How To Convert a Surface to a Solid in SOLIDWORKS?
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Surface modeling is an alternative (and often a complement) to solid-body modeling in SOLIDWORKS. It’s an advanced, powerful design approach that helps you build smooth, organic, and highly controlled geometry—especially when standard solid features struggle with complex curvature or awkward transitions.
The key limitation is that a surface body has zero thickness. It can represent shape, but it does not inherently represent volume. For manufacturing workflows like 3D printing, you typically need a closed, “watertight” solid (or at least a watertight mesh derived from a solid), so the slicer can correctly interpret inside vs. outside and generate toolpaths.
Open vs. Closed Surfaces (and Why 3D Printing Cares)
A surface body can be:
- Open (it has boundary edges and does not enclose a volume)
- Closed (its surfaces fully enclose a volume)
Most 3D-print preparation workflows expect geometry that is manifold / watertight—meaning there are no unintended holes and the “skin” of the part cleanly defines an interior. If your model has gaps, overlaps, self-intersections, or other non-manifold situations, slicers can misinterpret the part (missing walls, weird fills, holes, or outright import errors).
Before You Convert: Quick Pre-Checks That Save Time
- Check for gaps/open edges: If your conversion option is greyed out, you almost always have an opening, overlap, or surfaces that don’t meet within tolerance.
- Run geometry checks: The Evaluate > Check tools are helpful for finding invalid faces/edges and tiny gaps that prevent solids from forming.
- If the model is imported (STEP/IGES): try Import Diagnostics first. It can repair faces and knit them into closed bodies, and can help turn closed surface bodies into solids.
5 Ways to Convert a Surface Body to a Solid Body in SOLIDWORKS
Below are five practical methods to convert either closed or open surface bodies into solid bodies. In many real projects, you’ll mix these tools: patch holes (Fill/Boundary), trim excess (Trim), then knit everything into a watertight volume (Knit), or add thickness (Thicken) when the model is intentionally open.
Knit Surface
The primary purpose of Knit Surface is to combine multiple adjacent surfaces into a single, continuous surface body. However, it’s also one of the most common ways to convert a closed surface set into a solid. 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, non-intersecting surfaces. If your “surface body” is already a single enclosed surface, Knit may not be the right first step—Thicken is often the better option in that case.
In the Knit Surface PropertyManager, select all the surfaces you want to combine. If those surfaces fully enclose a volume, SOLIDWORKS will let you generate a solid by enabling the option often labeled Create Solid or Try to form solid (wording varies by version). Enable it to convert the enclosed surface volume into a solid body.
Note: Make sure the selected surfaces form a closed volume. If there are small gaps, use Gap Control to identify and (when appropriate) close gaps within tolerance. If gaps are larger than tolerance, you’ll need to repair/patch geometry before a solid can be formed.
Click OK. If everything is watertight and non-intersecting, you’ll end up with a solid body instead of separate surface bodies.
Best for: Converting already-closed surface “shells” into solids, and merging many surfaces into a single body.
Common pitfall: “Create solid / Try to form solid” stays unavailable because the surface set is not truly closed (gaps, overlaps, or missing patches).
Thicken
Thicken adds thickness to a surface, so it becomes a solid body. It’s especially useful when your surfaces are open by design (for example, a single skin that needs a wall thickness). Select Thicken in the Surfaces toolbar.
Select the surface to thicken, enter the thickness value, and choose the direction (one-side, other-side, or mid-plane—depending on your version and settings). Click OK to create a solid body that represents the thickened version of the surface.
Thicken can also convert an enclosed surface into a solid without adding wall thickness if the option Create solid from enclosed volume is available and checked (this usually appears when you select one fully enclosed surface body).
Note: Thicken typically works on a single surface body selection. If you have multiple surfaces, knit them into one surface body first, then thicken.
Best for: Turning an open “skin” into a printable wall, or converting one enclosed surface body to a solid using “enclosed volume.”
Common pitfall: Thicken can fail on tight curvature if the thickness exceeds local radius of curvature (offsetting would self-intersect).
Filled Surface
Filled Surface creates a patch surface bounded by an edge loop (a gap or hole). It’s often used to close openings in a surface body so the overall model can become watertight. It can also be used to create a solid when the fill completes the final opening of an enclosed volume. Start it from Insert > Surface > Fill or choose Filled Surface in the Surfaces toolbar.
Under Patch Boundary, select the boundary edges you want to close. Curvature Control defines how the patch behaves relative to surrounding surfaces:
- Contact creates a surface within the selected boundary.
- Tangent creates a surface within the selected boundary while maintaining tangency along the patch edges.
- Curvature creates a smoother surface by matching curvature across the boundary edge with adjacent faces.
Enable Create Solid if available. In many cases, you must also enable Merge Result for the Create Solid option to activate, because SOLIDWORKS needs to merge the patch with surrounding surfaces to create a closed volume.
