How to Loft in Fusion 360

By the end of this video, you’ll know how to use the loft command in Fusion 360. I’m going to cover many of the options in the Loft dialog. I’ll also be walking you through both a beginner and a more advanced loft example, with step-by-step instructions.

What is the loft feature?

A Loft creates a smooth transition between two or more profiles or faces.

There are three different loft features in Fusion 360.

Reference Image

End Conditions

The end condition controls the transition from the start and end profiles of the loft command.

There are six types of end conditions in Fusion 360. Which end condistions are available dependso n the type of geometry selected for the profile.

Takeoff Weight

Available when the end condition is set to Direction. Specifies the amount of influence the takeoff angle has along the Loft path.

Takeoff Angle

Available when the end condition is set to Direction. Specifies the start angle of the transition from the profile.

Tangency Weight

Available when the end condition is Tangent, Smooth, or Point Tangent.

Tangent Edges

Specifies whether the Loft operation merges tangent edges or not.

• Merge Merges tangent edges.
• Keep Keeps the tangent edges unmerged.

More Tutorials with Loft Examples

Transcript:

By the end of this video, you’ll know how to use the loft command in Fusion 360. I’m going to cover many of the options in the Loft dialog. I’ll also be walking you through both a beginner and a more advanced loft example, with step-by-step instructions. If you’re looking for the advanced tips and tricks then you can skip ahead by using the timestamp that I have down below in the video description.

Put simply, the loft command is like connecting the dots. Using the loft feature will join the selected profiles, resulting in a solid or surface.

To start, you should know that the loft command is available in 3 different environments.

We have the solid modeling loft command, found under the “create” dropdown of the solid tab. The surface modeling loft command, found under the “create” dropdown of the surface tab. Lastly, we have the form loft command, which is only available if you’re in the Form or sculpt environment.

At their core, all of these loft commands work similarly. Each loft feature does have some small differences that I’ll be covering near the end of this tutorial.

Let’s start with a basic loft project, where I’ll walk you through many of the options in the loft dialog.

I’m going to create a 100mm center circle on the bottom XY origin plane.

We’ll need to create the second profile on a construction plane since we don’t have any other faces or surfaces to reference.

I’m going to create an offset plane 100mm off of the XY origin plane. Once the construction plane is completed I’m going to create a center rectangle off of the offset plane. I’ll use the dimensions of 100mm in both directions.

At this point, we have the minimum requirement for creating a loft in Fusion 360.

I’m going to activate the loft command from the shortcuts box, where I’ll choose the blue solid modeling version. Notice how the Surface loft command shows up, but the Form loft command does not. The Form or t-spline loft will only show up in the shortcuts box if you’re in an active Form environment.

With the loft command active, we’ll first need to select our profiles. The first thing to know is that the order you select the profiles does matter, which we’ll take a look at in just a minute. For now, I’ll simply select both profiles.

Here we have the most basic loft, connecting a circle with a square, which is a shape that can’t be created with the revolve tool.

In the profile section of the dialog, you’ll notice a plus symbol and the letter “X”. As you’re selecting profiles you may find that you selected the wrong profile. If that is the case, simply select the profile you want to remove, and click the “X” or remove button.

If you want to add more profiles, you can hit the plus symbol or the add button and click the sketch profile that you would like to add.

The next item you should be aware of is the end condition. There are six different end conditions, with the availability depending on what type of geometry is selected.

I’ve put all 6 types and their descriptions on this tutorials resource page at ProductDesignOnline.com/22… that’s ProductDesignOnline.com/22 [two-two].

If I click on the default of “connected” you’ll see that I only have one other option, which is the direction. I’ll go ahead and look at this from the front view, so you can see what happens as I change the first profile to the direction option.

Notice how the loft goes from having a straight and efficient line to having an angled line.

The direction option applies an angle measured off of the sketch plane. This option is always available when the loft profile is a 2D sketch.

The default “connected” option simply connects the profiles in the most efficient manner, which is why we have a straight line from the circle’s edge to the edge of the rectangle.

If we don’t want this to simply be a straight line then we can also define the guide type, by defining a guide rail or a centerline.

You can also drag around the default rails that were created between each profile.

I’ll be walking you through adding custom rails with the next loft example. For now, let’s take a look at using a centerline to further define a loft.

I’m going to hit “OK,” to close the loft command.

I’ll hide the body and create a new sketch off of the XZ origin plane because this plane is perpendicular to the two profiles and directly in the middle of each profile. On this center plane, we can sketch out any sketch geometry that connects from the bottom profile to the top profile. The key takeaway is that your centerline sketch geometry must be connected to the center point of all the profiles that you’re connecting.

Because I created both profiles off of the center origin point, the center point was automatically projected. If you don’t have a center point to snap to you will need to either project one or create one with the “point” sketch feature.

I’m going to connect the profiles with the 3-point arc tool, making sure it snaps to each center point.

After finishing the sketch, I’ll drag it to before the loft feature in the timeline. I’ll double-click on the loft to edit the loft and I’ll select the “centerline” rail type. After that, we simply need to select the centerline.

