Design a Honeycomb Soap Mold in Autodesk Fusion for 3D Printing and Silicone Casting
Updated October 12, 2026
A custom silicone soap mold starts with the shape you want to cast—and a practical way to make it. In this tutorial, we’ll use Autodesk Fusion (formerly Fusion 360) to design a honeycomb soap bar, build a two-part 3D-printed casting assembly, and prepare the parts in PrusaSlicer.
What You’ll Learn
- Model a soap bar with a recessed honeycomb pattern.
- Use construction geometry and symmetric patterns to control your design.
- Create a silicone mold cavity with the Combine command.
- Build a casting assembly using surface offsets and thickening.
- Add alignment pins and clearance for 3D-printed parts.
- Plan print orientation to reduce the need for supports.
- Export the parts and prepare them in PrusaSlicer.
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: Create the Soap Component
Create a new component named Soap and make sure it is active before modeling.
In Fusion’s New Component dialog, name the internal component Soap and leave Activate selected. Subsequent sketches and features will then be created inside this component.
Keeping the master in its own component lets you hide it independently when inspecting the silicone cavity and include it selectively in the final mesh export.
Start with a centered rectangle and build the soap symmetrically around the origin:
- Width: 60 mm
- Length: 85 mm
- Height: 25 mm
Use Center Rectangle with its center coincident to the sketch origin, then dimension the footprint to 85 × 60 mm. The diagonal construction lines identify the rectangle’s center without dividing its extrusion profile.
This layout keeps opposite edges equally spaced from the origin planes. Later mirrored tooling features can reference those planes directly.
Extrude the rectangle to create the soap body.
Centering the model gives you useful reference planes for later operations. When it is time to mirror the alignment pins, you can use Fusion’s origin planes instead of creating additional construction geometry.
This body represents the finished soap shape. A printed version will also serve as the master used to form the cavity in the silicone.
Extrude the closed rectangular profile by 25 mm to establish the soap’s thickness. Keep this initial solid inside the active Soap component so its sketch and extrusion remain grouped.
The broad planar face provides the reference for the honeycomb sketch. The recesses and edge treatments are added afterward as separate features, leaving the base dimensions easy to edit.
Step 2: Sketch the First Honeycomb Cell
Create a sketch on the bottom face of the soap.
Choose Circumscribed Polygon and create a six-sided polygon. Set the distance from the polygon’s center to a flat side to 5 mm.
Sketch the first cell with Circumscribed Polygon, using six sides and a 5 mm center-to-flat dimension. This defines the hexagon’s size before the pattern is generated.
Place the cell at the origin so the repeated sketch can grow symmetrically across the soap face. Its orientation determines the directions needed for the staggered honeycomb layout.
That produces a hexagon measuring 10 mm across its flats. The distinction matters: a center-to-corner measurement of 5 mm would create a smaller cell.
Add two construction lines to define the honeycomb pattern directions. Use the midpoint of a polygon side as a reference; the demonstrated layout includes a direction line at 30°.
These lines guide the pattern without becoming part of the profiles you extrude.
Add construction lines from the cell center to establish the pattern axes. Use the polygon’s side midpoint to orient the angled reference, including the 30° direction shown in the workflow.
Construction geometry controls placement without creating extra closed regions. This keeps the later honeycomb profile selection separate from the reference lines.
Step 3: Pattern the Honeycomb Across the Soap
Use Rectangular Pattern inside the sketch:
- Select the hexagon geometry as the objects to pattern.
- Use the construction lines to define the two directions.
- Set the distribution to Spacing.
- Enter 12 mm spacing in each direction.
- Enable Symmetric distribution.
- Increase the quantities until the pattern covers the soap face.
With a hexagon measuring 10 mm across its flats, the 12 mm spacing leaves 2 mm between adjacent parallel sides along the pattern directions.
The pattern preview shows quantities of 10 and 12. Use enough instances to cover the face, including the area near its edges.
In Sketch Rectangular Pattern, select the hexagon edges and use the construction lines for the two directions. The displayed setup uses Spacing, 12 mm in both directions, and Symmetric distribution, with quantities of 10 and 12.
The preview extends beyond the soap outline. This extra coverage supplies cells near the perimeter; the smaller border rectangle will determine which parts of the patterned sketch are cut into the solid.
Step 4: Define the Border and Cut the Pattern
Create a centered rectangle measuring:
Open Sketch Shortcuts with S and search for Center Rectangle. Draw the border from the same origin used for the soap and honeycomb cell.
