Creating the same design 3 different ways
There can be multiple different ways to design a part in Fusion. We'll show how to create a part three different ways, and each method reaches the same final shape.
1. Revolve a constrained profile
Use constraints to keep the sketch simple
Create a centerline from 0,0 before drawing the profile. Fusion can use it to create diameter dimensions and later select it as the revolve axis. Set the overall height to 77.5 mm, then sketch the basic shape of the profile.
To make sketch relationships clear, draw lines slightly out of position before adding constraints. Add a horizontal constraint to make a line snap into place. Use collinear constraints to line up edges, and an equal constraint to make matching gaps the same width. This avoids adding separate dimensions for geometry that should match.
Dimension the profile from the drawing. The centerline lets Fusion create a 90 mm diameter dimension directly. The sketch also uses dimensions including 3 mm, 10 mm, 15 mm, 20 mm, and 7.5 mm. Equal and collinear constraints make related gaps and edges update together. Finish by checking that the sketch is fully constrained.
We'll keep the center hole out of this profile and add it later with Fusion’s Hole command.
Add the tabs, pattern, and hole
After finishing the sketch, use Revolve. Fusion recognizes the centerline and selects it as the axis.
Sketch one of the tab profiles on the flange face. Use a construction circle with a 140.1 mm diameter to locate them. Add the tabs 15 mm diameter circle and a second circle with a 16 mm radius, then constrain the relevant point vertically with the origin.
Extrude the tab profile to the bottom face. This keeps the tab’s thickness matched to the bottom flange if that flange changes. Add a 20 mm radius fillet to the tab edges.
Pattern the extrude and fillet features with a circular pattern. Select the Z axis as the pattern axis. If it is hidden inside the part, click and hold to choose it from the selection list. The pattern defaults to three instances.
Add a 5 mm radius fillet where the main cylinder meets the flange.
Create the center hole with the Hole command. Set its diameter to 75 mm and its extent to All so it passes through the part. I prefer this approach because the hole stays separate from the sketch and is easy to change, such as adding a countersink later.
2. Combine cylinder primitives with a sketch
This method begins with two cylinder primitives, then uses a sketch to cut the grooves.
Set the cylinder heights from the drawing
Create a cylinder with a 120 mm diameter and a 7.5 mm height for the wide bottom disc. Then start a second cylinder from the bottom face and set its diameter to 90 mm.
The drawing gives the taller cylinder’s height from the bottom, so enter 77.5 mm from that reference instead of calculating a height from the top of the disc. Drag the arrow upward, enter -77.5, and change the operation from Cut to Join when Fusion detects the overlap.
Sketch and revolve the grooves
Create a sketch on the front plane. Use the Project command and set the selection filter to Bodies and project the whole body. This brings the side edges into the sketch.
Draw two rectangles for the grooves. Make their matching lines equal, then dimension the sketch according to the drawing. Check that the sketch is fully constrained.
Use Revolve to cut the groove profiles. Since this sketch has no centerline, select the part’s face as the axis. Add the 75 mm through-hole with the Hole command and then add the 5 mm fillet.
Copy the tab sketch instead of redrawing it
To create the tabs, copy the sketch from the first design and paste it into the new one. The pasted sketch may include projected geometry linked to the original model. Turn off the bodies, delete the two unwanted circles and remove any stray geometery if it exists.
Move the remaining circle off center, then constrain its point to the origin.
Extrude the tab sketch to the object and make sure the operation joins the body. Add the 20 mm fillets, then circularly pattern the extrude and fillet features together.
Copying the sketch saves time because the tab geometry does not need to be recreated.
3. Build the part with Extrude From Object and offset
This approach uses one sketch to define most of the part, then builds the shape in layers.
Draw the main circles in one sketch
Start a sketch on the top plane. Add circles for the 90 mm and 120 mm diameters, the 75 mm center hole, and the circle defining the size of the grooves.
The groove circle sits 3 mm in from each side of the 90 mm circle. Because the sketch uses a diameter, calculate the new diameter as 90 - 6 = 84 mm. Fusion can show the equation when you hover over the dimension.
Extrude the profiles from existing faces
Extrude the top ring and center hole downward by 5 mm. Turn the sketch back on, select another profile, and use Extrude From Object to start the extrusion from an existing face. You can use this method to build the next levels from their actual starting faces.
Continue creating the object-based extrusions, including distances of -10 mm and -20 mm. The drawing identifies the final segment as 15 mm. For a case where that dimension is unavailable, we can build the bottom section another way, using Extrude Offset.
Select the needed profiles and use Extrude Offset. Set the offset to -77.5 mm and the extrusion distance to 7.5 mm. This places the profile 77.5 mm down, then extrudes it upward 7.5 mm. Measuring the result confirms a 15 mm distance between the faces.
From there, use Extrude From Object with the extent set to To Object. Select the target face, and Fusion finds the distance needed to join the remaining geometry into one body.
Reuse the tab sketch and finish the pattern
Paste the tab sketch again, remove the two unneeded circles, and confirm that the sketch is fully constrained. Extrude the tab and use a circular pattern to finish the part.
Grouping extrusions can make the timeline easier to read
The revolve method produces the shortest timeline. The primitive method takes a couple more steps, while the offset method creates more extrusion features in the timeline. In the longer timeline, select the extrusions, right-click, and choose Create Group to make the feature history easier to scan.
A clear timeline can help explain how a part was built, even when the design uses many features.
Conclusion
As you can see, there can be multiple different ways to design the same design in Fusion. The Revolve method took longer to create the sketch, but created the shortest timeline. The Primative method created simpler sketches, but required a few more steps. And lastly, the Extrude Offset method used only one sketch, but might be more difficult for someone to understand how the part was created.
Comments