How to Design a Custom Bottle Holder in Autodesk Fusion for 3D Printing
Updated August 21, 2026
Designing a part around an existing product is one of the most useful skills you can learn in CAD. In this tutorial, you’ll use Autodesk Fusion (formerly Fusion 360) to create a custom bottle and then build a prototype bottle holder directly around it using a top-down, parametric workflow.
The project combines surface modeling, splines, projected geometry, mirroring, tangent planes, slots, and several practical techniques for creating geometry that can later be refined for 3D printing.
What You’ll Learn
- How to generate a bottle using a Fusion script and use it as reference geometry
- How to organize a top-down design using separate components
- How to offset a surface by 3 mm to create clearance around an existing object
- How to build linked geometry with Fit Point Splines and 10 mm offsets
- How to use Intersect, Join, and Cut operations efficiently
- How to create a 3 mm thick structure around a curved surface
- How to use Mirror and rotate geometry by 90 degrees
- How to project existing geometry into new sketches to keep the design parametric
- How to create mounting geometry on a curved part using a tangent plane
- How to create a 12.5 mm Center Point Slot with a –2.5 mm offset
- How to design cuts and extrusions that remain robust when dimensions change
- Why fillets, wall thickness, clearance, and print orientation matter when preparing a prototype for 3D printing
Watch the Workflow — or Read It Step by Step
You can follow this guide in two ways:
- Read the steps below if you want quick written instructions, reference images, and modeling notes.
- Watch the full video at the end of this post to see the workflow in real time — including extra tips, camera angles, and shortcuts that don’t fit neatly into text.
Both formats build on each other.
Reading helps you understand why each step matters, while watching shows how to move faster in Fusion.
Step 1: Generate the Bottle with a Fusion Script
Start by opening Scripts and Add-Ins and running the Bottle script. Fusion generates a fully modeled bottle inside a new component, with the scripted modeling operations appearing in the parametric timeline.
Open Scripts and Add-Ins from Fusion’s Design workspace to generate the reference bottle used throughout the project. The shortcut menu is being searched for the command rather than navigating through the full toolbar.
The bottle will become the master reference for the top-down bottle holder workflow, so generating it first establishes the geometry that later surface offsets and holder features will follow.
The Scripts and Add-Ins dialog is open with the Bottle script selected under Sample Scripts. Clicking Run creates the bottle model automatically.
Using the script is simply a fast way to establish the reference object. The resulting model remains editable in Fusion’s parametric timeline, so its sketches and features can still be revised later.
The generated bottle works as the reference object for this tutorial. Because the model is parametric, however, you can revisit its sketches or features and modify the bottle before building the holder.
After running the script, Fusion creates the bottle as a modeled component and records its features in the timeline. A sketch feature is selected here with Edit Sketch available from the context menu.
This confirms that the scripted bottle is not just imported static geometry. Earlier sketches and features remain accessible, which is useful if the bottle dimensions need to change before or after the holder is developed around it.
This is an important advantage of designing parametrically in Autodesk Fusion. Rather than treating the bottle as static reference geometry, you retain access to the design history and can test how changes propagate through the model.
The bottle’s underlying profile sketch contains dimensioned arcs and lines that define the revolved form. Visible values include an overall 210 mm vertical dimension along with radii such as R150 mm and R160 mm.
Because this geometry is part of the parametric feature history, changing the profile can update the resulting bottle without rebuilding the model from scratch. The holder created later can then inherit those changes through its reference geometry.
Step 2: Create a Separate Component for the Bottle Holder
Before modeling the holder, activate the main component and create a separate component for it.
The modeled bottle is selected while the New Component dialog is used to create a separate component named Bottle holder.
Keeping the bottle and holder in separate components is important in this top-down workflow. The bottle remains the reference product, while all new holder geometry is created independently around it. This also preserves a cleaner structure if the design is later used as an assembly.
The bottle and bottle holder should remain separate components rather than being modeled together as one object. This keeps the design organized and makes each part easier to edit within its own parametric context.