Switch off construction mode for this rectangle. Its edges must divide the patterned sketch into selectable regions so the cut can stop at the intended border.
- Width: 54 mm
- Length: 79 mm
Dimension the inner rectangle to 79 × 54 mm. Relative to the 85 × 60 mm soap footprint, the centered boundary reserves 3 mm on each side.
Cells intersecting this rectangle create partial profiles at its edges. Select only the regions inside the boundary when making the recesses, preserving the continuous outer rim.
Turn off Construction before drawing it so the rectangle creates normal sketch profiles.
Compared with the 60 × 85 mm soap outline, this leaves a nominal 3 mm border on each side. Use the rectangle to limit the honeycomb detail to the central area of the face.
Fully constrain the rectangle. With Fusion’s default sketch colors, constrained geometry changes from blue to black.
Finish the sketch, select the honeycomb profiles within the boundary, and make an Extrude Cut 2 mm into the soap body. Check the preview to confirm the cut points into the solid.
The recessed pattern in the master produces raised details inside the silicone mold. Casting soap in that mold reproduces the recessed pattern on the finished bar.
Finish the sketch and select the patterned regions bounded by the inner rectangle. Use Extrude with the Cut operation and a depth of 2 mm into the soap.
Inspect the colored preview before confirming: the chosen regions determine which portions become recessed and which remain at the original face level. The surrounding sketch cells are references only and should not extend the cut beyond the border.
Step 5: Chamfer the Soap Edges
Orbit the model and add chamfers to soften the sharp edges.
Keep the edge groups in separate timeline features:
- One chamfer feature for the bottom edges.
- Another chamfer feature for the side edges.
This makes it easier to adjust one group without changing the other. No chamfer dimensions are specified in the video script, so choose values that preserve the border and honeycomb detail.
For the finished soap, softened edges should make the bar more comfortable to handle. For the printed master, edge treatments also affect the overhangs your printer must reproduce.
A chamfer can provide a more gradual printable transition than some rounded undersides, but its benefit depends on the final print orientation. Check the sliced preview before assuming an edge treatment is support-free.
Select the outer edges around the patterned underside and apply Chamfer. The bevel forms a transition between the side walls and the patterned face while leaving the honeycomb detail inside its border.
Keep this operation as its own timeline feature. The underside bevel can then be adjusted independently of the vertical corner treatment in the next step.
Apply a second Chamfer feature to the soap’s side edges. Orbiting the body exposes the corners and makes the intersection between the side bevels and the perimeter bevel easier to inspect.
Keep enough material around the patterned face so the chamfers do not break through the border. These finished master surfaces will define the corresponding surfaces of the cast soap.
Step 6: Model the Silicone Mold Blank
Activate the top-level component, then create a new component named Silicone Mold.
Return to the root of the design and create Silicone Mold as a new internal component. Activate it before adding the enclosing geometry.
This component represents the volume that will eventually be cast in silicone. Keeping it separate from the Soap component lets Combine subtract the master while preserving both parts for the tooling workflow.
Creating it from the top level keeps it alongside the Soap component in the Browser.
Create a sketch on top of the soap and use Project to capture its outline. Keep the projection linked so dimensional changes can propagate through the design.
Start a sketch on the soap’s flat face and use Project to bring its perimeter into the Silicone Mold sketch. Leave Projection Link checked to reference the existing shape.
The projected outline includes the clipped corners created by the chamfers. Offsetting that outline follows the actual master perimeter instead of replacing it with a simple rectangle.
Offset the projected outline outward by 10 mm.
This establishes the intended silicone wall allowance around the soap. It is a starting point for this prototype; reducing it may save silicone, but the mold still needs enough stiffness to hold its shape during casting.
Use Sketch Offset (O) on the projected perimeter. With Chain Selection enabled, a 10 mm outward offset follows the complete connected outline, including its chamfered corners.
The resulting outer profile defines the silicone blank’s footprint. Check that the preview surrounds the master on every side before finishing the sketch.
Extrude the outline so it fully encloses the soap and extends beyond its underside to form a silicone floor. The image shows an extrusion distance of −40 mm from the sketch plane.
At this stage, the silicone blank intentionally overlaps the soap body.
Extrude the full area inside the offset perimeter to form a solid blank. The displayed distance is −40 mm, directing the extrusion down from the sketch plane around the soap master.
