Stump The Chump - How would you model this?

Brad Tallis
2 days ago
7 min read

Have you ever looked at a 3D part and immediately thought, "That has to be a loft"? Sometimes the most obvious solution isn't the simplest one. A customer recently sent me a drawing of an angled component, asking for the best way to model it. While my first instinct was to use the loft command in Fusion, that path led to several unexpected challenges. This blog post details that full, problem-solving journey. I'll show you the loft-based method I first used, including the fixes for the issues I found. I'll also reveal a much simpler, alternative method I discovered at the end that likely created the original part. You'll learn two powerful approaches to tackling tricky 3D geometry.

Starting with the Foundation and Framework

The part has a rectangular base with angled sides supporting a circular top section. The first step is always to set up your workspace correctly. I started a new design in Part Design and set the units to millimeters, matching the engineering drawing.

Creating the Base Plate

I began a sketch on the top (XY) plane.
Using a center rectangle, I defined the main footprint: 104 mm by 100 mm.
I then drew lines to create the 8° angled sides shown in the top view of the drawing.
Once the sketch was fully constrained, I extruded the center profile to a height of 10 mm to form the solid base.

Establishing the Circular Profiles Next, I needed to create the circular top section.

I sketched on the front (XZ) plane.
I drew three concentric circles.
Using the drawing's dimensions, I set their radii to 32 mm, 25 mm, and 15 mm.
I positioned the center of these circles 135 mm up from the base and 150 mm over from the origin.
With the sketch done, I extruded the profiles. A key trick here is using the symmetric option. Since my base sketch was centered, extruding symmetrically in both directions from the front plane perfectly centers the cylinders on the part. I extruded the outer ring with a whole length of 36 mm and the inner ring to 46 mm.

The Loft Method: Building the Angled Support

With the base and top circles built, the challenge was the angled support connecting them. My plan was to use a loft between a profile on the base and a profile projected onto the cylindrical surface.

Creating the Profile Sketches

First, I sketched the side profile of the support on the front plane.

Using the line command, I started by clicking and holding on the outer circle to generate a tangent line automatically.
I drew the profile based on the drawing's dimensions: a height of 22 mm, a 60° lower angle, and a 45° upper angle.
I added the specified fillets: a radius of 15 mm at the bottom corner and a radius of 10 mm at the other corner.
This gave me a fully constrained "side profile" sketch to use as a guide rail.

Next, I created the loft's starting profile on the angled face of the base.

I sketched directly on that angled top face.
Using the midpoint line command, I drew a 65 mm line that expands equally from its center point. This is a fantastic tool for creating symmetric geometry.
I completed the rectangular profile, making sure it was parallel to the base's edges and fully constrained. I named this sketch "top angled profile."

Projecting Geometry and the 3D Sketch Challenge

The loft needs a second profile at the top. We must project the shape from the base up onto the cylindrical surface.

Using Project to Surface

I edited the "top angled profile" sketch and projected the inner hole of the cylinder through it.
I extended the profile lines to the center of this projected circle.
To get these lines onto the curved surface, I used Create > Project to Surface.
I selected the outer cylindrical face as the target and the extended profile lines as the curves.
Setting the projection type to "Along Vector" and choosing the Z-axis correctly wrapped the lines onto the cylinder's surface. I turned off "Projection Link" so I could later edit these lines, then used the Fix constraint to lock them in place.

Building the Final Profile with 3D Sketch

The projected lines were floating above the original sketch plane. To connect them and form a closed profile, I had to use a 3D sketch.

In a 3D sketch, the midpoint line command can snap between points and lines in 3D space.
I created lines from the center out to the angled edges to form the closed profile on the cylinder.
I used the Trim command to clean up extra geometry. Now I had my secondary loft profile.

Executing the Loft and Troubleshooting Issues

I switched to the Surfacing tab and activated the Loft command.

I selected the base profile and the new 3D profile on the cylinder as my two sections.
I added the "side profile" sketch as a rail to guide the loft's shape. Using chain selection made it easy to select the entire sketched path.
The initial preview showed a clean shape. However, when I tried to add the other side as a second rail, it created unwanted dimples and wrinkles in the surface. The software struggled because the rails weren't along the exact path of the final edges.

