If you ask a room full of SOLIDWORKS users how often they use surface Modelling, many will admit they rarely — or never — touch the Surface toolbar. That’s understandable. The majority of mechanical parts can be created using familiar solid modelling features such as Extrude, Revolve, Sweep and Loft.
For everyday engineering work, solid modelling is often all you need.
Eventually, however, most designers encounter geometry that refuses to cooperate. Perhaps you’re working with imported data that contains missing faces. Maybe you’re trying to create a smooth transition between complex shapes, or you’re designing a consumer product with flowing curves. These are situations where surface modelling can transform a frustrating task into a manageable workflow.
The good news is that surface modelling isn’t a completely different way of thinking. Most of the tools resemble their solid counterparts, and many of the techniques you’re already familiar with still apply. The biggest difference is simply that you’re creating geometry without thickness.
In this article, we’ll introduce the basic concepts behind surface modelling, explore the most commonly used surface features and demonstrate how surfaces fit naturally into a traditional SOLIDWORKS workflow.
Understanding the Difference Between Solids and Surfaces
Before opening the Surface toolbar, it’s worth understanding what makes a surface different from a solid body.
A solid body represents a completely enclosed volume. It has mass, can be assigned material properties and can be used directly for manufacturing or simulation. Every face joins together to create a watertight model.
A surface body, on the other hand, is nothing more than the “skin” of a model. It has no thickness, no enclosed volume, and therefore no physical mass. Think of it as a sheet of paper floating in space. It has shape, but no depth.
This distinction often confuses new users because surface features look very similar to solid features. In many cases, they even begin with the same sketches. The difference lies in the result: instead of creating material, you’re creating geometry that can later be trimmed, extended, combined or eventually converted into a solid.
Once you begin thinking of surfaces as construction geometry rather than finished parts, their purpose becomes much clearer.
Surface bodies appear in their own folder within the FeatureManager. Unlike solid bodies, a single part can easily contain many independent surface bodies that are later combined using Knit Surface.
Why Use Surface Modelling?
If solid modelling works so well, why learn another set of tools?
One of the biggest advantages of surfaces is flexibility. Because surfaces don’t need to form a closed volume, they can be manipulated in ways that would be impossible with solid bodies.
One common example is imported geometry. Models received from customers or suppliers occasionally contain missing or damaged faces.
Rather than recreating the entire model, you can often replace the missing areas using surface tools before converting the body back into a solid.
Surface modelling also excels at creating smooth transitions. While Loft features work well in many situations, more complex shapes often benefit from Boundary Surfaces or Filled Surfaces that provide greater control over tangency and curvature.
Industrial designers frequently rely on surface tools when creating ergonomic handles, plastic housings or consumer products with flowing organic shapes. Even in traditional mechanical design, surfaces can simplify difficult modelling tasks that would otherwise require numerous solid features.
A useful rule of thumb is that Lofted Surfaces are often faster to create, while Boundary Surfaces provide greater control when surface quality is important.
Perhaps most importantly, experienced SOLIDWORKS users rarely think in terms of solid modelling versus surface modelling. Instead, they combine both techniques, using each where it offers the greatest advantage.
Exploring the Surface Toolbar
Before exploring the tools, it’s worth enabling the Surfaces tab in the CommandManager. While not strictly required, it provides quick access to the commands discussed in this article.
Right click on the command manager and select Tabs.
Then select Surfaces.
If you prefer, you can select the Toolbar in the command manager and select the “Surfaces” toolbar.
The Surface Tab contains more than a dozen commands. Rather than exploring every option in detail, this article focuses on the tools you’re most likely to use when getting started with surface modelling.
Creating Surface Geometry
Most surface models begin with one or more individual surfaces. If you’ve worked with SOLIDWORKS solid features, you’ll notice that many of the surface tools look familiar. In fact, several of them have direct counterparts in the Features toolbar. The key difference is that instead of creating a solid body, they create an infinitely thin surface that can later be modified, combined or converted into a solid.
You’ll probably notice that every one of these tools has a solid counterpart. That’s intentional. If you’re already comfortable creating Extrudes, Sweeps, Lofts and Revolves, learning their surface equivalents is much easier than you might expect.
Extruded Surface
Extruded Surface works almost exactly like Extruded Boss/Base. You select a sketch, specify the extrusion distance and create geometry.
The important difference is that no material is added. Instead, SOLIDWORKS creates an infinitely thin surface extending from the sketch.
Because the workflow feels familiar, Extruded Surface is often an excellent first step into surface modelling.
