What a Fine Mesh We’re In
Until recently, the number of SOLIDWORKS users who needed to import mesh files in SOLIDWORKS was relatively small. They would have typically needed to reuse geometry created in an artistic modeling software, such as Maya or 3DS Max, or import point cloud files representing scanned data. The process of importing and converting these files to SOLIDWORKS as usable geometry was cumbersome and frustrating, and many times the point cloud would be so large that it could not be imported into older SOLIDWORKS versions.
With the 3D printing revolution, the number of mainstream SOLIDWORKS users who need to insert 3D-scanned models into assemblies, or modify such models, increased exponentially. These “typical” users, accustomed to the speed and elegant workflows available when working with SOLIDWORKS models, expressed strong feelings when facing the awkward methods for dealing with mesh files. They also developed innovative ideas for repurposing the imported scanned data.
- Insert a 3D-scanned part into an assembly the fastest way possible.
- Determine mass properties of the imported model.
- Get measurements from the imported model.
- Apply mates to a 3D-scanned component in an assembly.
- Show 3D-scanned component in a bill of materials.
- Show 3D-scanned component in a drawing view.
- Attach dimensions to a 3D-scanned component in a drawing view.
- Use imported geometry as reference for creating SOLIDWORKS native entities.
- Modify geometry originating from point cloud files.
“And… could we perform all these operations fast and easy? Thank you!”
SOLIDWORKS is known as a company that listens to its user community—most of its new enhancements are user-driven. It did not take long to discover solutions and enhance the software.
Let’s look at the answers provided by SOLIDWORKS 2018 in streamlining these operations, using specific case studies. For more details and technical terms, please use this link to access the relevant chapter inside the What’s New in SOLIDWORKS 2018 document.
Challenge 1: Import a Mesh File to Quickly Create a Drawing and Dimension the Model
When importing large mesh files, the user should always ask: “What do I need this file for?” Depending on the answer, he or she could skip over cumbersome converting operations.
The mesh file formats that could be imported in SOLIDWORKS 2018, without the need for accessing the ScanTo3D add-on, are shown in Figure 1.
The most common are:
- STL (Standard Triangle Language, or Standard Tessellation Language): Native format for stereolithography CAD
- OBJ: Open-source simple data-format representing 3D geometry alone
- 3MF (3D manufacturing): XML based 3D printing format developed by the 3MF Consortium. In addition to geometry, it includes information about material and colors, which could not be represented in the STL format.
For full control over the way a mesh file would open in SOLIDWORKS, in the Open File dialog, filter by the file type, as shown in Figure1; do not use the default All Files option.
By selecting a certain file type, you get access to the Options button, see Figure 2.
Options allow the user to import massive amounts of data as Graphics Bodies, see Figure 3.
Figure 4 shows the result of importing a graphics body. The import process was almost instantaneous for this model.
Notice that in addition to the Graphic 1 feature, SOLIDWORKS collects all the graphics bodies in their own dedicated folder.
Let’s change the color of the whole part. The standard workflow for applying and managing appearances has been extended to graphics parts too. Let’s “paint” it yellow.
At this time, appearances cannot be controlled at the graphics body or graphics feature level.
When changing the display style for the model in anything other than shaded, the user can see the triangular facets that are typical for meshes.
Figure 7. Facets displayed in Shaded with Edges and Hidden Lines Removed.
When working with graphics entities, it is important to be able to select individual facets, edges or vertices from a graphics body. For that, let’s add specific mesh filters to the filter toolbar.
A quick way to display the filter toolbar is using a keyboard shortcut. The default is F5 (Figure 8).
Let’s use the Customize tool for dragging these three icons over the filter toolbar (Figure 9).
That enables advanced selection abilities for graphic entities (Figure 10).
Note that there is no need to activate such filters when using the Measure tool (Figure11).
Let’s save this part and insert it into a drawing. The first thing to notice is that only draft quality views show graphics bodies. Since SOLIDWORKS needs the body data for computing the edges of high-quality views, such views will be empty (Figure 12).
Once the view quality is set to draft, SOLIDWORKS displays the BREP facets directly. All display styles are available: Shaded, Shaded with Edges, HLR, HLV and Wireframe (Figure 13).
There are serious limitations with what can be done with a graphics model in a drawing. At this time, you can only create model views and projected views of such models. Sections, details or other type of views are not currently supported.
Because there are no SOLIDWORKS entities in the model, trying to apply dimensions will not work. That is the same limitation that one encounters when attempting to dimension SpeedPak assemblies.
The good news is that a similar technique to the one used in preserving SOLIDWORKS entities containing body data in SpeedPak can be applied in SOLIDWORKS 2018 for extracting SOLIDWORKS surfaces from graphics models.