This is particularly useful when designing products made from multiple physical parts. Later, you can move, align, or use the components in an assembly without rebuilding the geometry.
The bottle will now act as the reference object around which the holder is designed.
Step 3: Offset the Bottle Surface by 3 mm
Instead of manually recreating the bottle's curvature, use a top-down design workflow.
Open the Surface Modeling workspace and use Offset to create a new surface based directly on the bottle.
Set the offset distance to:
3 mm
The Surface > Offset command is applied to the bottle with a distance of 3 mm and the operation set to New Body.
That offset creates a surface that follows the bottle accurately while introducing clearance between the physical bottle and the holder. Modeling clearance directly from the reference body is more robust than manually redrawing an approximate bottle contour.
For a 3D-printed prototype, the 3 mm gap also leaves room for real-world variation in the bottle and printed part rather than assuming a mathematically exact fit.
This surface becomes the starting geometry for the holder while providing approximately 3 mm of clearance from the bottle.
Clearance is especially important when designing parts for 3D printing. A holder modeled exactly against the nominal bottle surface could become too tight because of printer dimensional tolerances, material shrinkage, surface texture, and variation in the physical bottle.
Once the offset surface has been created, hide the original bottle component. You can bring it back later when you need to check the fit or visualize the complete assembly.
Step 4: Create the Main Holder Sketch
Use the ViewCube in the upper-right corner of the Fusion canvas to position the model at a comfortable sketching angle.
Start a new sketch on the vertical construction plane facing the model. You can press and hold the mouse wheel to pan and fine-tune your view.
The model has been repositioned to a straight-on view before starting the holder sketch. A vertical construction plane through the bottle is being selected as the sketch plane.
Sketching from a central plane makes the bottle silhouette easier to reference and keeps the upcoming holder geometry aligned with the model origin. The ViewCube can be used to establish this orthographic orientation before sketching.
Draw a regular line through the center of the model and convert it to a construction line. This geometry is only being used as a reference and should not contribute to the final profile.
A line is drawn vertically through the center of the bottle and converted to construction geometry. It serves only as a reference and therefore does not create a selectable profile for later solid operations.
Center-based reference geometry is useful here because several subsequent sketch elements are positioned relative to the bottle rather than arbitrary locations on the canvas.
Next, create another line starting from the midpoint of the construction line. Fusion should automatically snap to the midpoint.
Offset this line by:
10 mm
Repeat a similar workflow below the model: create another line and offset it so the resulting geometry remains linked to its parent geometry.
Placing these references beyond the immediate boundary of the model gives you more freedom when creating the curved profiles in the next step.
The Sketch > Offset command is being used on one of the horizontal reference lines with a distance of 10 mm.
Because the second line is created as an offset rather than drawn independently, Fusion maintains a parametric relationship between the two. That relationship becomes useful when the surrounding spline geometry is adjusted later.
The same construction is repeated below the bottle to provide controlled endpoints beyond the main body of the model.
Step 5: Shape the Holder with a Fit Point Spline
Select Fit Point Spline and sketch the approximate outer shape of the holder.
Don't try to perfect the spline immediately. Establish the general form first, then refine it by moving the spline points and manipulating the green handles.
A useful rule for spline modeling is to use as few control points as possible.
Adding more points may initially appear to give you more control, but it also makes the curve more difficult to manage. Simpler splines generally produce smoother geometry, lighter sketches, and more predictable downstream features.
This becomes particularly valuable when the final object will be 3D printed. Smooth, continuous curvature tends to produce cleaner transitions than unnecessarily complex surfaces containing small changes in direction.
You'll also get a much better sense of the shape once the sketch becomes three-dimensional, so avoid spending excessive time perfecting the initial 2D curve.
A Fit Point Spline is now being shaped alongside the bottle using the previously created 10 mm reference geometry.
The spline does not need to match the bottle surface exactly because the holder will ultimately be derived from the offset surface created earlier. At this stage, the spline primarily controls the design language and width of the structural band.