Solution: Lofting Thin Strips

Instead of lofting the entire complex profile at once, I lofted it as two thin strips.

I used Loft, selecting one edge from the base profile to its corresponding edge on the top profile, with the side sketch as the rail.
I repeated this for the other side edge. This created two clean, separate surface faces.

Patching and Stitching into a Solid

To close the ends of the support, I used the Patch command to create surfaces for the front and back faces.
A problem arose: one long edge needed to be broken into segments for the patch to work. I edited the original sketch and used the Break command at the intersection points.
With all surfaces created, I used Stitch to sew them into a single, watertight solid body.
Finally, I used Combine to join this new solid body with the base and the circular top.

Overcoming a Hidden Geometry Problem

Even after combining, the model looked strange at the joint between the support and the cylinder. Using Inspect > Section Analysis revealed the issue: a tiny gap.

The patched end surface had a slight curvature, preventing a clean merge. Here was my fix:

I used Offset on the cylindrical surface with a distance of zero. This created a copy of that face.
I used this copied surface with the Trim command to cleanly cut the end of the support body.
I re-patched, re-stitched, and re-combined. This resulted in a perfect, clean intersection.

Completing the Part Details

With the main form complete, I finished the part based on the drawing.

Adding Internal Geometry

I edited the original side profile sketch to add a rectangular window based on given dimensions (21 mm offset, 46 mm up, 65 mm from center).
I extruded this profile symmetrically through the entire support.
I used the Shell command with an 8 mm thickness to hollow out the inside of the support stand.
I added Rule Fillet to apply a 5 mm radius to all edges of the window extrusion at once.

Modeling the Mounting Pads

I sketched on the top face of the base, projecting the body's edges for reference.
Using the drawing, I created the profile for the mounting pads: a Ø10 mm hole inside a 10 mm radius pad, positioned 76 mm apart and angled 30° from center.
A key trick: using a diameter dimension from a centered construction line to position the pads.
I extruded these profiles. Important: I made sure to select the profile edges behind the angled support face so the extrusion would fully merge with the angled geometry, leaving no gaps.
I used the Hole command to create the Ø10 mm through-holes, which is better for drawings and future edits than extruding cuts.
I mirrored these pad and hole features to the other side of the part.

Creating the 45° Angled Cut For the final 45° slice through the cylinder, I used a quick method:

Construct > Plane at Angle. I simply selected the cylindrical face, and Fusion generated a temporary axis. I entered 45°, creating the plane.
I then used Modify > Split Body, selecting that plane as the splitting tool, and removed the leftover piece.

A Simpler Alternative Method Revealed

As I finished, I noticed my model had two distinct edges along the support-top joint, while the drawing showed only one. This hinted that the original part might have been made differently.

I explored an alternative method that is likely the true, simpler way the part was designed.

The Intersect Method

I started by extruding the original "top angled profile" sketch straight up to the full height of the circular top (135 mm - 10 mm + 32 mm).
This created a simple, tall, angled block.
I then took the "side profile" sketch and extruded it symmetrically using the Intersect operation.
This command keeps only the volume where the new extrusion and the original block overlap.
The result was the perfect angled support shape in just two steps, with clean, single edges where it meets the cylinder.

This method avoids all the complexities of lofting, projecting to surfaces, 3D sketching, and surface patching. The rest of the features (window, shell, pads, holes, fillets) are added the same way.

Conclusion: Choosing the Right Tool for the Job

This project was a powerful lesson in 3D modeling problem-solving. The loft method is a valid, powerful technique for creating complex, organic shapes. You learned how to:

Use project to surface along a vector.
Employ 3D sketches to connect geometry in space.
Troubleshoot loft issues by using simpler sections and rails.
Use section analysis to find hidden geometry problems.
Patch and stitch surfaces into a solid.

However, the alternative method—using a simple extrusion followed by an intersect operation—shows the value of stepping back and re-evaluating the design intent. Often, a simpler, more direct approach exists. It creates a cleaner model with less computational history and fewer potential errors.

Both techniques are essential tools. The first builds your advanced skill set for truly complex shapes. The second reminds you to always look for the most efficient path to your final goal. Try modeling this part both ways in Fusion to solidify these concepts and expand your modeling toolbox.