Click OK. If the Filled Surface completes a fully enclosed volume and merges properly, your surfaces will convert into a solid body.
Best for: Closing irregular holes/openings with a controlled patch (especially when you want tangent or curvature continuity).
Common pitfall: If the boundary isn’t clean (tiny gaps, non-manifold loops, overlapping edges), the patch may fail or won’t merge into a solid.
Boundary Surface
Boundary Surface is similar in intent to Filled Surface (patching/creating surfaces), but provides strong control over continuity in two directions. It is conceptually similar to a lofted surface, but it can often deliver higher-quality, smoother results because it supports tangency/curvature continuity in both directions—making it a go-to tool for Class-A-ish transitions and “pretty” surfaces.
To create a Boundary Surface, click Boundary Surface on the Surfaces toolbar, or go to Insert > Surface > Boundary Surface.
In Direction 1 and Direction 2, select sketch curves, model edges, or faces to define the surface. Boundary surfaces are created based on the order you select curves (so selection order matters). The two directions are interchangeable and should produce the same result regardless of whether you select curves as Direction 1 or Direction 2. Apply Tangency/Curvature constraints if needed, then enable Create Solid (if available) under Options and Preview.
Click OK. The Boundary Surface feature will create the patch surface and, when it closes the last opening of an enclosed surface set, it can also convert the surface body into a solid body.
Best for: High-quality patches where you can clearly define two directions (often four-sided regions) and want stronger continuity control.
Common pitfall: If your boundary curves don’t intersect cleanly or the region is topologically messy, the surface may twist or fail.
Trim Surface
Trim Surface trims intersecting surfaces using other surfaces, planes, or sketches. It’s frequently used to “clean up” overlaps and remove excess so the remaining surfaces can form a closed volume. You can access it from the Surfaces toolbar or through Insert > Surface > Trim.
To create a solid body, select Mutual under Trim Type in the PropertyManager (this trims multiple surfaces against each other). Under Selections, select the surfaces that will represent the final closed shape. With Keep Selections enabled, select the faces that form the enclosed volume. If your selected, trimmed result forms a closed volume, the Create Solid option becomes available.
Click the Green Checkmark and you will have your solid body.
Troubleshooting: When “Create Solid” Is Greyed Out (or the Feature Fails)
1) You still have an opening (even a tiny one)
If “Create Solid / Try to form solid” won’t appear, assume you have at least one boundary edge somewhere. Common causes include micro-gaps between edges, missing patches, or edges that don’t meet within the current knit tolerance. Use:
- Knit Surface > Gap Control to locate gaps and adjust tolerance appropriately.
- Evaluate > Check to identify problematic edges/faces and gaps.
2) The model is non-manifold (or creates “zero thickness” situations)
A true solid must have valid topology. If edges are shared incorrectly (for example: overlapping surfaces, internal faces, T-junctions, or “touching at a line/point”), you can trigger non-manifold or zero-thickness problems that prevent a solid from forming and can also break slicing for 3D printing.
3) Thicken fails on complex curvature
Thicken is effectively an offset operation plus side-wall creation. If the offset distance causes the offset surface to collide with itself (common when the thickness exceeds small local radii), the feature can fail. Typical workflow fixes include reducing thickness, splitting the surface into simpler regions, or adjusting geometry in the tight-curvature areas before thickening.
4) Imported geometry needs repair first
If you’re working with STEP/IGES, run Import Diagnostics early. It can repair faulty faces and help knit surfaces into closed bodies so you’re not manually chasing dozens of tiny defects.
3D Printing Checklist After You’ve Converted to a Solid
- Confirm watertight/manifold intent: Your solid should represent a clean interior and exterior with no accidental openings or non-manifold conditions.
- Verify minimum wall thickness: Minimum printable walls vary by material, printer, and process. If you’re printing through a service, check their published guidelines; if you’re printing in-house, test your chosen material/printer combination.
- Export with appropriate mesh resolution (STL/3MF): SOLIDWORKS export settings typically allow you to control tessellation using deviation (chordal tolerance) and angle tolerance. Too coarse can create visibly faceted curves; too fine can create huge files with little real benefit.
FAQ
Can you 3D print a surface body directly?
Usually, no. A surface body is zero-thickness, and most slicers expect a closed, watertight volume (or a mesh that accurately represents one). The practical solution is to either close the surface set and create a solid (Knit/Fill/Boundary/Trim) or add thickness (Thicken).
What’s the fastest method if my surfaces already enclose a volume?
Start with Knit Surface and enable Create Solid / Try to form solid. If you have a single enclosed surface body and Knit isn’t applicable, try Thicken with Create solid from enclosed volume (if available).
Which patching tool should I try first: Filled Surface or Boundary Surface?
Use Filled Surface for general “close this opening” scenarios (especially irregular boundaries). Use Boundary Surface when you can define clean Direction 1/Direction 2 curves and want more control over tangency/curvature quality.