Immediately after, the loft will adjust based on the centerline. As you can see, this is a very simple way to further define your loft results.

Let’s take a look at why the order of selecting the profiles matters and then I’ll walk you through an advanced loft example.

I’ll click “OK” to update the loft. I’m going to create a new offset profile off of the top face of the model. I’ll create a center circle on the construction plane and finish the sketch.

Once again, I’ll need the loft command at the end of the timeline, so I can reference the sketch I just created.

After re-editing the loft command, I’m going to clear out the centerline, as that doesn’t connect all three profiles, so we can no longer use it.

I’ll then click the “plus” symbol in the profile section and I’ll select the top circle profile. Notice how this connects all three profiles and creates a nice transition from one shape to another.

Generally, you’ll always want to create your lofts by starting at one end and then selecting the profiles in order as you work your way to the other end.

Watch what happens to this loft if I were to click the middle profile last.

You’ll see the shape folds in on itself, creating unrealistic geometry, which in many cases Fusion 360 won’t be able to solve.

In the case that you select profiles out of order, or if you decide to add profiles later on, then you can always reorder the profiles without having to reselect them.

You can either select the profile order from the dropdown list on the model or by selecting the order in the loft dialog.

Let’s now take a look at lofting a more complex object. I’ll walk you through an ergonomic handle with spots for each finger to rest.

I’m going to hide the basic loft component and I’ll create a new component for the handle.

I’ll first attach a reference image to help recreate the contour. If you’re looking to follow along, I’ve placed the reference image on this tutorials resource page at ProductDesignOnline.com/22.

I’ll attach the image to the XZ origin plane and then I’ll calibrate the image to have an approximate handle height of 125mm.

I like to start the first profile off of the bottom origin plane, so I’m going to re-edit the canvas image to adjust the position so it aligns with the bottom plane. I’m also going to center the image to the origin point.

For the first profile, I’ll create an ellipse on the XY origin plane. I’ll make the major axis 40mm and the minor axis 30mm.

One thing to understand with more advanced lofting is that you’ll often want to break the lofts into sections. I’m going to break this handle into three main sections. For the first loft, I’m going to loft from the bottom of the handle to the middle of this top curve. For the second loft, I’ll loft from the middle of the top curve to the cap of the beginning of the nozzle. Finally, for the third loft, I’ll create the large area of the nozzle.

I’m going to create an offset plane 110mm from the XY origin plane. The handle gets smaller towards the top, so I’ll create a second ellipse, making this one 35mm at the major axis and 25mm at the minor axis.

I’ll finish the sketch and we’re ready to create our guide rails.

First, I’m going to drop the opacity of the canvas down so it’s not quite as opaque, so it’s easier to trace the image.

I’ll then create a sketch from the XZ origin plane, as I want these rails to be defined in the center so the shape is symmetrical. However, it’s important to note that rails do not need to be created directly in the center as the centerlines do.

To create guide rails you can use any of the sketch geometry. The key takeaway is that you’ll always have to make sure that your guide rail touches every single profile. This point can’t be stressed enough. I often see beginners struggling to get their loft to work because the rails aren’t snapped to each profile.

For example, if you have 5 profiles it needs to touch all 5 at some point. In our case, we have only two profiles, so I’m going to use the spline command to trace the handle shape.

Starting at the bottom, I’ll make sure that it snaps to the major axis of the ellipse. If you’re creating a guide rail and having trouble getting it to snap to a profile then you have a few different options. You can project the point, create a construction line, create a sketch point where you want it to snap, or you can use a coincident constraint after the fact, to force it to stay together.

In this case, the start of the spline snapped into the major axis of the ellipse. I’m going to trace this image, placing points at all the vertices.

Once I get to the top, you’ll see that the end of the spline is not wanting to snap to the top ellipse. I’m going to simply click to place the point and then I’ll use a coincident constraint to force it to connect with the endpoint of the major axis.

Because I’m going to create a second loft on the top of this one, I’m going to also add a vertical constraint to the spline handle, so the exterior geometry ends up with a smoother connection to the next loft.

I’m going to activate the loft command so we can see how the guide rail works.

I’ll select the bottom profile as the first, and the top profile as the second.

At the moment, we have a nice straight handle with a small taper. To add our guide rail I’ll simply click the plus symbol for the rails section and I’ll select the spline geometry. Notice how the loft shape now zig-zags and follows our desired shape. However, I don’t want the back of the handle to have the same zig-zag effect, so we’ll need to create a second guide rail.

I’ll hit the “cancel” button in the loft dialog so we can create a second spline for the back. I’ll retrace the back silhouette, once again making sure that the starting and ending points of the spline snap into each profile. If not, I’ll force them to with the coincident constraint.

Once again, I’ll also add a vertical constraint to the handle of the top spline point.

I’ll reactivate the loft command, and this time I’ll select both guide rails. Notice how the contour of the handle is now further defined, with the help of rails. If we wanted to, we could continue to add rails on the sides of the profiles. In fact, we could technically add as many rails as we would like, so long as they all touch every profile in our loft.

