What is Zero Thickness Geometry?
Zero-Thickness Geometry (also known as non-manifold geometry) exists when edges or vertices in a solid model do not properly connect with adjacent geometry. A Zero Thickness Geometry is a solid geometry that touches itself at a point or an edge. Every edge of a solid body must have exactly two adjacent faces.
Although, there are some CAD softwares that allows this but SolidWorks does not allow zero thickness geometry because it can lead to mathematical problems and weird errors in the model as you continue to work. Also, it is impossible to manufacture a part with Zero Thickness Geometry in a single piece.
Potential Error Messages in SolidWorks
Note that Solidworks doesn’t always show errors mentioning that there is a Zero Thickness Geometry. Following error messages may also be shown because of this:
- Features: Unable to create this feature because it would result in zero-thickness geometry.
- Split: The body cannot be split by selected tool(s).
- Section View: Sectioning at this position will produce invalid bodies. Please select a different section position. (OR) The model could not be properly sectioned by the section line. Please check that the section line cuts through the model.
What are the types of Zero Thickness Geometry?
In this article, we will explain all types of Zero Thickness Geometry and also how you can troubleshoot them. So let us begin.
- The image below shows a Tangent Line, where zero thickness is located.
- The edge, where zero thickness geometry is located. (Notice that the highlighted edge has more than two adjacent faces.)
- The vertex, where zero thickness is located.
- Zero thickness also occurs when you attempt to perform a cut that is tangent to a hole. If this cut were to be allowed there would be no thickness left at the point where the line is tangent to the hole. This is frequently the cause of failed section views.
How to fix Zero Thickness Error?
- Add or remove enough solid material to the area of the zero thickness geometry to properly connect the edges and vertices.
- When creating the feature, in the PropertyManager, if available, clear the Merge Result option in Direction. This creates a multibody part.
How to Troubleshoot Zero Thickness Geometry?
Method 1: Using the Interference Detection Tool
Let’s take a look at this geometry. We have created a sketch that we want to extrude. Everything may seem good at first glance as it is a fairly simple and fully defined sketch.
But as soon as we go to create the Boss-Extrude feature we get this error.
It says there is a Zero Thickness Geometry but doesn’t say where that Zero Thickness is located?
To troubleshoot it, we are going to create this feature by unchecking the Merge Result option present in the Direction menu. Without the Merge Result option, that feature will create a new solid body (See image below). But there are various reasons why you may not want a different body, so we are going to find where this Zero Thickness Geometry is located and eliminate it.
Note that this Merge Result option is not available in all of the features that are used to add material to the model.
1. There is a tool called Interference Detection that can help us find where that is. To initialize it go to Interference Detection present in the Evaluate tab or use the SolidWorks Search options.
2. In Selected Bodies, the entire part will come pre-selected. However, if your part has a lot of Solid Bodies, you may want to select the body that you just created and the bodies that are nearby it. Running Interference Detection on a huge number of bodies may take a lot of time.
3. Under the Options menu, it is necessary to check the Treat Coincidence as Interference option and then press Calculate. It will show you all the interferences that are present in the selected bodies.
4. Click on all the Interferences one by one that is shown in the Results. If one of the Coincident Interferences shows a straight line for interference in the graphics window then we have found our culprit.
Note: The Red-line in the graphics area is not marked by us. Interference Detection uses red color to show interferences.
So now that we know where this Zero thickness Geometry is located we can extend the sketch to add more material and rebuild the feature with the Merge Result option checked to merge the bodies.
In this example, we showed you how to locate the tangent line where Zero Thickness Geometry is located. Similarly, this same method can also be used to find the edge where Zero Thickness geometry is located.
Drawbacks of this method:
- The feature that is used to add material should have a Merge result option for you to uncheck. Features such as Wrap don’t allow this.
- You can’t use this method when you’re getting Zero Thickness Geometry during a cut or removal of material.
- You can’t locate the Zero Thickness vertex using this method.
Method 2: Trial and Error
This is the approach you gonna have to use where the Interference Detection can’t help. Here are some tips to avoid Zero Thickness Geometry error:
1. In a sketch, always give all the necessary dimensions and relations. Working with fully defined sketches is the best way but it’s not necessary always. Sometimes you think that a line is horizontal but if there is no Horizontal relation to it, there is a chance that it’s at a very small angle, say 0.001 degrees to the horizontal which you won’t be able to tell just by looking at it.
2. If you are using a Cut feature and get this error, find the entities (lines, arcs, splines, etc.) that are on the edge and have a tangent relation applied to them. Remove the tangent relation and move that entity a very small distance. This method also works for Splits that are failing due to Zero Thickness Geometries.
3. If you get this error during Section Views, try to shift the section line/plane by a small distance. It usually solves the problem.
4. If you use Convert entities/Silhouette entities to convert an edge or something, it is recommended (unless you know what you are doing) not to delete their relations as doing so may cause Zero Thickness Errors.
5. If all else fails, then the culprit may be a feature that you have previously created which had errors but SolidWorks allowed that. In Settings, you will find Verification on Rebuild under the Performace menu in System Options Tab.
When this option is active, SolidWorks checks every new or changed feature it is building against all existing faces in the model, not just the adjacent ones which it does when this option is deactivated. This ensures that there is no bad geometry present in your model. However, this option is inactive by default because it comes at the cost of performance, especially in large and complex models with many faces.
After you have checked this option and clicked Ok to save the settings, rebuild the entire model by pressing Ctrl+Q on your keyboard. After the rebuild is done, SolidWorks will let you know if it has found any errors or warnings in the previously created features.