Use as few fit points as practical. Excessive spline points make curvature harder to control and introduce unnecessary complexity into downstream surfaces and solids.
Step 6: Offset the Spline by –10 mm
Once the first spline has the general shape you want, offset it by:
–10 mm
This creates a second spline linked parametrically to the original.
The Fit Point Spline is being refined by moving its control points and tangent handles. The visible angular and distance inputs illustrate how the curve can be shaped interactively after placement.
This is the stage to refine the overall character of the holder rather than trying to fully constrain every curve immediately. Since the next operations turn this 2D sketch into geometry following the bottle surface, checking the result in 3D is more informative than endlessly adjusting the initial spline.
The relationship is useful because changing the original spline's control points or handles will also update the offset geometry.
You are effectively defining the shape once and allowing Fusion to maintain the relationship between the two curves.
Close the remaining boundaries with lines so that you have valid closed sketch profiles.
You can oversketch the closing lines for speed or terminate them precisely if you prefer cleaner sketches. Either approach can produce a usable closed profile for the following solid-modeling operation.
Step 7: Extrude the Profiles and Use Intersect
Finish the sketch or press E to launch the Extrude command directly.
Select the closed profiles and extrude them far enough to extend completely through the relevant surface geometry.
It is useful to deliberately over-extrude here rather than creating an extrusion that only barely reaches the current model. If the bottle geometry changes later, the oversized extrusion has a better chance of continuing to intersect the required geometry.
Set the Extrude operation to:
Intersect
Instead of simply adding or removing material, Intersect retains only the geometry shared by the extrusion and the existing model.
This converts the sketch-driven shape into geometry that follows the curved reference surface derived from the bottle.
The closed sketch profiles are selected for Extrude, and the extrusion is extended well beyond the bottle geometry. The visible distance is 200 mm, while the operation menu is being changed to Intersect.
Intersect keeps only the volume shared by the extruded profiles and the existing reference geometry. This converts the freeform sketch into geometry that conforms to the bottle-derived surface instead of creating a simple planar extrusion.
Over-extruding is intentional. It prevents the operation from becoming dependent on a narrowly chosen distance that could stop intersecting the model after earlier dimensions are edited.
Step 8: Give the Holder a 3 mm Thickness
The resulting geometry is still too thin to function as a practical holder.
Set the thickness to:
3 mm outward from the center
You now have a more substantial structure that can form the basis of the physical prototype.
Wall thickness is an important 3D-printing consideration. Extremely thin walls may be difficult for a slicer to resolve consistently and can result in a fragile print. A 3 mm structure provides a much more useful starting point for prototyping, although the final required thickness depends on the material, print settings, layer orientation, loading conditions, and intended use.
At this stage, rotate the model and inspect it from several angles.
This is a good point to make aesthetic changes because much of the remaining geometry will depend on this initial sketch. Since the workflow is parametric, changing that sketch later should automatically update dependent features.
The curved result is converted into solid geometry with Thicken. The thickness is set to 3 mm, with One Side selected in the command.
This creates the structural section that the rest of the holder will build from. A 3 mm wall is also a practical starting point for a functional FDM prototype, giving substantially more material than a thin cosmetic shell.
The eventual strength will still depend on print material, wall count, layer orientation, and loading direction, so the CAD thickness should be treated as an initial engineering choice rather than a universal value.
Step 9: Mirror the Holder Geometry
The design is centered around the Fusion origin, which makes the default construction planes useful for symmetry operations.
Open Mirror, select the relevant geometry, and use the central construction plane as your mirror plane.
Set the Mirror operation to:
Join
This combines the mirrored geometry with the existing geometry instead of creating disconnected bodies.
Centering a product around the origin early in the workflow can save substantial time later. Default planes can then be reused for mirrors, sketches, sections, and other operations without creating unnecessary construction geometry.
The first thickened holder section is selected in Solid > Mirror, with one of Fusion’s origin planes used as the Mirror Plane.
