Loft vs. Boundary: Which to Use When?
When SOLIDWORKS introduced the Boundary Surface feature in 2008, I was just finishing writing the first SOLIDWORKS Surfacing and Complex Shape Modeling Bible.
It was a new feature, and it was being added to the book at the last minute. I didn’t have many or good examples, and there wasn’t much of a description for why we needed this new surface type aside from, “It allows curvature continuity and treats profiles and guide curves the same.”
Both of those enhancements were certainly welcome at that time. Curvature being available in only one direction on the Loft feature really limited the quality of work you could do.
However, it turns out that the differences between the Loft and Boundary features are much more than just continuity in both directions. It also turns out that there’s not a simple answer to the question of which is better, because whether by initial design or evolution over years of enhancements, there are many differences—and it turns out they are best applied in different applications.
In this article, I’m going to go through what differentiates the Loft and the Boundary features, as well as the overlap between them. But because I know this is going to come up later, I’ll start by addressing the solids versus surfaces question now.
Solid Versus Surface
Both Loft and Boundary can be made as solids or surfaces. In my view, if you’re using one of these features as a solid feature, you’re really not getting as much out of it as you could. I have actually used a solid Boundary once—not in a real part, but instead more in the lines of tech support. I don’t think I would ever use a solid Boundary feature in a real project, because there’s just not nearly as much benefit and flexibility as when you use it in its native state: the surface.
To be honest, if I didn’t have to acknowledge the solid features, I wouldn’t. All my examples are surfaces. If you are regularly using either of these features on the solids side (especially the Boundary), you’re really missing out.
Solid lofts are much more common; still, while some of my examples will work in either solids or surfaces, I’m only demonstrating surface functions in this article. If you want to talk about solids versus surfaces, that’s a different article.
The Loft feature has been in SOLIDWORKS since at least 1997, and maybe even earlier. It is the simplest way to allow the software to interpolate a shape between two or more profiles. It works with solids and surfaces, and it has unique functions as well as some overlap with the Boundary feature. Let’s talk about what makes Loft unique.
Loft has several unique functions:
- Centerline Loft
- Closed Loop
- Add Loft Section
- Loft Interface
The Centerline Loft is one that frequently gets overlooked. It is the answer to the multi-section sweep you may find in other software. The distinguishing feature of the Centerline Loft is that you can add a centerline or spine that functions like a guide curve, except that it doesn’t need to actually touch any of the profiles. It makes this kind of feature possible:
In this example, it works like a loft in that it transitions or interpolates between two differently-shaped end profiles. But it also works like a sweep in that it follows the centerline path that doesn’t touch either profile. You can download a sample SOLIDWORKS 2020 file from this link.
As an interesting side note, the Centerline Loft appears to require 2D sketches as profiles. It doesn’t work if one of the profiles is a SelectionManager selected set of model edges.
Closed Loop Loft
This has a lot of benefits, especially when a revolve feature just won’t get you where you need to go. You can do this with the Boundary feature, but it takes two features instead of one with the Loft.
The closed loop in this case is an elliptical guide curve. To get the loft to close, use the Close Loft option in the PropertyManager, but it requires one of the boundary directions to be a closed loop. You can download this example from this link.
Add Loft Section
Add Loft Section is a very handy tool for those times when you need more control in an existing loft feature. SOLIDWORKS automatically creates a plane and a profile and adds it to the list of profiles for you. Once the profile is created, you can edit it to control the shape even more. Profiles can also be added manually, but it’s a nice touch that the software can do it for you automatically. To initiate this function, right click on a loft feature and select Add Loft Section.
The Loft Interface is to some extent easier to use than the Boundary interface. You could argue that this is because it doesn’t do as much, and you might be right about that.
The first part of the interface that’s easier is that the end tangency conditions are always showing. On the Boundary feature, you have to select the profile and then set the tangency. Boundary does enable you to set the tangency direction for any profile, while Loft only allows you to set tangency for the first and last profiles. Plus, you can use the callouts in the graphics area to set the tangency for each profile.
Loft also automatically adds connectors if you have a profile with multiple segments. However, Boundary enables you to add as many connectors as you want (in both directions).
Boundary also has several unique functions:
- Curvature continuity allowed in both directions.
- Connectors allow more control over UV flow.
- Allows the use of more “arrangements” of profiles.
