Hybrid Mesh Modeling in SOLIDWORKS 2022
Working with mesh bodies in SOLIDWORKS has historically been a rather involved and often difficult process, typically including a lot of cleanup and manual intervention to create “real” solids and surfaces from imported mesh files or, alternatively, utilizing the limited capacity of Boolean operations to achieve the desired results. Additionally, adding subsequent features to models containing both traditional and mesh body types has always been problematic, only complicating and slowing down the design process.
SOLIDWORKS 2022 introduces a new workflow for mesh enthusiasts known as Hybrid Mesh Modeling, which allows users to directly combine traditional SOLIDWORKS geometry with mesh geometry. In addition, most classic features (think extruded cuts and fillets, for example) can now be added to the combined result, even in areas containing both faceted mesh geometry and traditional SOLIDWORKS geometry.
This new capability follows the release of Parasolid v33.1 (the kernel used by SOLIDWORKS), where it is also known as convergent modeling.
To demonstrate a use case for working with hybrid mesh modeling, consider the unicycle seat pictured above. The goal is to combine the mesh file (in STL format) of the handle with the seat, which was created using traditional SOLIDWORKS features. Once they are combined, I will want to add some downstream features for the placement of fasteners and create a blend between the handle and the seat. Please note that this workflow does involve a multibody approach and the Insert Part command.
First, make sure to open the mesh file you plan to work with on its own and convert it to a solid body. Typically, mesh files import as graphics bodies to improve performance, which is great for visualization but does not offer much in the way of design. Once the mesh file opens, look for a Graphic Bodies folder in the FeatureManager design tree. Expand this folder, right-click the body and use the context menu to select Convert to Mesh Body. Then save the file as a SOLIDWORKS document.
Once that is done, navigate back to your main document (the seat). Use the Insert dropdown, choose Part, browse to the newly saved SOLIDWORKS file containing your mesh body and select Open. You’ll find that the PropertyManager for this command will allow you to choose a configuration, if applicable, along with any information you’d like to transfer.
Because we are inserting one existing document into another, any information we choose not to transfer will be inaccessible in our top-level design. While dimensions and materials typically are not important when inserting mesh files, transferring the default planes along with any axes and/or coordinate systems (if you created any in the mesh file prior to inserting it) may help with proper positioning.
Optionally, use Locate Part with Move/Copy Feature to activate the Locate Part command immediately after inserting the mesh file to reposition the body.
Click OK once finished and the mesh file will be inserted. By default, a link will be created to the original file, so if any updates made to the original will propagate to the inserted mesh. This can be controlled in the Insert Part PropertyManager. Your design now contains both a traditional SOLIDWORKS body and a mesh body, giving you access to the hybrid mesh modeling workflow.
Up to this point, however, nothing is particularly novel—this is the same workflow that would be used to add a mesh body to an existing document in SOLIDWORKS 2021 and earlier versions.
But this is where things get interesting. Let’s take a look at some of the improvements SOLIDWORKS brings to mesh modeling in 2022, starting with Combine. With the handle model in proper position, we will use Combine in Add mode to merge these two bodies together.
It was technically possible to combine SOLIDWORKS and mesh bodies prior to 2022, but it required that the SOLIDWORKS body first be converted to mesh, which limited many downstream applications. Now, taking a look at the result in SOLIDWORKS 2022, you will see that boththe traditional and mesh geometry are maintained along with easily accessible dimensions, even though the result is a still single body.
Classic SOLIDWORKS features such as fillets and extruded cuts/bosses are supported between body types as well and the results can be rather interesting. For example, adding a fillet between the mesh and SOLIDWORKS bodies yields additional faceted mesh faces as seen below.
However, adding features that do not blend with any faceted mesh geometry are treated just like regular SOLIDWORKS features and result in real SOLIDWORKS geometry suitable for referencing, sketching (assuming the resulting face is planar) and other downstream operations. Here, we have added a couple simple extruded cut/boss features to illustrate this behavior. Again, while technically possible to achieve similar results prior to SOLIDWORKS 2022, the old workflow required the construction and conversion of separate bodies and the use of (often several) combine operations and the result was still a fully faceted mesh body with additional limitations.
There is, however, one exception to this behavior that we have identified so far. If any features are created using an offset from Surface end condition where a mesh face is specified as the reference surface, the resulting end face of the feature will be a mesh face. As such, it is not possible to sketch on the resulting face, even if it is planar. Below, we have created a slot-shaped extruded cut illustrating this behavior. As you can see, the side faces of the feature are SOLIDWORKS geometry, whereas the end face is faceted, as a result of the Offset from Surface end condition.
Hybrid (or convergent) mesh modeling is a significant step toward enabling better collaboration between SOLIDWORKS users and their mesh-oriented counterparts, but it still comes with some important limitations that need to be considered prior to diving head-first into mixed-body design.
First, while hybrid mesh modeling allows you to maintain your original SOLIDWORKS geometry, keep in mind that you are still introducing mesh elements into your design. Though well-suited for applications such as 3D printing, mesh files are known for causing difficulty in CNC and CAM applications. Therefore, traditional manufacturing techniques may not be suitable for mixed-body models.
Additionally, there are still significant limitations for mesh models in the SOLIDWORKS drawing environment. As of this release, it is not possible to reference mesh bodies for the creation of dimensions or other annotations and section views cannot be created for meshes in drawings. This may add another layer of difficulty to the manufacturing process for hybrid models, as shown below.
All that being said, you should find working with meshes easier in SOLIDWORKS 2022, as being able to directly combine SOLIDWORKS and mesh body geometry has significant implications. Rather than limiting your modeling approach to Boolean operations such as Combine in multibody parts, hybrid mesh modeling enables the majority of standard SOLIDWORKS features to be applied to models with mixed body types, even in areas that blend traditional and mesh geometry. In most cases, faces resulting from added features are created in true SOLIDWORKS BREP format and can be used in downstream operations—or even sketched on, if planar— which opens the door for many new creative uses.
Whether you collaborate directly with mesh users, download mesh files from online services such as GrabCAD, or create your own mesh models in a third-party program, hybrid mesh modeling is an exciting and long-awaited enhancement to SOLIDWORKS 2022 for any mesh enthusiast.
About the Author
Jacob Ames is a Senior SOLIDWORKS Applications Engineer with Hawk Ridge Systems based out of Olympia, WA. He’s been producing SOLIDWORKS content, training students, and providing product demonstrations for over 5 of his 10+ years of CAD experience. If he’s not in front of his computer, you’ll likely find him playing video games or wandering the trails of the Pacific Northwest.