's base to the origin with a Horizontal Constraint so it stays put.

Dimensioning for Full Constraint Success

Click the centerline, then an outer line, to add a diameter dimension. Do the same for 28 mm and 42 mm. Switch and do the height dims.

Your lines turn black, but the sketch might not show the lock symbol, signifying it is fully locked down or fully constrained. Hit auto constrain; it flags the centerline needs a dimension, say 40 mm. Now it's fully locked. Finish the sketch and revolve around that axis.

Building Out the Rectangular Body and Mounting Holes

With the cylinder in place, add the rectangular protrusion. This 90 mm by 60 mm base sticks out 7 mm, per the drawing.

Creating the Extruded Base with Centered Geometry

Sketch on the bottom face. Draw an 80 mm diameter circle first, then add a center rectangle inside, 90 by 60 mm. Center it at 0,0 for easy alignment.

Select the rectangle profile and extrude negative 7 mm.

Advanced Hole Placement: Filleting Before Drilling

Fillet the rectangle's corners to 8 mm radius first. This will create points to locate hole centers perfectly. For four 6 mm holes, project the filleted face to grab those radius points.

Use the hole tool's "from sketch" mode. Pick the points, then set the distance to through-all. One feature handles all four—way better than separate ones.

Sculpting Complex Contours and Mirroring Features

Now shape the recesses on the rectangle's underside. These 30-degree angled cuts remove 2 mm of material, with 5 mm radii. Symmetry screams for mirroring to avoid double work.

Sketching and Extruding the Symmetrical Recesses

On the bottom face, project the cylinder's edge and use tangent lines. Hold to snap tangent on the circle, then dimension the angle to 30 degrees from horizontal. Link the other side's angle to this one—change one and they both update.

Extrude the profile as a cut, negative 2 mm. Fillet the inner edges to 5 mm. Use the Mirror command and choose Features, then select the Extrude and Fillet Features from the timeline and mirror across the front origin plane.

Defining the Arm Geometry and Wrapping Features

The arm is the beast: curved, with slots and big radii like 108 mm. Build a rough mass first, then cut away extras. Project the body for a silhouette to guide your sketch.

Imagine roughing out clay, then trimming details. This mimics machining from stock, making the model logical.

Building the Arm Mass and Joining Bodies

Sketch on the front plane, project the full body for edges. Add 8 mm and 20 mm slots using center-to-center slot. Use the drawing to mock up the shape of the arm to the slot. Extrude the profile two-sided to the points where the cylinder joins the rectangular portion of the body. You'll end up getting two bodies—join them by extruding the flat face to the cylinder. Fillet the edges with selection sets: 5 mm on one, 10 mm on others, all in one go.

Removing Material with Large Radii Cuts

Create a new sketch on the arm's top: project the body, add lines at 71 mm and 28 mm from center. Use three-point arcs from end to end, set radii to 90 mm and 108 mm.

Cut extrude two-sided: all on one, to the top face on the other. Add 10 mm fillets around for smoothness. We've now machined away a majority of the material, leaving the detail of the arm.

Incorporating the Rib and Final Detailing

Finish with the rib: a 5 mm thick support that connects the cylinder and the arm like a brace.

Creating the Rib Feature with an Offset Plane

Offset a plane from the front: minus 48 mm, then another minus 7 mm. Sketch the profile on it—project the part, draw a centerline, then dimension the profile to 130 mm and 166 mm diameters.

Use the rib tool on the profile edge. Set thickness to minus 5 mm for the right side—it projects automatically to the cylinder. Fillet: 5 mm on one edge, 30 mm on another, via selection set.

Final Chamfers, Fillets, and Design Verification

Add a 3 mm hole: place 8 mm from one edge, 7 mm from another, through-all. Now, use the Mirror command and select all of the features that were used to define the arm. If the Mirror fails, try a different Compute Type, like Identical.

Chamfer small edges to 1 mm distance. For 0.75 mm fillets, select faces to grab chains fast. You can also click on edges to select whole edge chains.

To verify that your model behaves correctly, reactivate some of your sketches and then tweak a dimension, like the 60mm width to 65 mm and watch the model update.

Conclusion: Mastering Parametric Modeling Workflow

You've now built a full flange mount from a drawing, step by step. Break shapes into simple revolves, extrudes, and features for simplicity. Keep your sketches simple. Use mirror when possible, and group your timeline and name features to stay organized.

These steps help control your design. Test changes often to ensure features update correctly instead of waiting until the very end.