Most people have come across a Zero Thickness Geometry error at one time or another. Generally, this is because of something that was unintentional, and can be corrected without much of an issue. We are going to look at what causes the Zero Thickness Geometry error, and how to maintain your design intent if you need to work around this error.
What Causes the Zero Thickness Geometry Error?
The first place to start will be defining why SOLDIWORKS throws this particular error, and luckily for us it is pretty straightforward. In SOLIDWORKS, every edge, whether it’s on a solid body or surface, must have two adjoining faces. Yes, even surfaces that have no thickness are still subject to this rule. So, any place in a single body where there is a coincidence at a point or along a line, we will see this error.
Common Examples of Zero Thickness Geometry
Let’s look at some examples. First, we have an edge shared by two separate bodies, see figure 1. As previously mentioned, this edge would have four adjoining faces as a single solid body, which is a problem for SOLIDWORKS.
Similar but slightly different is tangency. Tangency to a curve can also create an edge with more than two faces. Looking at the continuation of the first model, see figure two, there is a sketch line to highlight the edge that would cause the Zero Thickness Geometry error.
Additionally, looking at a second model, see figure 3, the edge of this extrude cut is coincident with the edge of the hole in the plate, which would also cause a Zero Thickness Geometry error.
Finally, a point coincidence can also cause the Zero Thickness Geometry error, see figure four.
Workarounds for Zero Thickness Geometry Errors
There are two major ways to work around this error. The first option is to create an imperceptible gap between the bodies to eliminate the error. The second is that we can overlap the two bodies in question in a subtle way to not change our design intent. In both cases, when dimensioning either gaps or overlaps, I use a dimension at minimum an order of magnitude smaller than the smallest tolerance in my part. Looking at the overall model we have to work with, see figure 5, we can use two features to combine all of those bodies into a single body.
Without altering any of the original model dimensions, we can combine three of the bodies together using tiny extrudes. These will eliminate the problematic geometry and not be visible in the final product. Here we can apply all sketch relations and then fully define the sketch with one dimension, see figure 6.
Moving on to the point coincidence, we could fix this with a midplane extrusion, or in this case a revolve, see figure 7.
Some Additional Considerations
Once you have your model successfully combined into a single body you may find yourself with some aesthetic issues you may want to correct, see figure 8. In this case, all the top surfaces of the model are now one face, which is affecting the original appearances of the model. This can be corrected using the Split Line tool.
To wrap up, let’s recap the three tips to consider when dealing with the Zero Thickness Geometry errors.
- Do you need a model to be a single body? If not, then don’t merge your features where you are getting errors.
- When combining multi-body models, does it make more sense to have imperceptible gaps or overlaps in your model to correct Zero Thickness Geometry errors? Be sure to dimension those gaps or overlaps at least an order of magnitude smaller than your tightest tolerance.
- Verify if you need to correct any appearances on your model.
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