Loft Tool in Fusion 360: Model a Complex Glass Bottle (Day 4)

Kevin Kennedy: Your fourth challenge in Fusion starts right now: modeling this complex glass bottle. I’m Kevin Kennedy, and this is Day 4 of Learn Fusion in 30 Days.

Today, we’re mastering the Loft tool, along with offset construction planes, Intersecting geometry, and more. Let’s get started!

Start with a new Part Design file and save your design. The Loft tool allows you to connect two or more closed sketch profiles. We’ll loft between four closed sketch profiles to recreate the example bottle.

We’ll also add guide rails to further define the shape. Let’s sketch each of the four profiles. Activate Create Sketch and select the XY origin plane to start

with the bottom of the bottle. Press ‘R’ on the keyboard to activate Rectangle. In the Sketch Palette, switch to the Center Rectangle tool.

Click the origin point to start the rectangle. Using the Center Rectangle instead of a 2-point rectangle keeps the bottle symmetrical to the center axis.

This simplifies mirroring the sketch later. Type 63mm for the width and 76mm for the length. Remember, you can press the Tab key to toggle between the dimension inputs.

Click to place the rectangle. In the first three days, we used modeling fillets to round over sharp edges. Today, we’ll use Sketch Fillets from the sketch toolbar to round

the corners of our rectangle. Select each side of the rectangle and repeat this for all four corners. Notice how the Fillet command rounds the sharp corner edges.

This single input controls all four corners. Define the fillet radius as 7mm and press Enter. Note that Sketch Fillets are not ideal; the warning icon indicates they have

removed some existing sketch constraints. Follow the best practice in Fusion by choosing Modeling Fillets over Sketch Fillets when possible.

However, Lofts and Sweeps represent two common use cases where sketch fillets remain necessary for many desired shapes. Adding these rounded edges to the sketch profiles ensures the Loft tool

generates a smooth, continuous surface. The first profile is now complete. Select Finish Sketch.

Fusion requires you to start all sketches on an origin plane, a flat planar surface, or a construction plane; it does not allow sketches to float in space. The Construct menu offers many types of construction planes.

Each one leverages different types of geometry. Offset construction planes are the most common, as they simply require an existing sketch or planar face to offset from.

Let’s view the model from the Home position. Activate Offset Plane and select the bottom origin plane or the previous sketch.

Define the specified distance to offset the plane from your selection. Type 114mm and click OK. Here’s a pro tip: construction planes in Fusion are technically infinite.

The orange graphic defaults to a small square, but you can click and drag the corners to enlarge it. This helps you visualize how the plane intersects your model.

Click in space to deselect the construction plane. Our second profile is also a rectangle, so press “R” for Rectangle. Select the new offset construction plane to sketch on.

Activating a sketch command provides another way to create a new sketch. Once again, use the Center Rectangle option from the Sketch Palette and start from the origin point.

This profile requires a width of 76mm and a length of 95mm. Click to place the rectangle. Add 12mm sketch fillets to each corner.

Ensure you activate the Sketch Fillet tool rather than the Solid Modeling fillet tool. Two of the four sketch profiles are now complete.

Let’s create two more offset construction planes to quickly sketch the circle profiles for the stem of the bottle. Activate Offset Plane from the Solid tab and select the previous sketch.

Define the offset as 38mm. Choose your offset object carefully. If this object changes, the distance of the additional

offset plane will change as well. Typically, you should offset from the origin plane since it never changes, or offset from an object that you don’t anticipate changing.

For this practice project, either method works fine. Press Spacebar to repeat the Offset plane. Select the previous plane and define the offset as 89mm.

Press Enter or click OK in the dialog. We can now sketch two different-sized circles for the stem of the bottle. Press C to activate the Circle tool.

Select the lower construction plane. Remember, our Browser lists all construction planes. Hide the topmost plane so it does not obstruct the sketch.

Start the circle at the origin point and define the diameter as 40mm. Click to place the circle. View the sketch from the Home view to verify you are

sketching on the correct plane. Let’s also finish the sketch. Again, press “C” for Circle.

Although you previously hid the topmost construction plane, you can still select it in the Browser when prompted to select a plane to sketch on—even while it remains hidden.

Start from the center origin and define a diameter of 30mm to taper the stem of the bottle. Click to place the circle and select Finish Sketch.

Review the four sketch profiles. The light blue shading indicates each profile is fully closed, meeting the requirement for the Solid Loft tool.

On Day #2, we created a glass soda bottle using the Revolve tool. This more complex bottle shape requires the Loft tool because the shape lacks symmetry in all four directions.

Activate the Loft command from the Solid tab. Note that Loft also exists in Surface and T-spline modeling; ensure you activate the blue Solid Modeling Loft.

Once active, we can select our sketch profiles. This is very important! Loft requires you to select the profiles in the order you

want them to be connected. Start at the bottom and select each profile in order, working up to the top. Observe the results as you select them.

Fusion joins the sketch profiles to create a 3-dimensional body. Looking at the bottle from the Front view, you can see the shape automatically slopes as it connects each profile.

This does not create the desired final shape, so we must refine the geometry. First, change the ‘Connected’ option to ‘Direction’. This automatically applies an angle based on the sketch plane.

This looks much closer to our target shape; however, we can still define the Loft with more intention. We can add guide rails or a centerline to improve the shape.

Rails consist of 2D or 3D sketches that influence the loft shape between profiles. You can add any number of rails to the loft, but they must touch every profile in the Loft.

In this case, your rail must touch all four sketch profiles. The other option is to use a Centerline. However, only one centerline can be used at any given time.

Cancel the loft in the dialog so we can sketch our guide rails. A quick heads up, you can now get a bundle of all the written instructional guides. Link in the video description.