For now, I’ll click “OK” to confirm the loft so we can look at creating the second loft to finish off the handle.

When working with the loft command, it’s a best practice to break the object into sections that could be lofted individually. This will give you more control and make it easier to create guide rails, as they won’t have to touch as many profiles.

Typically, when starting a new loft from another, you’ll want to project the surface geometry. I’m going to select the top surface and I’ll project the ellipse geometry onto the surface.

I’ll also create a construction line running across, so I have endpoints to connect the rails too.

Then, before we can create the next profile, I’m going to first create one of the guide rails. I’ll then use the guide rail to create a construction plane for the next profile.

I’m going to trace the bottom of the shape using the spline tool and the coincident constraint to force the points to snap to the first profile. I’ll also make sure there is a vertical constraint added to the first spline handle, so the geometry has a nice transition from one loft to another.

After that’s complete, I’ll create a construction plane on the end of the guide rail using the option “Plane along path”.

From that plane, I’ll then create a new sketch, where I’ll create a 2-point circle, with the first point starting from the end of the spline. I’ll make the circle 35mm in diameter. To help ensure the rail snaps into the circle I’m going to create a sketch point where the rail should connect.

Then, I’ll create another sketch on the XZ origin plane, where I’ll create the top rail, once again, making sure that the spline points snap into the ellipse and circle respectively. If not, I’ll use the coincident constraint to force them to snap together. I’ll also add a vertical constraint to the bottom spline handle.

At this point, we’re ready to use the loft tool. I’ll select both profiles, starting with the first one on the existing surface. Then, I’ll select both guide rails. Before clicking the “OK” button you’ll also want to decide if you want this second loft to create a new body, or to join the other loft body.

You’ll see that we can also create a new component, use the loft tool to cut away bodies, or the intersect option, which removes all material from the solid that does not overlap the new feature. For now, I’ll set this to “Join” and I’ll click “OK”.

Lastly, I’ll create one last offset plane off of the top surface. I’ll set the offset distance to 45mm.

I’ll first project the other circle to this sketch, ensuring that we use the same center point. I’ll then create a new center circle with a diameter of 75mm. I’ll also create two sketch points on the circle, so it’s easier to connect a guide rail.

We’ll then need to use the 3-point arc tool to define the guide rail. I’ll also use the coincident constraint to force these lines to connect.

Repeating the loft command, we can create a third loft that finishes off the overall shape of the handle and nozzle.

Looking at the model, there are a few things I would do at this point. First off, it appears that the transition from the first loft to the second loft is not completely smooth, as you can see this crease or line. This is caused by the width of the shape having different geometry near the meeting point. To fix this, we would need to define a few more guide rails for each loft, making sure they’re parallel at that meeting point.

I would also then apply fillets to the model, where the second loft and third loft are joined, further smoothing out the transition. As well as adding a fillet to the bottom edge of the handle.

To finish up this tutorial, I want to show you the differences between the surface and form loft commands.

I’ll drag the timeline marker to just before the first loft command and I’ll turn the original sketch geometry back on so I can reuse it.

This time, I’ll activate the surface loft command from the shortcuts box. Watch what happens as I recreate the loft. At a distance, everything seems to work the same. However, you’ll notice as I zoom in that this only created a surface body, which is represented by the thin gray and yellow surface. With surface lofts, the ends won’t automatically be sealed off and you’ll have to use the Patch command to do so.

Other than that, the surface loft command follows the same rules and best practices as the solid modeling loft command.

Before I show you the Form loft command, let me know which loft command you find yourself using the most by commenting “Solid” or “Surface” down below in the comments!

While you’re at it, click that thumbs up button to let me know you’re learning something new in this tutorial.

I’m going to undo the surface loft command so we can take a look at the Form loft command.

To access the form loft command, I’ll enter the form or sculpt environment.

To start the loft we’ll need to follow the same steps as the other two loft commands. Once the loft is created, this is where the form loft command becomes different.

Notice how I have all of these t-spline faces that are connected to make up the body. The difference in the form loft command is that we can define the number of faces in each direction. We can also define whether the faces should be uniform, which is the default or we can set this to the curvature option, where the number of faces adapts based on the defined curvature.

I’ll click “OK” to complete the loft. At this point, you’re left with a t-spline body that can be manipulated just like any of the other t-splines in the Form or sculpt environment.

For example, I can drag over the front of the shape to select it. I’ll edit the form and I’ll drag the planar direction icon towards the left to alter the handle’s thickness.

A few other things to note with the Form loft command is that it won’t be recorded in the timeline below, as everything is simply created under the form icon. Along with that, you’ll see the Form loft only allows one to create a new body or component, as you’re not allowed to cut or intersect from any of the form bodies.

To summarize, the loft command is available in three different formats. Solid modeling, surfacing, and sculpting. The loft command is commonly used to bridge the gap between sketch profiles. Be sure to break complex objects into multiple lofts, which will make it easier for you to avoid common loft errors.

Last but not least, I want to give a shoutout to Jim Ferguson for supporting all of the Fusion 360 content that I make!

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