Building the design around the origin allows the default construction planes to drive symmetrical features without creating extra reference geometry. This is one reason centering the initial model pays off as the timeline becomes more complex.
The mirror establishes the opposing holder geometry while keeping both sides geometrically consistent.
The mirrored body is previewed on the opposite side of the holder with Operation > Join selected in the Mirror dialog.
Using Join combines the mirrored geometry with the existing connected solid rather than leaving another independent body. This keeps the holder consolidated as the symmetrical structure develops.
The preview is worth checking before confirming the feature, particularly where the mirrored geometry meets the lower frame. The bodies need sufficient overlap for Fusion to complete the join reliably.
Step 10: Rotate the Joined Geometry by 90 Degrees
With the mirrored bodies joined, open Move/Copy.
Position the pivot at the center of the model and rotate the joined geometry by:
90 degrees
The completed holder section is selected with Move/Copy and rotated 90° around the Z axis. Create Copy is enabled, so the original geometry remains in place while the rotated version is added.
This reuses the existing bottle-conforming structure instead of constructing another set of splines and surface features. The copied geometry therefore retains exactly the same curvature and proportions.
Repeating geometry by rotation is particularly effective for this design because the holder wraps around the bottle from multiple directions while maintaining a consistent visual language.
You should now have the rough structure of a bottle holder surrounding the bottle with a few millimeters of clearance.
Because the holder was constructed directly from offset bottle geometry, its position and curvature are inherently related to the bottle rather than being approximated independently.
Before continuing, inspect the holder carefully. If the proportions or spline shape need adjustment, this is a good time to return to the earlier sketch in the timeline.
The bottle body is made visible again inside the assembled holder geometry to inspect the relationship between the two components.
At this stage, the earlier 3 mm surface offset can be evaluated in three dimensions rather than only from the original sketch view. The curved ribs follow the bottle form while remaining separated from its actual surface.
Temporarily toggling reference-body visibility is useful throughout a top-down modeling workflow: the bottle can remain available for fit checks without becoming part of the holder's final solid geometry.
Step 11: Project the Holder Geometry for the Rear Connection
The next task is to create geometry connecting the holder to its mounting area.
Create a sketch on the appropriate construction plane and use Project to bring key edges from the existing model into the sketch.
Start the Create Sketch command, then select the vertical construction plane running through the bottle holder. This defines the 2D plane for the next section of the model.
The plane is positioned through the existing holder geometry, which allows its edges to be referenced in the sketch. Once the sketch plane is confirmed, the next step is to use Project to transfer the required 3D edges into the sketch.
With the sketch active on the construction plane, open Project/Include > Project and select the relevant edges from the existing bottle holder. The Project dialog shows 4 selected edges.
Fusion converts these references into projected sketch geometry, visible in purple. This provides an exact connection between the existing solid model and the new profile without manually recreating its dimensions.
The projected geometry will now serve as the reference for constructing the symmetrical profile in the following steps.
Projected geometry appears as purple sketch lines in Fusion.
Draw a straight line through the center of the projected geometry and convert it into a construction line. This line will serve as the axis for another symmetrical sketch.
A 30 mm horizontal line is added from the projected geometry in the bottle holder sketch. The line provides reference geometry for positioning the angled profile that will form the next section of the frame.
Keeping this geometry in the sketch makes the location of the new frame feature controlled by dimensions rather than manually positioned.
Create one half of the closed profile on one side of the construction line.
A second line is drawn from the endpoint of the horizontal reference geometry and constrained with a 135° angular dimension.
The angular constraint defines the direction of the new bottle holder frame section while keeping its orientation parametrically controlled in the sketch.
Then use Mirror to reproduce it on the opposite side.
The Sketch > Mirror command is used to duplicate the angled line across the horizontal centerline. The original angled geometry is selected as the object and the horizontal line is selected as the Mirror Line.
This creates matching geometry on the opposite side without drawing and constraining a second line independently.
