Creating a Solid Body from Surfaces

This article outlines the different methods you can use to create a Solid Body using Surfaces. It will outline the different requirements and output abilities based on the feature used. For full descriptions on the individual features and how to apply, we recommend utilizing the SOLIDWORKS help files.


Depending on your modeling methods, you may find yourself with a surface instead of a Solid Body. While this may show the shell of your part accurately, it will not contain mass properties or be usable for simulation. Based on the surface or surfaces you are working with, there are multiple ways to create a Solid Body.


Thicken (Insert > Boss/Bass > Thicken)

This is probably the simplest of the methods to create a solid. It only requires a single surface that does not have to be enclosed. When this option is selected, you can select what side of the surface you want thickened (or both) and a thickness. This thickness will be applied normal to the surface in the direction you choose.

If you have a fully enclosed surface body, you will have the option to "Create solid from enclosed volume."


Trim Surface (Insert > Surface > Trim)

When you have multiple surfaces that intersect to form an enclosed volume, you can use the Trim feature to create a solid. Within the trim property manager, the trim type needs to be set to "Mutual." Select all the intersecting surfaces under surfaces, then either remove the surfaces not needed to enclose the volume or keep the needed surfaces. If the resulting surface is fully enclosed surface, the option for "Create Solid" will become accessible.

We have a separate article on the enhancements made to this feature in 2016 to make previewing the kept/removed surfaces easier. Click here to view that article


Knit (Insert > Surface > Knit)

The knit feature can be used to create a solid from surfaces or faces that form an enclosed volume. The main purpose of the knit command is to combine surfaces, but when the combined surfaces create an enclosed volume, the "Create solid" option becomes available. For the knit feature to work, there must be multiple surfaces selected, if you already have a fully enclosed, singular surface body, this feature will fail and you should use the thicken command instead.


Boundary Surface/Filled Surface (Insert > Surface > Boundary Surface/Fill)

During your modeling, if the surface you are working has a gap that prevents it from creating a fully enclosed volume, using either the Boundary Surface or Filled Surface feature can fill the gap and create a solid. In both commands, the "Create solid" box under Options and Preview will become accessible if the resulting surface is fully enclosed.


Intersect (Insert > Features > Intersect)

Similar to the trim surface command, you can use the Intersect command to find internal regions and create a solid from surfaces. This command can also be used to join Surfaces to existing Solid Bodies. Select all the surfaces or solids that you want to find an intersection for, then select the "Create internal regions" option and select the Intersect button. The region list should populate with all the enclosed volume regions, and selecting the green check mark will result in the creation of a Solid Body.


Delete Face (Insert > Face > Delete)

This works very similar to the Knit/Thicken command in that it requires the surfaces to be a single entity that is enclosed or only contains minor gaps. With the enclosed surface, select a face to delete, then under options select Delete and Fill. This feature is optimal if there are small gaps preventing the surface from being fully enclosed that are difficult to fill. Instead of individually patching the surfaces, this feature will delete the face selected attempt to automatically fill the gaps and create a solid.


If you have any questions or need clarification on any of the methods described in this article, feel free to contact Hawk Ridge Systems Technical Support at


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