Include both the center and the surrounding band so the result is an enclosing volume, not just a hollow wall. Combine will remove the master’s shape from this blank in the next operation.
Step 7: Cut the Soap Cavity
Use Combine with these settings:
- Target Body: Silicone Mold
- Tool Body: Soap
- Operation: Cut
- Keep Tools: Enabled
If the soap is difficult to select through the enclosing body, press and hold the left mouse button to access the selection list.
Confirm the operation, then hide the Soap component to inspect the cavity.
Keeping the tool body is essential because the soap master is needed again when building and exporting the casting assembly.
You now have the digital model of the silicone mold. The next steps create the printed tooling used to cast it.
Set Silicone Mold as the target body and Soap as the tool body in Combine, choose Cut, and enable Keep Tools. The overlapping master supplies both the cavity outline and the inverse honeycomb detail.
Target and tool order matters: the retained result must be the silicone volume surrounding the soap. Keeping the Soap body makes it available for the later printed master assembly.
Step 8: Create the Mold Base from Offset Surfaces
Save the project.
Activate the top level and create a component named Mold Base.
Hide Soap to reveal the cavity and its honeycomb floor, then create Mold Base from the top level of the design. The finished silicone geometry now becomes the reference for the rigid casting container.
This reverses the design task: the next part must enclose the outside of the silicone volume while leaving its upper opening accessible.
In the Surface tools, use Offset to copy the silicone mold faces needed to form the base. Set the offset distance to 0 mm.
With Mold Base active, use Surface Offset on the exterior side and bottom faces of the silicone model. Enter 0 mm to copy their exact positions into surface geometry.
Leave the top opening out of the selection. The copied surfaces define the contact boundary between the silicone and its printed container; wall material will be added outside that boundary.
A zero-distance offset creates a surface copy without moving it. Hide the source component to inspect the result.
Use Thicken and enter 10 mm to turn the copied surfaces into the solid mold base. Check the direction carefully: the material should extend away from the space reserved for the silicone.
Select the copied surfaces in Thicken and add 10 mm on the outward side. The preview should preserve the interior boundary while creating a solid floor and surrounding walls.
Hide the Silicone Mold component while selecting the surface copy to avoid choosing the original solid faces. After thickening, show it again to check that the two volumes meet without consuming the casting space.
Turn the Silicone Mold component back on to check the fit. Confirm that the casting space remains open and accessible.
The 10 mm thickness is the prototype value used here. Thinner walls could reduce print time and material use, provided the base remains rigid and holds the liquid silicone.
Step 9: Build the Mold Top
Create another top-level component named Mold Top.
Create Mold Top as another component under the root of the design. This will contain the support geometry that locates the soap master above the base.
Separating the top from the base allows each printed piece to be exported and oriented independently. Keep the existing tooling visible as reference while establishing the support positions.
This part holds the soap master in position relative to the mold base while the silicone is cast. The prototype uses a simple locating arrangement without screws.
Sketch the support geometry over the soap and extrude it to a thickness of 5 mm.
Begin the support sketch with Mold Top active. Use S to find Center Rectangle and reference the design origin while viewing the mold from above.
The base outline provides a visual guide for the support span. The sketch can extend beyond the required footprint because the ends will be fitted to the base with later solid features.
Dimension the long support rectangle to 150 mm, as shown, and keep its center at the origin. The sketch extends beyond both sides of the base to provide material for the subsequent fitting operations.
This central strip establishes the first support direction. Its profile will become a 5 mm thick solid before the second support is copied and rotated.
Extrude the support profile by 5 mm as a body in Mold Top. The bar bridges the master and extends across the surrounding base rim.
Keeping the initial bar as a simple solid makes it easy to copy and rotate. Its overhanging ends remain available for trimming to the final tooling footprint.
Create a copy of the support part and rotate the copy 90°, as shown in the Move/Copy preview. Use additional extrusions to adapt the ends to the mold base.
Use Move/Copy with Create Copy to duplicate the support body about the central axis. The displayed preview uses a 90° rotation, placing the second bar perpendicular to the first.
The crossing bars provide support in both directions while leaving the surrounding quadrants open. Those openings preserve access to the silicone casting space around the master.
The initial sketch can extend beyond the final boundaries, then be refined with solid modeling operations. Check that the resulting assembly still leaves access for pouring silicone.
Use Extrude (E) on the support’s end face with the Cut operation to shorten the bar. The displayed adjustment is −12.5 mm, bringing the protruding end back toward the mold base.