This approach reduces duplicate sketching and ensures that both sides remain symmetrical.
If oversketching leaves unwanted geometry behind, use Trim to clean it up. Alternatively, excess lines can sometimes remain if they don't interfere with profile selection or later operations.
The Trim tool is used to remove the portions of the mirrored sketch geometry that extend beyond the existing bottle holder frame.
Trimming the intersections leaves the required sketch profile connected to the existing geometry and ready for the following solid operation.
Step 12: Extrude and Join the Rear Connection
Launch Extrude and pull the new profile up to the top of the required geometry.
If you want the new feature to become part of the existing holder, set the operation to:
Join
This keeps the bottle holder as one unified solid body.
Alternatively, you could choose New Body or New Component if your design requires the feature to remain independently editable or manufacturable.
There isn't one universally correct choice. The appropriate body/component structure depends on what you intend to do with the model later.
For this prototype, combining the holder geometry into one body creates a straightforward part for subsequent modeling and eventual 3D printing.
The completed sketch profile is selected and Extrude is used to extend it across the bottle holder. The image shows a distance of 139.966 mm with Operation: Join.
Using Join incorporates the extrusion into the existing bottle holder body, creating another structural member between the surrounding frame geometry.
Step 13: Continue Building with Projected Geometry
Create another sketch and once again use Project to capture geometry from the latest part of the model.
The view is moved to the bottom of the bottle holder and an existing horizontal frame edge is selected.
This lower section of the model provides the geometric reference for constructing the next part of the bottle holder base.
Inside a new sketch, Project is used to bring existing bottle holder geometry into the active sketch. The Project dialog shows 2 selected edges.
Projected geometry creates associative references to the existing model, allowing the new base feature to be positioned from the surrounding frame rather than recreated with independent dimensions.
Expand the required lines outward and project additional geometry until you have a new closed profile.
The Line tool, accessible with the L keyboard shortcut, is used to draw vertical lines from the projected reference points.
These lines begin defining the boundaries of the new base profile between the existing bottle holder components.
The Project command is used again, this time with four edges selected from the existing lower frame geometry.
Projecting these edges completes the references needed to define the base profile directly against the surrounding bottle holder structure, maintaining alignment with the existing model.
The key principle is to reference existing geometry rather than manually recreating dimensions whenever possible.
This helps preserve design intent. If an earlier feature changes, dependent sketches have relationships that allow them to update with the model.
Extrude the resulting profile and use the back edge of the projected geometry as the reference for both the depth and length of the extrusion.
The completed base profile is selected and Extrude is applied along the bottom of the bottle holder. The visible extrusion distance is approximately 62.713 mm, with Operation: Join.
The extrusion spans the space between the existing frame members and joins the new geometry to the bottle holder body, adding another structural section to the base.
Step 14: Join the Geometry and Cut Away Excess Material
Use Extrude again to refine the rear section.
First, perform an Extrude Join to bring the relevant geometry together into a single solid.
The newly created base profile is given thickness with Extrude. The extrusion distance is set to 3 mm and Operation: Join is selected.
This turns the previously defined profile into solid base geometry and joins it to the existing bottle holder frame.
Then use Extrude Cut operations to remove unwanted material.
For the cuts, extend the cutting geometry:
All the way to the bottom of the model
Avoid defining a shallow arbitrary distance when the design intent is for the cut to pass through the entire relevant section.
This makes the feature more robust. If you later change the thickness of the holder, the cut can continue to remove the required material rather than stopping at an obsolete fixed depth.
The same principle is useful throughout parametric CAD: whenever possible, define features according to design intent rather than simply entering dimensions that happen to work for the current version.
Two profiles are selected and Extrude is used with Operation: Cut. The extrusion distance is set to −3 mm, removing material from the base.
This cut cleans up the overlapping geometry where the newly created base intersects the surrounding bottle holder structure.
Step 15: Add Fillets to Strengthen the Prototype
Add fillets to selected transitions around the holder.