Let’s switch back to the part environment. In the Command Search file type “mesh” and drag the resulting command over one of the toolbars to make these specific tools easily accessible (Figure 14).
Now let’s create a surface body directly from the mesh. I intend to display a dimension on the drawing representing the thickness of the wall in a certain area. To make the selection easier, I will switch the display style to Shaded with Edges.
Activating the Surface From Mesh command offers the option to quickly generate different surfaces. Primitives like planar, sphere, cylinder and cone are available. For detailed information on how to use this tool, click here.
In this case, I will attempt to extract a planar face representing the thickness. Since the result will be a planar face, I will select only on facet and count on SOLIDWORKS to select the rest of the facets laying in the same plane and connected to this one (Figure 15).
The result is a SOLIDWORKS surface body, which can be seen in Figure 16.
Let’s return to the drawing and apply the dimension to the edges of the surface body (Figure 17).
Warning: In SOLIDWORKS 2018 SP0.1, you might encounter a situation where the graphics bodies will be hidden in the drawing views upon a drawing rebuild. I will report this issue to SOLIDWORKS and report back in the comments section with any possible workarounds.
Challenge 2: Reference the Mesh Entities in Sketches for Creating Standard SOLIDWORKS Features
Let’s create a gasket part that would match the mesh model. For that, follow the steps described above for inserting the mesh into a new SOLIDWORKS file as a graphic body.
New in SOLIDWORKS, I can now refer Mesh Facet Vertices in Sketches. First, let’s turn the Filter Mesh Facet Vertices on, see Figure 18.
Since the Plane feature does not currently accept a facet, facet edge or facet vertex from a graphic body as input, let’s define points in a 3D Sketch.
Start a 3D Sketch and add 3 Point entities on vertices of the facets where the gasket will be placed (Figure 19).
Use these points to define a new plane (Figure 20).
Open a 2D sketch on the new plane and sketch lines and arcs that have coincident relations to the facets vertices. Notice that relations to the mesh vertices can be inferred only when the viewport is oriented normal to the sketch plane (Figure 21).
Once the sketch is created, it can be used in defining standard SOLIDWORKS features. See Figure 22.
Note: This specific case study could have been solved faster by using the Surface From Mesh feature to extract the flat facets of the gasket, followed by a Thicken command (Figure 23).
The standard SOLIDWORKS planes, sketches, faces, edges and vertices can be easily used in defining mates for such components in assemblies.
This way, the user gets the best of both worlds:
- Speed due to using graphic bodies
- Precision due to using SOLIDWORKS standard entities in mating
It is worth mentioning that Graphic Bodies or components can be sectioned in part and assembly environments, as long as the Graphics-only section setting is checked (Figure 24).
Challenge 3: Modify a Mesh File in SOLIDWORKS
The 3D-printing community will be happy to learn that one of the biggest enhancement in SOLIDWORKS 2018 is the ability to create new mesh bodies and modify existing meshes using Boolean operations.
Let’s add holes to our model before 3D printing. For that I will import the model as a mesh (Figure 25).
The result is a solid mesh body (Figure 26).
Let’s define the plane for the hole orientation based on three vertices of a facet (Figure 27).
In a sketch opened on the newly created plane, I drew a circle representing the hole profile. To fully define the sketch, I added two reference points coincident to two vertices in the mesh (Figure 28).
Let’s define the tool for punching the hole by extruding the sketch in both directions (Figure 29).
To apply a Boolean operation between similar types of bodies, I need to convert the solid body of the tool to a mesh body. For that I will use the ConvertMesh Body command (Figure 30).
Let’s subtract the tool from the main mesh body (Figure 31).
The result is a hole through the original mesh body (Figure 32). Now I can send this part to the 3D printer.
SOLIDWORKS 2018 is a game changer for two types of users:
- Users who work with large point cloud data and need to:
- Quickly insert and precisely mate imported components containing graphic bodies in an assembly.
- Section imported components containing graphic bodies.
- Reference meshes in creating new features or components.
Users who need to quickly modify the mesh of their models in preparation for 3D printing.
About the Author
As an Elite AE working for Javelin Technologies, Alin Vargatu is a Problem Hunter and Solver, and an avid contributor to the SOLIDWORKS Community. He has presented 19 times at SOLIDWORKS World and tens of times at SWUG meetings organized by four different user groups in Canada and one in the United States. Vargatuis also very active on SOLIDWORKS forums, especially on the Surfacing, Mold Design, Sheet Metal, Assembly Modeling and Weldments sub-fora. His blog and YouTube channel are well known in the SOLIDWORKS Community.