How to Create a Parametric Paper Towel Holder in Fusion
The parametric paper towel holder is modeled in Fusion from a primitive cylinder as its starting point. Its decorative grooves connect to the cylinder’s circumference and pattern quantity.
Start the Fusion Model with a 4 in Cylinder Primitive
Create a new design and choose Hybrid and inch. The customer supplied an image without dimensions, so use small example values: a cylinder primitive with a 4 in diameter and 4 in height.
Fusion can create a live parameter while you enter a value. In the cylinder diameter field, enter cylinder_diameter = 4. Open Change Parameters to see cylinder_diameter set to 4 and saved in Favorites.
Shell the Cylinder and Build the Tooth Profile
Pre-select the top face, right-click, choose Shell, and set the thickness to 0.2 in. The result is a hollow cup.
Select the top face again, right-click, and choose Create Sketch. Because the diameter might change, choose Project, select the face, and keep Projection Link turned on. The projected geometry gives the sketch lines a connection to the changing diameter.
The tooth-profile sketch setup starts with a line between projected points. Convert that line to construction geometry, then apply Horizontal/Vertical so it is vertical with the point at 0,0.
Draw the two tooth-profile lines by snapping them near the middle of the construction line. They begin at different lengths on purpose. Apply Equal to those lines, then make the matching point Coincident with the edge. Moving one point now moves the other like a mirror.
Add a dimension from one point to the other. The sketch becomes fully constrained, and you can finish it.
Extrude the Tooth Profile
Select the tooth profile, choose Extrude, and set the extent to To Object. Select the bottom face.
Use Offset instead of a distance. Entering 1 in sends the extrusion one inch past the selected object, so change it to -1 in. The extrusion then stays 1 in from the bottom, even if the cylinder height changes.
Pattern Tooth Feature Around the Cylinder
Start Rectangular Pattern, change the pattern type to Circular Pattern, and set Object Type to Features. Select the extrude, select the inside cylinder as the axis, and set the quantity to 50.
This first pattern looks close, but the teeth do not end at sharp points. The model may look fine from the current view, yet the spacing is not mathematically correct.
Calculate Tooth Spacing from the 12.57 in Circumference
Select the bottom edge and measure the circumference. The total length is 12.57.
Use this formula:
circumference / pattern quantity = tooth spacing
For 50 teeth:
12.57 / 50 = 0.2514
The sketch dimension is still 0.25, so edit the sketch and change it to 0.2514. Finish the sketch, and the teeth meet in sharp points around the cylinder.
Test the formula with a pattern quantity of 43. Calculate 12.57 / 43, copy the result into the tooth dimension, and finish the sketch. All the teeth match correctly.
Undo this test to return to a quantity of 50, then confirm the tooth dimension is 0.2514.
Center the 0.75 in Front Opening
Create a sketch on the top face and draw the rectangle for the front opening. Use the Horizontal/Vertical constraint to keep it centered.
Hold Shift while hovering over the edge to reveal the midpoint icon. Select the midpoint and align it vertically with 0,0. The rectangle now stays centered.
To keep the opening attached when the diameter changes, make one edge Tangent to the outside edge. Then make the matching point Coincident with that edge. If the cylinder gets smaller, the point follows it and continues touching the outside edge.
Set the opening width to 0.75 in. The sketch should now be fully constrained.
Select all the opening profiles and choose Extrude. Set the extent to To Object, then select the inside face instead of entering a distance. The opening will always reach the inside face.
Add the Opening Fillets in One Fusion Feature
Select the two large edges around the opening and choose Fillet. Set the fillet to 0.75 in.
Add a selection set, then select the two bottom edges. Set those smaller fillets to 0.1 in.
Fusion shows one fillet feature in the timeline, but that feature contains four fillets. This keeps the opening fillets easier to manage.
Fillet the Vertical Edges with a Crossing Window
The crossing-window edge selection handles the teeth without manually selecting every edge.
First, test Rule Fillet. Use the pattern as the rule and set the value to 0.02 in. The operation fails. Rounds Only also fails, while Fillets Only handles the inside fillets but also tries to round unwanted edges.
Switch back to Constant Fillet. A left-to-right window selects only items fully inside the window. To select the vertical edges across the model, drag from right to left for a Crossing Window.
The first crossing window selects 103 faces and 104 edges. To have Fusion not select the faces, open Select > Selection Priority and choose Edge Priority. Clear the selection.
Draw the crossing window again. It now selects only the 104 vertical edges.
Apply a 0.02 in fillet first. It works across the selected edges. Change the value to 0.05 in for the final result, where the teeth roll over each other.
Add the Center Post
Use another cylinder primitive for the center post. Set its diameter to 1" and its height to 10 in.
The top should have a flattened, rounded shape. A regular fillet creates a different top, so use Asymmetric Fillet to control how steep and shallow each side becomes.
Because the post diameter is 1 in, setting a fillet value to 0.5 produces an error. Use 0.499 instead, which leaves a very small point. Set the other value to 0.25, then accept the feature.
Add Fusion Parameters for the Cylinder and Tooth Pattern
Changing cylinder diameter from 4 in to 5 in at this stage creates warnings. The teeth no longer touch because the spacing still uses fixed values.
Using parameters replaces those fixed values with expressions.
Set the Circumference Expression
The design already has the cylinder_diameter parameter. Create a new parameter named circumference.
Set its unit to inch and use this expression:
cylinder_diameter * PI
Link the Circular Pattern to pattern quantity
Create another parameter named pattern_quantity. Set it to 50 and give it no unit.
Open the Parameters table, expand the pattern, and change its static 50 expression to pattern_quantity. The circular pattern now uses the parameter instead of a fixed number.
Change the pattern_quantity parameter to 60 as a test. The pattern updates, but the fillets show issues because they may be too large for that change. Set the parameter back to 50.
Link Tooth Width to the Circumference and Pattern Quantity
Create a parameter named tooth_width. Set its unit to inch and use this expression:
circumference / pattern_quantity
Fusion displays the calculated value as 0.25 at the shown precision. The earlier calculation gives the more exact value of 0.2514.
Expand the tooth-profile sketch and replace its static dimension with tooth_width. The model remains correct while the tooth width now follows the cylinder diameter and pattern quantity.
Test the 4 in, 5 in, and 6 in Diameter Values
With the expressions linked, change the cylinder diameter from 4 in to 5 in. The tooth width changes, and the fillets update.
One fillet fails at the edge around the opening width. The possible fixes are to parameterize that width or return to the model and add a fillet to that edge manually.
Change the diameter to 6 in. The opening stays relative to the cylinder diameter, while the teeth stretch and change width. Set the diameter back to 4 in.
Parameterize the -1 in Depth Offset and Cylinder Height
Select the tooth-profile extrude and create a parameter named depth_offset. Change the static dimension for the offset in the extrude dialog to depth_offset. Now, change the depth_offset parameter from -1 to -1.5. This changes the height of the teeth from the bottom of the part.
Change the cylinder height from 4 in to 5 in. The model updates, and the extrusion remains 1.5 in from the bottom.
Change the cylinder height to 8 in, and the same relationship remains in place.
Keep the Paper Towel Holder Ready for Different Rolls
A parametric design matters when the physical roll changes after printing. If you 3D print the holder for a standard roll and later buy an extra bulky roll, changing the diameter from a smaller size to a larger size updates the design instead of requiring a full redesign.
Adding constraints and formulas takes more work than making a one-off model, but it makes future changes much easier.
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