A 2 mm Fillet is initially attempted on three connected edges. Fusion reports the error “mitred vertex too complex to process,” indicating that this combination of edges cannot be filleted successfully as selected.
Instead of forcing the operation, the fillets are applied more selectively in the following steps.
Fillets aren't only cosmetic. They can reduce sharp transitions and distribute stresses more gradually through the geometry.
That can be particularly useful for 3D-printed functional parts, where abrupt changes in cross-section may become weak points under load.
Fillets can also improve print quality by replacing certain harsh geometric transitions with more gradual surfaces. However, don't assume that adding fillets automatically makes a part strong.
The final strength of a printed holder will also depend on factors such as:
- Material
- Layer orientation
- Wall count
- Infill strategy
- Print temperature
- Layer adhesion
- Loading direction
- Fastener geometry
- Overall wall thickness
Treat this model as a prototype that can be tested and refined rather than assuming that the first printed version is ready for demanding real-world use.
The Fillet command is applied to a single edge at the junction between the angled support and lower frame. The radius is set to 2 mm.
Selecting the edge individually avoids the geometry conflict encountered when several connected edges were included in the previous fillet operation.
Additional longitudinal edges of the angled support are selected with the Fillet command. Two of the four edges are highlighted in the image for the operation.
These fillets soften the sharp edges of the support and create smoother transitions around the structural member.
Step 16: Create a Tangent Plane on the Curved Back
The back of the holder is curved, which means you can't simply create the next sketch on a conventional flat rear face.
Instead, create a tangent plane.
Position the construction plane so that it is tangent to the curved rear surface of the holder.
This gives you a flat sketching reference positioned exactly against the curved geometry.
Tangent planes are particularly useful in product design because many real objects don't provide convenient planar faces exactly where features such as holes, logos, clips, or mounting slots need to be added.
A new construction plane is created using Construct > Tangent Plane. The curved face of the bottle holder is selected as the reference face.
The tangent plane provides a flat sketching surface positioned against the curved frame, allowing the next feature to be designed relative to this part of the bottle holder.
Step 17: Create a 12.5 mm Center Point Slot
Create a new sketch on the tangent plane and orient the view so you're looking directly toward the center of the model.
Select the Center Point Slot tool.
A new sketch is started on the construction plane and Center Point Slot is selected from the Sketch shortcuts menu.
The slot tool creates a symmetric elongated profile from a centerline, making it suitable for defining the opening in the vertical section of the bottle holder.
Start the slot from the center, define its length, and set its width to:
12.5 mm
You can adjust the slot position by dragging it, or add dimensions and constraints if you want the sketch to be fully defined.
The exact slot size should ultimately be adapted to the mounting system you're designing around. For this tutorial, 12.5 mm provides the working example.
The Center Point Slot is positioned vertically on the bottle holder. The visible width dimension is 12.5 mm, with the slot centered along the vertical reference geometry.
Using a center-point slot keeps both sides symmetric around its centerline while the dimensions control the overall geometry.
Step 18: Offset the Slot by –2.5 mm
With the first slot complete, use Offset to create another closed profile.
Set the offset distance to:
–2.5 mm
You should now have two closed slot-shaped profiles.
This gives you an outer region that can be used to create a recessed mounting surface and an inner region that can become the actual opening through the holder.
Using an offset instead of manually drawing the second slot keeps the two profiles geometrically related.
The slot is dimensioned to 110 mm in length, then Offset is applied to its perimeter. The Offset dialog shows a distance of −2.5 mm with Chain Selection enabled.
This creates a second slot-shaped profile inside the original geometry with a consistent 2.5 mm offset around the perimeter.
Step 19: Extrude the Outer Slot Profile –2 mm
Select the outer slot profile and extrude it:
–2 mm
This creates the first level of the mounting feature.
When creating recessed features on a 3D-printed part, consider how they will be oriented on the print bed. Deep horizontal recesses can introduce overhangs that require support material.