Fit the support ends before positioning the locating pins. This establishes the final bearing areas on the base rim and avoids placing pins in material that will later be removed.
Step 10: Add the Alignment Pins
Sketch a circle with a 5 mm diameter and dimension its position relative to the edge of the mold top.
Use Center Diameter Circle to draw a 5 mm pin profile near the end of the support. Keep it within the area where the support overlaps the base rim.
The pin and its eventual hole will be derived from the same solid geometry. Establish the circle’s diameter first, then constrain its center relative to the support edge.
Position the pin where there is enough surrounding material, and extend it into the mold base far enough to locate the top.
Dimension the circle center 5 mm from the support’s end edge while retaining its 5 mm diameter. The center lies on the support’s central axis.
This leaves a nominal 2.5 mm of material between the circular profile and the end edge. Referencing the edge gives the pin a defined location before it is extruded and mirrored.
Extrude the circle using New Body.
Fusion may suggest Cut because the extrusion intersects another body. Override that suggestion: you need the pin body first, then you will use it to create the matching hole.
Extrude the circular profile downward by 15 mm, using the negative direction shown. Set Operation to New Body so the pin exists as a separate solid within Mold Top.
Its overlap with the base is intentional at this stage. The separate pin body will act as a cutting tool for the matching socket, rather than removing material during this initial extrusion.
Mirror the pin using the appropriate origin plane. Repeat the process to create four alignment pins in total.
Use Mirror with the pin body selected and the origin plane that bisects this support. The preview places a matching pin at the opposite end of the bar.
Mirror the body rather than redrawing a second circle. Both ends then share the same pin geometry and remain symmetric about the centered assembly.
The centered design makes the origin planes useful here. Mirrored pins stay related to the original geometry, reducing the need to reposition them manually after edits.
Create the pin profile on the perpendicular support using the same 5 mm diameter and 5 mm center-to-end dimension. Reference this bar’s own end edge so the pin lies over its seating area.
The rectangular base has different spans in the two directions. Defining this second pair from its support avoids assuming that rotating the first pair would place all four pins correctly.
Extrude the second pin profile downward by 15 mm as a New Body. Hiding the base exposes the pin ends and makes their direction easier to compare.
Match the first pair’s projection beneath the support. Consistent pin engagement helps the top seat evenly when all four locating features enter the base.
Mirror the new pin across the origin plane that bisects the second support. This completes the four-pin arrangement, with one locating feature at each support end.
Check the body selection before confirming so only the intended pin is duplicated. The two perpendicular mirror operations now define the locating layout for the base sockets.
Step 11: Cut the Matching Holes and Add Clearance
Use Combine to create the holes in the mold base:
- Target Body: Mold Base
- Tool Bodies: The four alignment pins
- Operation: Cut
- Keep Tools: Enabled
Use Combine Cut with Mold Base as the target and all four pin bodies as tools. Enable Keep Tools so the locating pins remain part of the top assembly.
This transfers the pin positions directly into the base without recreating their sketches. The first holes match the pin geometry exactly; the next feature supplies the clearance needed for assembly.
Hide the Mold Top component to inspect the holes.
A hole cut directly from its matching pin has no designed clearance. Printed parts generally need some allowance to fit together.
Use Offset Face on the cylindrical hole walls and enlarge the holes by 0.5 mm radially. Check the preview to make sure the holes grow rather than shrink.
Hide the top and select the cylindrical socket walls with Offset Face. The demonstrated −0.5 mm offset removes material around the holes, increasing their radius by 0.5 mm.
This changes a nominal 5 mm hole to 6 mm diameter while leaving the pins unchanged. Verify the preview’s direction: the fit allowance belongs in the sockets, and the selected faces should move away from their axes.
For a cylindrical hole, a 0.5 mm outward wall offset increases its diameter by 1 mm. A hole cut from a 5 mm pin therefore becomes nominally 6 mm in diameter.
This is the clearance used in the demonstrated prototype, not a universal fit setting. If you want a closer fit, print a small pin-and-hole test before committing to the full assembly.
Step 12: Prepare the Soap and Mold Top for Upside-Down Printing
The soap master and mold top will be printed together, upside down.
This places the honeycomb detail facing upward during printing and uses the opposite side as the bed-facing surface.
To create a flat printing surface:
- Project the soap geometry into a sketch.
- Select the required profile.
