Home » How To Convert Surface To a Solid in SolidWorks?

Surface Modeling is an alternative to Solid-Body Modeling. Surface modeling is an advanced and powerful design method, which allows for the generation of complex geometries and parts. It is an important modeling technique because it not only makes modeling easier, it sometimes makes modeling possible. There are geometries that are impossible to create without using surface features. It is an essential tool if you want to create smooth and organic shapes for components. But a Surface Body is a zero-thickness geometry. Hence, a surface model can’t be used for 3D printing.

A Surface Body can either be closed (i.e. enclosing a volume) or open. So, today we are going to show how you can convert an open as well as a closed surface into a solid body so you can 3D print it. There are a total of 5 ways to do so:

Knit Surface


The main purpose of the Knit Surface tool is to combine multiple adjacent surfaces into a single surface. But it is the most commonly used feature for converting a closed surface body into a solid body. You can find the Knit Surface command in the Surfaces Toolbar or go to Insert -> Surface -> Knit.

The Knit Surface command requires two or more adjacent and non-intersecting surfaces to work.

In the Knit Surface Property Manager, select all the surfaces that you want to convert into solid. Select the Create Solid checkbox to use the selected surfaces to form a solid.

Note: Make sure that these surfaces form a closed volume. If there are some gaps between these Surfaces use Gap Control to fill in those gaps.

Click Ok and you will be presented with a solid body instead of your surfaces.


This feature allows you to add thickness to a surface and hence creating a solid body from that surface. Useful if your surfaces do not form a closed volume. Select Thicken command present in the Surfaces Toolbar.

Now, select the surface that you want to thicken and enter the value of thickness. You have the option to change the direction of thickness. Click Ok and you will have a solid body which is the thickened version of your surface body.

Thicken can work in the same way as the Knit command shown above if Create solid from enclosed volume is checked.

Note: Thicken command only works with a single surface. If you want to thicken multiple surfaces, knit them together first.

Filled Surface

This feature allows you to fill a gap or hole in your surface body. Additionally, it can also be used to create a solid body. Initialize the tool from Insert -> Surface ->Fill or select Filled Surface present in the Surfaces Toolbar.

Under Patch Boundary, select the boundary which you want to close. Curvature Control defines the type of control you want to exert on the patch you are creating:

  • Contact creates a surface within the selected boundary.
  • Tangent creates a surface within the selected boundary while maintaining the tangency of the patch edges.
  • Curvature creates a surface that matches the curvature of the selected surface across the boundary edge with the adjacent surface.

Now select the checkbox for Create Solid. You may need to check Merge Result for the Create Solid option to activate.

Click Ok and your surfaces will now be converted into a solid.

Boundary Surface

To create a solid body with enclosed surfaces, the Boundary Surface feature is similar in usage to the Filled Surface feature that we discussed above. This feature itself is very similar to the Loft tool but it lets you create surfaces that can be tangent or curvature continuous in all directions. In most cases, this delivers a higher quality result than both the Loft and Surface Fill tools.

To create a Boundary Surface feature, click Boundary Surface present in the Surface toolbar or go to Insert Surface Boundary Surface.

In Direction 1 and Direction 2 select your sketch curves, faces, or edges to connect. Boundary features are created based on the order of curve selection. The two directions are interchangeable and give the same results regardless of whether you select the curves as Direction 1 or Direction 2. Apply Tangency/Curvature if needed and select the Create Solid under the Options and Preview menu.

Click Ok and the Boundary surface feature will now create the patch surface and also turn your surface body into a solid body.

Trim Surface

The Trim Surface feature is used to trim intersecting surfaces from two or more surfaces. Select Trim Surface available in the Surfaces Toolbar or go to Insert -> Surface -> Trim.

To create a solid body, you must select Mutual under Trim Type in Property Manager. Under Selections, select all the surfaces that will represent the final solid body. With Keep Selections selected, select faces that form the enclosed volume of your solid. If your selected surfaces form a closed volume, then the Create Solid button becomes visible and you can select it.

Click the Green Checkmark and you will have your solid body.