Whenever possible, orient or shape mounting features so that the printer can build them progressively from the previous layers. Reducing unnecessary support generally means less material, shorter print times, cleaner surfaces, and less post-processing.
The slot-shaped profile is selected and Extrude is set to Cut. The extrusion distance is −2 mm.
This removes material from the vertical bottle holder section according to the slot geometry, beginning the recessed opening while retaining the surrounding frame.
Step 20: Cut the Inner Slot Completely Through the Holder
Next, select the inner slot profile and extrude it through the model using a Cut operation.
If you can't select the sketch, Fusion may have automatically hidden it after the previous extrusion. Turn sketch visibility back on in the Browser.
Because the back of the holder is curved, targeting a specific terminating face can make the feature unnecessarily fragile.
Instead, over-extrude the slot so the cut passes completely through the holder.
This creates a more robust parametric feature. If the thickness of the holder changes later, the cut is less likely to fail or leave unwanted material behind.
For features that are intended to pass completely through a 3D-printed object, this type of modeling logic is often preferable to relying on a fixed numerical cut depth.
A second Extrude Cut is applied to the slot geometry and extended farther into the model. The dialog shows a distance of −21.069 mm.
This deeper cut removes the remaining material behind the slot profile, producing the opening through the relevant section of the bottle holder.
Step 21: Inspect and Adjust the Remaining Wall Thickness
Before finishing the model, use Inspect to check the remaining thickness around the mounting feature.
In this example, the measured distance is:
Just over 1 mm
That's a useful warning that the geometry deserves another look.
The Measure tool is used to check the minimum distance between two selected edges after creating the slot feature.
Fusion reports a minimum distance of 1.065 mm. This measurement is used to evaluate the remaining clearance between the new feature and the adjacent bottle holder geometry.
Rather than adding another extrusion to compensate for the issue, go back in the parametric timeline and edit the original extrusion.
This is generally a cleaner CAD workflow.
Adding corrective features every time something needs adjusting can create a long and difficult-to-understand timeline. Editing the feature that actually controls the geometry keeps the model easier to maintain.
The measurement is also particularly relevant for 3D printing. A wall just over 1 mm may be printable depending on nozzle size and slicer settings, but printability is not the same as adequate mechanical strength.
If this holder will experience real loads, evaluate the mounting area based on your printer, material, perimeter count, layer orientation, and expected forces.
An existing extrusion is adjusted to fine-tune the geometry after checking the clearance. The Extrude dialog shows a 1 mm distance with Operation: Join.
This small dimensional adjustment increases the material in the affected area and refines the spacing between neighboring bottle holder features.
Step 22: Review the Component Structure
At this point, most of the bottle holder geometry has been created using Join operations.
The result is one bottle-holder body contained inside its own component, while the bottle remains a separate component.
This is a useful structure if you later want to create an assembly, reposition the bottle, evaluate fit, or develop additional components around the design.
It also keeps the manufacturing logic clear: the bottle is your reference product, while the holder is the part you are actually developing.
Step 23: Add Appearances and Evaluate the Finished Design
With the functional geometry complete, add appearances to make the design easier to evaluate visually.
For example, apply a glossy red appearance to the holder to create contrast against the green bottle.
The Appearance panel is opened to change the visual finish of the completed bottle holder. The library is searched for glossy red, with several red metal, paint, and plastic appearances available.
A red appearance is applied to the model, providing a clearer visualization of the finished bottle holder without changing its physical geometry.
Changing appearances doesn't affect the physical CAD geometry, but it can make proportions and surface transitions easier to understand. It's also useful if you want to create renders, thumbnails, portfolio images, or product-development visuals before committing to a physical print.
This is also a good time to turn the bottle component back on and inspect the complete assembly from multiple angles.
Check the clearance, mounting area, wall thickness, transitions, and overall proportions.
Step 24: Prepare the Bottle Holder for 3D Printing
Before exporting the finished prototype, think about how the holder will actually be manufactured.
The CAD model is only one part of designing successfully for additive manufacturing.