Observe that the final bottle shape is symmetrical from the centerline. This means we must create the same guide rail on each side of the bottle. We’ll sketch one first, then mirror it to the other side.

Select Create Sketch and choose the XZ origin plane, as it runs directly through the middle of the sketch profiles. You can create guide rails with any sketch geometry.

Recreate this bottle shape using a regular line at the top and a Spline at the bottom to create the curves. Pay close attention here, this is very important.

A Loft guide rail must touch every profile in your loft. Since we have four profiles, the rail must touch all four. Otherwise, you will encounter a common Loft error stating, “the guide rail

isn’t touching all sketch profiles.” To ensure the guide rail snaps to each edge of the four sketch profiles, use the Intersect command to reference existing geometry.

Find Intersect in the Create menu of the Sketch tab, within the Project/Include flyout folder. Once active, view the model from the Home position.

Imagine the current sketch plane slicing all four profiles in half. Hover over the sketch lines until a red dot appears. This dot represents the area where the sketch plane

intersects the existing geometry. By selecting this geometry to intersect, you create points on your active sketch plane exactly where the existing sketch passes through it.

This allows you to guarantee that your guide rails connect to the four profiles. Select each of the four sketch profiles. The circles automatically intersect on both sides; however, you only need the

left side of the rectangles since you will mirror the sketch geometry later. In the Intersect dialog, ensure the Projection link option is checked by default.

This ensures the intersected geometry updates automatically if you change any dimensions of the four sketch profiles. Click OK and notice that the color purple indicates the intersected geometry.

You now have four points to snap to as you create the guide rails. Select Look At in the Sketch Palette to view the sketch directly. Activate the Line tool and draw a straight line to connect the top two points.

This represents the straight stem of the bottle. Notice how the line snaps to the intersected points. If you clear the Line command and select an endpoint, you will find

that Fusion automatically added a Coincident constraint, forcing the line to remain connected to each sketch point from the Intersect command. Activate the Fit Point Spline command.

Start from the bottom point and select the next two points in order. Remember, as we discussed on Day 2, you must press the Enter key or select the checkmark icon to complete the spline.

The second most important requirement for a Loft guide rail is that Fusion requires guide rails to be continuous. This means your spline and line must have a smooth transition between them.

Press ESC to clear the Spline tool. Click and drag the topmost spline handle and release it where it snaps to the straight line.

This ensures the spline transitions smoothly into the line, creating a single continuous guide rail. We can now adjust the spline handles to improve the overall shape.

Select the middle spline point. Click and drag the handle to adjust the curve until you are happy with the bottle's shape.

Remember, you can edit the sketch to update this at any time—a major benefit of parametric modeling in Autodesk Fusion. You may also want to adjust the bottom spline handle.

The left guide rail is now complete. To create the right one, use the Sketch Mirror command. Activate Mirror from the Sketch tab.

Ensure you activate the sketch mirror rather than the solid mirror. Select the straight line and the spline. On Day 2, we created a centerline down the middle of the bottle.

Alternatively, you can reference the vertical axis instead of creating a new centerline. Since the origin never moves, select the Mirror line selector, followed

by the Z-axis in the Origin folder. Click OK to mirror the sketch. The mirrored geometry appears on the right and automatically

applies the Symmetry constraint. This allows you to adjust your geometry while the opposite side updates automatically.

Activate Loft from the Solid Modeling tab and view the model from the Home position. Select the four sketch profiles in order, as previously discussed. Select the plus sign to add a new guide rail.

Before selecting the rails, ensure ‘Chain Selection’ is checked by default. As with the paperclip example, use chain selection to include all touching sketch objects.

You can now select the two guide rails. The guide rails greatly improve the Loft. You will often find rails necessary for creating complex shapes.

Let me know if you encounter a loft error. Verify that your spline and line connect correctly to each of the four sketch profiles.

If those connections are secure, ensure the spline snaps to the straight line to form a single continuous path. Click OK, and let’s finish the bottle by adding a few more

details before hollowing it out. The bottom of the bottle is completely flat. Activate the Modeling Fillet command and select the bottom edge.

Add a 5mm fillet to round over the sharp bottom edge. Apply this fillet before hollowing out the body, just as you did with the glass bottle on Day 2, so the Shell command follows this outer contour.

Let’s create a stem at the top to add a thread. Press “C” for the Circle tool and select the top planar face. Start at the center origin and define the diameter as 27mm.

Press “E” for Extrude and select the new circle profile. Extrude this 12mm. Before clicking “OK,” ensure you set the operation to “Join.” You

must join this 3D body to the existing one so the Shell command can trace a single, continuous shape. Activate Shell from the toolbar.

Select the top planar surface of the bottle. This removes the top opening as you define the bottle’s thickness as 2mm. If the Shell command triggers an error, edit the guide rails sketch

and adjust the spline curvature. The Shell command cannot apply the defined thickness if the curvature is too sharp. Let’s add one last Modeling Fillet to the top sharp edge.

Define the fillet radius as 2mm. Add a thread to the top of the bottle using Fusion’s Thread command, located in the Solid toolbar.

Start by selecting the cylinder as the face for the thread. Be sure to check the “Modeled” option to create a physical thread in the model. If you leave this unchecked, Fusion represents the threads with an

image, and they will not appear if you 3D print or export the file. Uncheck the ‘Full Length’ option to drag the directional arrows and change the thread’s length.

Define the thread by leveraging various international thread standards. Experiment with different thread types and adjust the length to suit your design. Great job completing this complex bottle!

Save your progress, and I’ll see you on Day 5, where I’ll share a secret trick for the Shell command.