- Extrude using Join to fill out the intended flat surface.
Project the soap face into a new sketch to capture the outline needed for the flat printing surface. Projection Link preserves the reference to the master’s perimeter.
The projected profile supplies the boundary for filling the space between the supports. This prepares the combined master and top for an inverted orientation on the printer bed.
The goal is a stable contact area on the build plate and a geometry that can print without supports in the demonstrated orientation.
Check that the soap master, supports, and alignment pins form the intended connected printed assembly. Exporting several bodies in one STL does not automatically join bodies that are separated by a gap.
Extrude the projected profile by 5 mm and change the suggested operation from Cut to Join. This adds material up to the support level instead of removing it from the master.
The resulting continuous flat surface becomes the bed-contact face when the assembly is flipped. Confirm that the added volume joins the intended master and supports while leaving the silicone casting space outside the master clear.
Step 13: Inspect the Casting Assembly with Section Analysis
Use Section Analysis to inspect how the parts fit together.
Check that:
- The soap master is positioned correctly inside the base.
- Space remains around and beneath it for the silicone walls and floor.
- The alignment pins engage their matching holes.
- The mold top leaves accessible openings for pouring.
- The intended printed solids do not occupy the silicone casting space.
Toggle component visibility while the section remains active to inspect individual interfaces.
The manufacturing sequence is:
- Print the mold base and the combined soap-master/top assembly.
- Assemble them to define the silicone casting space.
- Cast the silicone around the soap master.
- Remove the printed tooling after the silicone has cured.
- Use the flexible silicone mold to cast soap.
Follow the silicone manufacturer’s instructions for mixing, compatibility, release agents, and curing. Those details are not covered by this CAD workflow.
Use Inspect > Section Analysis and move the cutting plane through the assembly. The hatched sections distinguish the master and outer base so the intervening silicone volume can be checked.
Toggle component visibility in the Browser while the analysis remains active. Inspect the space beneath the honeycomb face as well as the side walls; this confirms that the master is suspended above the container floor.
Step 14: Export the Printed Parts as STL Files
The project uses two export workflows.
For the mold base:
- Right-click Mold Base in the Browser.
- Choose Save as Mesh.
- Select STL.
- Save the file.
For the soap master and mold top together:
- Save the Fusion project.
- Show the Soap and Mold Top components.
- Hide the other components.
- Use the design-level Export workflow demonstrated in the video.
- Select STL and save.
Import both files into the slicer and verify their contents. The second file should contain the soap master, top supports, and pins, without the silicone body or mold base.
Also check the dimensions after import. STL does not store explicit unit information, so confirm that the soap still measures 60 × 85 × 25 mm before slicing.
Right-click Mold Base and choose Save as Mesh. The displayed export uses STL (Binary), millimeter units, and One File to create a separate mesh of the container.
Only the base is selected for this export. Export the master and top assembly separately so PrusaSlicer can orient the two printed pieces independently and exclude the digital silicone volume.
Step 15: Slice the Mold Base in PrusaSlicer
Import the mold base into PrusaSlicer. In the demonstrated workflow, it arrives in the intended print orientation.
Use File > Import > Import STL/3MF/STEP/OBJ/AMF to load the mold-base mesh. The visible setup has 15% infill, Supports set to None, and an Original Prusa i3 MK3S & MK3S+ printer profile.
The selected print preset is labeled 0.30 mm DRAFT @MK3 with ironing. Check the imported base orientation and inspect the sliced wall and floor paths before exporting G-code; the tutorial reports a 6-hour-44-minute estimate for this part.
The settings used include:
- Infill: 15%
- Ironing: Enabled
- Printer: Original Prusa i3 MK3S+
- Estimated print time: 6 hours 44 minutes
The prototype did not leak silicone with this setup. However, infill percentage alone does not determine whether a print holds liquid. Perimeters, solid layers, extrusion quality, and gaps between printed paths also matter.
Inspect the sliced walls and floor before printing. The screenshot shows a 0.30 mm DRAFT @MK3 preset with ironing. A filament type, perimeter count, and solid-layer count are not specified here, so confirm those settings in your own printer profile.
Ironing can smooth exposed horizontal top surfaces, but it adds print time and does not smooth vertical walls.
Step 16: Slice the Combined Soap Master and Mold Top
Import the second STL and flip the assembly upside down so the prepared flat surface rests on the build plate.