Consider print orientation first. The strongest orientation isn't necessarily the orientation that looks most obvious in the slicer. FDM prints are anisotropic, meaning they generally behave differently along the layer lines than across them. Try to avoid orienting highly loaded mounting features so that forces simply pull layers apart.
Also inspect the holder for steep overhangs. Geometry that can be built progressively upward is usually preferable to horizontal features that require extensive support. The curved structure and fillets used in this design can help create smoother transitions, but the final orientation still matters.
Finally, check wall thickness and clearance. The holder begins from a surface offset 3 mm from the bottle and uses a 3 mm structural thickness, but the mounting feature creates locally thinner areas. As the Inspect step demonstrated, some geometry can end up only just over 1 mm thick.
Treat your first print as a functional prototype.
Test the bottle fit, mounting geometry, flexibility, and strength. Then return to the Fusion timeline and adjust the features that control those characteristics. That's where a parametric workflow becomes particularly powerful: you can iterate on the design instead of rebuilding it.
Key Takeaways
This project demonstrates how a relatively complex product can be built from a small number of repeatable Fusion techniques.
The 3 mm surface offset establishes clearance directly from the bottle geometry, while the 10 mm and –10 mm sketch offsets create linked geometry that can be adjusted parametrically. A 3 mm thickness turns the surface-driven form into a more practical structural prototype.
Mirroring around the origin, rotating geometry 90 degrees, and repeatedly projecting existing edges allow later features to remain connected to the original design intent rather than being positioned independently.
At the rear, a tangent plane provides a clean way to sketch against curved geometry. The 12.5 mm Center Point Slot, –2.5 mm slot offset, and –2 mm outer-profile extrusion demonstrate how mounting geometry can be constructed without requiring a flat surface on the original part.
Most importantly, the workflow is designed around iteration. Instead of treating the first model as finished, use Fusion's parametric timeline to test clearances, wall thicknesses, mounting geometry, and print orientation—and then modify the features that actually control them.
That approach is useful far beyond this bottle holder. The same top-down modeling principles can be applied to brackets, cases, mounts, clips, enclosures, tool holders, and other custom 3D-printed products designed around existing objects.
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Chapters
00:09 How to Use Scripts and Add-Ins in Fusion
00:26 Editing Features with the Timeline in Fusion
00:44 Create and Activate a New Component in Fusion
00:58 Offset a Solid Body to Create a Surface Model
01:32 Start a New Sketch in Fusion
01:47 Add a Construction Line in Sketch Mode
02:08 Offset Sketch Lines in Fusion
02:32 Create Curves Using Fit Point Splines
02:50 Edit Fit Point Splines for Precision
03:35 Create Closed Sketch Profiles for Extrude
04:05 Extrude Closed Sketch Profiles in Fusion
04:26 Use Extrude Intersect for Complex Shapes
04:43 Thicken a Surface Body to Create a Solid
05:08 Mirror a Body in Fusion
05:29 Mirror and Join Solid Bodies Together
05:39 Copy and Rotate Bodies in Fusion
06:20 Sketch the Back of a Bottle Holder
06:31 Project Sketch Geometry to Maintain Design Links
07:00 Mirror Sketch Geometry in Fusion
07:18 Trim Sketch Lines for Clean Profiles
07:29 Extrude a Projected Sketch Profile
08:07 Project a Solid Body into a Sketch
09:17 Use Extrude Cut to Remove Material
09:32 Add Fillets to Smooth Edges in Fusion
10:07 Why You Can’t Sketch on a Curved Surface
10:26 How to Sketch on a Tangent Plane
10:43 Create a Center Point Slot Sketch
11:06 Move a Sketch Without Using the Move Tool
11:38 Extrude Cut the Center Point Slot
12:03 Fix Selection Issues When Extruding Bodies
12:41 Inspect Wall Thickness in Fusion
13:10 Project Summary and Design Review
13:26 Apply a Glossy Appearance to Your Model
13:55 More Fusion Tutorials from The Maker Letters