How to Fix Zero Thickness Geometry in SOLIDWORKS

One of the most common modelling errors faced by SOLIDWORKS users is the Zero Thickness Geometry error. Many designers know how to avoid it, but only a few understand why SOLIDWORKS shows this error and what it really means for the model.

In this blog, we will break down:

• What Zero Thickness Geometry actually is
• Why SOLIDWORKS does not allow it
• And finally, three simple ways to solve it

Zero Thickness Geometry (also known as non-manifold geometry) happens when two solid features in your model touch each other only at a single edge or a single point, without sharing a real volume of material.

A valid solid body in SOLIDWORKS must follow one strict rule:

Every edge in a solid must have exactly two adjacent faces.

If an edge has:

·        Only one face → invalid

·        More than two faces → also invalid

·        Features touching only at a point or line → non-manifold → error

So, if a corner or an edge collapses to a zero-thickness connection, the software immediately flags it.

Why SOLIDWORKS Does Not Allow Zero Thickness Geometry

It Is Physically Impossible

In the real world, you cannot manufacture a solid part where two bodies coincide at an edge or at a vertex. Solids must have thickness everywhere.A zero-thickness connection cannot exist as a real manufactured part.

It Breaks the Mathematical Rules of Solid Modelling

SOLIDWORKS uses B-Rep (Boundary Representation) modelling.This needs clear definitions of inside, outside, edges, faces, and volume and this definition is validated by Euler’s Formula.

Zero-thickness conditions break Euler’s formula, which governs how vertices, edges, and faces must relate for a valid 3D solid.Allowing zero-thickness would destroy model integrity.

Zero-thickness conditions break Euler’s formula, which governs how vertices, edges, and faces must relate for a valid 3D solid.Allowing zero-thickness would destroy model integrity.

It Causes Problems Downstream

If SOLIDWORKS allowed non-manifold geometry, you would face issues in:

·        CAM programming

·        Drawings (section views fail)

·        3D printing (slicer rejects the file)

·        Meshing errors in Simulation

·        Import/export between CAD systems

·        Combining or subtracting bodies

So instead of letting you proceed with a damaged model, SOLIDWORKS blocks it early.

What Conditions Cause Zero Thickness Geometry?

There are several common modelling situations that instantly create this error.
Below are the ones every designer eventually encounters.

Overlapping Edges

In this situation, two features create an edge that ends up being shared by four faces instead of the required two.This instantly becomes a zero-thickness condition.

A valid solid must have exactly two faces meeting at every edge. When four faces meet at the same edge, the part becomes non-manifold, which is physically impossible and mathematically invalid.

SOLIDWORKS blocks it to prevent further modelling issues.

Bodies intersecting at point/vertex

Here, two extruded features touch each other only at one point (a single vertex).

There is no actual material connecting the bodies. Since the bodies do not share any thickness or overlapping region, SOLIDWORKS sees this as zero volume and flags it as Zero Thickness Geometry.

Tangent Contact Between a Cylinder and a Block

When The cylinder touches the block along a perfect tangent line with no real intersection. A tangent contact means the cylinder and block only touch along one line, and do not share any volume.SOLIDWORKS cannot treat this as a single solid body because the connection has no thickness.

A Cut-Extrude Touching the Edge of a Hole

If a slot or rectangular cut touches a circular hole exactly at one point, the bodies do not fully intersect. Because the new cut does not actually intersect the existing cut’s volume, they meet only at a single line or point.

How to Fix Zero Thickness Geometry in SOLIDWORKS

Here are the three most reliable methods to solve the issue.
These are easy to apply and work for almost every scenario.

1.   Add a Small Gap Between the Bodies

This ensures the bodies do not meet at a point or edge. Even a tiny clearance avoids the zero-thickness condition. This solution is best when the two bodies should not physically overlap. This is done by

·        Add a small dimension (example: 0.1 mm)

·        Break tangent relations in sketches

·        Offset the feature slightly

·        Move the profile away from the touching edge

2.   Make the Bodies Intersect Properly

Instead of touching tangentially or at a point, make the features overlap slightly so there is real material between them. This creates a valid solid with proper edges and faces, satisfying Euler’s rule.

3. Use a Multibody Part (Do Not Merge). 

If your design requires the bodies to touch tangentially or at a single point, do not force them into one solid body. SOLIDWORKS allows this because each body is treated independently — zero-thickness rules apply only inside a single body. 

Now that we understand what Zero Thickness Geometry really is, it becomes much easier to avoid this error and fix it quickly whenever it appears. With this clarity, we can design better, make fewer mistakes, and work more efficiently in SOLIDWORKS. Let us continue creating cleaner, smarter, and more reliable models.

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