Import the combined master and top mesh, then orient it with the prepared flat face on the build plate and the honeycomb detail upward. The selected object includes the protruding support ends and locating pins.
Use the layer preview to check how those features begin and connect to the rest of the print. The visible setup keeps supports disabled; verify the actual sliced paths before relying on that choice for the full assembly.
Use the ironing preset for this part as well.
Surface finish matters because texture on the printed master can transfer into the silicone and then into the finished soap. Ironing can reduce visible lines on suitable top surfaces, although it will not remove every printed texture.
Review the layer preview before generating G-code:
- Confirm that the assembly sits flat on the bed.
- Check that all intended connected parts actually meet.
- Look for unsupported sections around the supports and pins.
- Inspect the honeycomb recesses to ensure the detail is preserved.
The model is designed around a support-free orientation, but the sliced preview is the final check for your printer and settings.
Seat the printed master and top assembly in the base using the alignment pins. The cross supports rest on the rim, positioning the master above the floor and leaving room around it for silicone.
The prototype is held with an external clamp rather than built-in screws. Apply only enough pressure to keep the top seated; the support contact surfaces establish the master’s position within the casting container.
The released soap bar reproduces the honeycomb pattern from the printed master. The flexible blue silicone mold remains available for subsequent casts after the rigid printed tooling has been removed.
Fine texture is also visible on the cast surface. Both the intended geometry and the master’s surface finish can pass through the silicone, so finishing the printed master affects more than the sharpness of the honeycomb outline.
Key Takeaways
- Model the finished object first. The soap body becomes both the reference for the silicone cavity and the printed casting master.
- Use symmetry early. A centered model simplifies patterns, mirrored pins, and later changes.
- Keep related geometry linked. Projections, surface copies, and Combine operations help the tooling follow the original design.
- Allow for printed fits. This prototype uses 5 mm pins and a 0.5 mm radial enlargement of their matching holes.
- Plan orientation before export. A flat bed-facing surface and upward-facing honeycomb detail make the master easier to print.
- Treat the settings as prototype results. The 10 mm base thickness and 15% infill worked in this example; other printers and materials may need adjustments.
- Surface texture carries through the process. Improving the printed master’s finish can improve the silicone mold and the soap it produces.
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Want to build on the modeling techniques used in this honeycomb silicone soap mold project? Explore a soap holder with a removable tray, an industrial-style pen holder, and a dedicated honeycomb pattern guide to develop your Fusion skills for practical 3D-printed designs.
These tutorials extend the progression from a digital model to a useful printed object. Practice fitting separate parts with the soap holder, explore another product with the pen holder, and refine the honeycomb geometry you can reuse in future molds and 3D-printing projects.
Step-by-step guide to follow along in Fusion
00:10 Start Your Fusion Project with a New Component
00:33 Build a Center-Based Sketch for Symmetrical Design
01:02 Create a Honeycomb Pattern in Fusion (Perfect for Soap or Mold Designs)
02:48 Extrude the Honeycomb Pattern into a Solid Model in Fusion
03:39 Add Chamfers and Fillets for a More Refined Mold Design
04:09 Design the Silicone Mold Geometry in Fusion
04:30 Reuse Existing Sketch Lines Efficiently in Fusion
05:19 Use the Combine Command to Cut Away Parts in Fusion
05:45 Design the 3D Printed Mold That Will Cast the Silicone Mold
06:13 Offset Faces in Fusion to Prepare for Mold Wall Thickness
06:39 Thicken Surfaces to Convert Your Mold Design into a Solid Body
07:15 Model the Top Part of the 3D Printed Mold for Silicone Casting
08:05 Copy and Rotate Bodies to Complete Your Mold Assembly
08:18 Shorten a Body Using the Extrude Command in Fusion
09:21 Mirror Bodies in Fusion for a Symmetrical 3D Printed Mold
10:35 Cut Holes and Adjust Clearances for FDM 3D Printing Tolerances
11:37 Fine-Tune Your Mold Design for Successful 3D Printing
12:32 Inspect the Mold with Section Analysis in Fusion
13:09 Export Your Design: Best Practices for STL and Mesh Files in Fusion
13:58 Slice Your 3D Printed Mold in PrusaSlicer — Setup and Tips
Follow the honeycomb soap mold workflow in Fusion using sketch patterns, Combine Cut, surface offsets, and Thicken to build the casting assembly. See how alignment-pin clearances, STL export, and PrusaSlicer preparation connect the design to 3D printing and silicone casting.