Revolved Surface
Revolved Surface follows the same principle as Revolve. Instead of revolving a profile to create a solid, it creates a revolved surface around an axis.
These surfaces are often used as reference geometry or as part of more advanced surfacing workflows.
Swept Surface
Swept Surface follows the same principle as Sweep. Instead of sweeping a profile to create a solid, it creates a surface along the selected path.
Swept Surfaces are often used to define complex shapes that will later be combined with other surfaces or converted into solids using Knit Surface or Thicken.
Lofted Surface
Lofted Surface follows the same principle as Loft. Instead of creating a solid body between two or more profiles, it creates a surface connecting the selected sketches.
Lofted Surfaces are ideal for creating smooth transitions between multiple cross sections. For many designs, a Lofted Surface is the quickest way to define the overall shape before refining it with additional surface features or converting it into a solid body.
Boundary Surface
Boundary Surface is similar to Lofted Surface, but offers greater control over how the surface behaves in two directions. This makes it the preferred choice when surface quality and curvature continuity are critical, such as in consumer products or industrial design.
Filled Surface
Filled Surface creates a new surface inside a closed boundary of existing edges.
This makes it particularly valuable when repairing imported models or filling gaps left after trimming operations.
Freeform
Freeform differs slightly from the other tools in this group. Rather than creating a new surface from sketches or profiles, it allows you to manipulate existing faces by dragging control points, much like shaping a piece of clay.
This makes Freeform particularly useful for adding subtle ergonomic or aesthetic changes to a model without rebuilding the underlying geometry. While it isn’t typically the first tool you’ll reach for when learning surface modelling, it can be a powerful way to refine complex shapes.
Surface Utilities
Not every surface tool is used to create complex freeform geometry. Some commands are designed to generate simple reference surfaces, prepare geometry for downstream operations or support specialized workflows. While they may not be used in every model, they’re valuable tools to have in your surface modelling toolbox.
Planar Surface
Planar Surface creates a flat surface from a closed sketch or a closed loop of edges.
Although it’s one of the simplest surface features, it is frequently used to close openings, repair imported geometry, or create reference surfaces before knitting multiple surfaces together.
Offset Surface
Offset Surface creates a copy of one or more faces at a specified distance from the original geometry.
Offset Surfaces are commonly used to create reference geometry, define wall thickness or prepare surfaces for mold and tooling design.
You can also use offset surface to create a copy of an existing surface by setting the distance to “0.” Note that the command name changes to “Copy Surface.”
Ruled Surface
Ruled Surface creates a surface by extending one or more selected edges. Several different methods are available, depending on how the new surface should relate to the existing geometry:
- Tangent to Surface – Extends the surface while maintaining tangency to the adjacent face, creating a smooth transition.
- Normal to Surface – Extends the surface perpendicular to the selected face.
- Tapered to Vector – Creates a ruled surface at a specified draft angle relative to a selected direction or vector, making it useful for mold and tooling design.
- Perpendicular to Vector – Creates a surface that remains perpendicular to the selected vector along the entire edge.
- Sweep – Extends the selected edge by sweeping it along a specified direction, providing additional control over the resulting surface.
The different options make Ruled Surface a versatile tool for everything from simple surface extensions to creating parting surfaces and draft geometry for manufacturing.
Surface Flatten
Surface Flatten unfolds a copy of the surface into a flat pattern while preserving its shape as accurately as possible.
This tool is primarily intended for manufacturing applications involving materials such as fabric, leather or sheet-like composites.
Note: Because of its specialized nature, Surface Flatten is only included with SOLIDWORKS Premium.
Fillet
Surface Fillet creates a smooth transition between two intersecting surfaces without requiring a solid body.
Surface fillets are often applied before the model is converted into a solid, allowing you to maintain smooth, continuous geometry throughout the surface modelling process.
Editing and Combining Surfaces
After creating and modifying your surfaces, the final step is to edit, repair, and combine them into a complete model. These tools allow you to remove unwanted geometry, extend surfaces, repair imported models, and ultimately convert multiple surfaces into a single body.
Delete Face
Delete Face removes one or more faces from a solid or surface body.
When working with imported geometry, this tool is often the quickest way to remove damaged or unwanted faces before repairing the model with new surfaces. It is also the quickest way to convert a solid model to a surface model if need be.
Replace Face
Replace Face replaces one or more faces with another selected surface.
Rather than rebuilding features, this command allows existing geometry to conform to a new surface, making it particularly useful when editing imported models.
Delete Hole
Delete Hole automatically identifies and removes simple holes from imported geometry.