- Trim By Direction.
Curvature continuity in both directions was the original selling point for the Boundary surface more than a decade ago, and this is still valid. The Loft still cannot do this.
Connectors are one of the most powerful tools you have at your disposal for fine tuning the flow of the UV mesh on your SOLIDWORKS NURBS models. Connectors are often the difference between a shape that uses all the right sketches but just looks wrong, and perfection.
For example, look at the following screenshots. The top one is unruly and twisting, while in the lower image the UV mesh flows the way it should. Situations where the preview twists like this can cause the deformed feature shown, or even cause the feature to fail.
If you didn’t know about connectors, you wouldn’t know where to look to fix a problem like this. The connectors are the pink and green dots and connecting lines that govern how the profiles connect to one another. These can be added, deleted, shown, hidden and reset from the RMB menu while editing the Boundary feature.
As a note, the UV mesh (black lines in the orange preview) can be enabled and adjusted in the Curvature Display panel of the Boundary and Loft PropertyManagers.
The Boundary feature enables you to take advantage of multiple “arrangements” of profiles. I describe these arrangements with letters. For example, an X arrangement would be two profiles that cross in the middle. An L arrangement would be two profiles that touch at the ends. An E arrangement would be 3 Dir1 profiles and 1 Dir2. Many other arrangements are possible with Boundary, like F, T and H, plus # and some arrangements we don’t have characters for.
If you look at the mesh in the image below, you could make a Boundary feature from any 2 (or more) curve elements. Profiles in different directions must touch each other, either at an end or in the middle.
The part of Boundary profile arrangements that is so different from Loft is that you can have profiles that hang-over, like an F or a T.
Trim By Dir1/2
Related to the “arrangements with hang-overs” is the Trim By Dir1/2 option in the Boundary PropertyManager. Using the image above, let’s set up another demonstration.
If we used the grid above to create a # type arrangement, we’d get something like this:
The Boundary feature enables you to trim off the hang-overs with the profiles in the opposite direction. So, if we used Trim By Dir1, we’d get this:
And if we trim by both directions, we get this:
Trimming by direction is useful when you have large profiles, but you don’t want the surface feature to follow the entire profile. If the profile is an edge and you can’t trim it, simply adding a profile and then using it to trim the feature is a great solution to that problem.
There is a lot of overlap between Loft and Boundary.
If you make all of your curves in a single 3D sketch, you can drag the curves while editing the feature. Very cool. (You’d better read that one again.)
Loft to a Point Tangency
Both Loft and Boundary enable you to loft to a point, and then apply tangency to that point, and it will be rounded off like a dome. Generally speaking, this kind of shape is better handled by a feature such as Fill due to degenerate points, but that’s a discussion for a different article.
Apply To All
Tangency weighting can be applied to all segments of a profile equally, or you can apply different values to different segments.
The mesh, Zebra Stripes and Curvature Combs can all be displayed in the preview of both Lofts and Boundary features. These can help you predict if the feature will fail, or if it will have funny little artifacts such as ripples, creases or curvature inflections.
To be clear, the Boundary is not a replacement for the Loft. We still need both of these features because each of these features has unique strengths.
However, there is a fair amount of overlap between the two, and when I have the choice, I select the Boundary feature because in the end, for me and what I do, Boundary is more flexible and ultimately more capable. The functions I need most are the curvature continuity in both directions and the connectors in both directions.
I most frequently use Loft for centerline function, and when I think I might want to use the automatic Add Loft Section capabilities.
Understanding the capabilities of each tool will help you select the appropriate feature for every area of your model without the need for trial and error.
About the Author
Matt Lombard is the author of the SOLIDWORKS Bible series (SOLIDWORKS Bible, Surfacing Bible and Administration Bible), including the latest Mastering SOLIDWORKS, as well as video courses for SolidProfessor and Infinite Skills, and the Dezignstuff blog. Matt’s latest endeavor is an online e-learning site called Dezignstuff Surfacing Episode, with theoretical and practical examples using text, images and video.
Matt’s early career got him interested in plastics design, and from there he developed an interest in CAD and complex shapes. He has been a SOLIDWORKS user since he bought the software in 1996. Since then he has worked at SOLIDWORKS resellers, as an independent consultant for 17 years and took some time to work for Solid Edge. Mr. Lombard lives in western Virginia with his wife Kim.