It is primarily intended as a model simplification and repair tool, helping prepare imported parts for modification or simulation.
Extend Surface
Extend Surface lengthens one or more edges while maintaining the mathematical definition of the original surface.
Extending surfaces before trimming is often easier than trying to create perfectly matching geometry from scratch.
Trim Surface
Trim Surface removes unwanted portions of one or more surfaces using intersecting geometry, planes or sketches as trimming tools.
It is one of the most frequently used surface commands and an essential part of almost every surface modelling workflow.
Untrim Surface
Untrim Surface restores areas that were previously trimmed away.
This can be extremely useful when repairing imported geometry or when a trimmed surface needs to be extended back to its original boundaries.
Knit Surface
Knit Surface combines multiple touching surfaces into a single surface body.
If the knitted surfaces form a completely enclosed volume, SOLIDWORKS can automatically create a solid body during the Knit operation. This makes Knit Surface one of the most important commands in the entire Surface toolbar, as it often represents the final step before continuing with traditional solid modelling.
Thicken
Thicken adds material to a surface body by applying a specified thickness to one or both sides of the selected surfaces.
This is one of the most common ways to turn a finished surface model into a manufacturable solid part while preserving the carefully created shape.
Thickened Cut
Thickened Cut removes material by thickening a surface and using it as the cutting tool.
It provides a simple way to create cuts from complex surface geometry without first converting the surface into a solid body.
Cut With Surface
Cut With Surface uses a surface to split or remove material from a solid body.
Because the cutting tool is an infinitely thin surface, this command is especially useful when trimming solids with complex geometry that would be difficult to create using traditional solid features.
Bringing Everything Together
A common misconception is that surface models remain surfaces forever. The reality is that many workflows begin with surfaces because they’re easier to manipulate, then end as traditional solid bodies.
Imagine creating a streamlined cover.
You might begin by creating several surface features to define the overall shape. Next, Trim Surface removes unwanted areas while Boundary Surface creates smooth transitions between sections. Once every opening has been closed, Knit Surface joins everything into a single body.
If the geometry forms a watertight volume, SOLIDWORKS can create a solid directly from the Knit feature. Alternatively, if the design represents a thin-walled component, the Thicken command can add material by assigning thickness to the finished surface body.
From that point forward, the model behaves like any other solid part. You can add fillets, holes, patterns and all the other familiar SOLIDWORKS features.
A Simple Exercise
If you’re completely new to surface modelling, don’t begin with an advanced consumer product or an automotive body panel. Instead, try a simple exercise.
First, create a sketched circle.
Next, use extrude surface to create a cylinder.
Use the “Planar surface” to close off both ends of the cylinder by selecting edges.
As you will see, you currently have three Surface bodies.
Finally, use the “Knit Surface” command, select all three surface bodies (1) and enable “Create Solid” (2). This can only be done if the whole model is enclosed and watertight.
And congratulations, you have now converted your first surface model to a solid.
To convert it back to a Surface model, simply use the “Delete Face” command to delete one of the ends of the cylinder
This short exercise introduces the fundamental workflow you’ll use repeatedly as your surface modelling skills grow.
Tips for New Surface Modelers
Like any modelling technique, surface modelling becomes easier with practice. A few habits can make the learning process smoother:
- Don’t think of surfaces as finished parts. Think of them as construction geometry.
- Keep an eye on the Surface Bodies folder in the FeatureManager to understand how many separate bodies exist.
- Use Knit Surface frequently to verify that adjacent surfaces connect correctly.
- Zoom in and inspect gaps carefully — very small openings can prevent a model from becoming a solid.
- Hide solid bodies while editing complex surfaces to make the geometry easier to understand.
- Don’t be afraid to combine surface and solid features in the same model. In many cases, that’s exactly how experienced users work.
Conclusion
Surface Modelling has a reputation for being one of the more advanced areas of SOLIDWORKS, but the basic concepts are surprisingly approachable. At its core, surface Modelling simply gives you another way to create and manipulate geometry before turning it into a finished part.
You don’t need to replace your existing solid modelling workflow. Instead, think of surface tools as an extension of your toolbox — one that becomes invaluable when working with imported geometry, creating smooth transitions or tackling shapes that are difficult to produce using solid features alone.
By becoming comfortable with just a handful of commands such as Extruded Surface, Boundary Surface, Trim Surface, Filled Surface and Knit Surface, you’ll be prepared to solve a wider range of design challenges and build a strong foundation for more advanced surfacing techniques in future projects.