Mesh files, a common type being STL, are a type of 3D model files that store information through polygons with vertices, edges, and faces. They differ from SOLIDWORKS files, which have parametric data that can be defined through arithmetic and interpolations, and they require processing to be used in SOLIDWORKS in most cases.

SOLIDWORKS provides tools to work with mesh files that can be found in the Mesh Modeling tab (activate it by right-clicking on the CommandManager > Tabs > Mold Modeling).

Note: Due to the numerous facets and faces that a mesh file can contain, SOLIDWORKS may perform poorly until the mesh data has been reduced, either natively, with other software, or with the Decimate Mesh Body command. It is recommended to import in Parasolid or STEP files for the best initial import result for SOLIDWORKS, if possible.

Mesh Files as Solid, Surface, or Graphics Body

We can try importing the file as solid or surface before importing the mesh files into SOLIDWORKS by changing the import option in Tools > Options > System Options > Import > File Format [STL/OBJ/OFF/PLY/PLY2].

However, data translation between different file types and software can cause inaccuracy. It is likely that when you try importing the data as solid bodies, it will result in surface bodies that need to be fixed with the surfacing tool due to gaps. It's also likely that when you try importing the data as surface bodies, it would result in numerous surface bodies that make it inefficient to work with. Importing graphics bodies and then modifying them may be a better option.

How Can Graphics Bodies from Mesh Files Be Used?

There are three typical workflows for working with mesh bodies after importing and cleaning up the graphics bodies:

1. Use the graphics bodies as physical or visual references.
2. Use the graphics bodies to create the standard Boundary Representation (BREP) geometry (such as surfaces and solids), with tools such as Surface from Mesh.
3. Create a hybrid model that contains both geometry made from SOLIDWORKS and geometry from the graphics bodies.

Mesh geometry can use the following tools in SOLIDWORKS:

• Determine mass properties.
• Add coordinate axes, reference axes, and reference planes.
• Select mesh vertices when sketching and add sketch relations.
• Measure distances between mesh elements using the Measure tool.
• Create section views.
• Trim surfaces.
• Shell, offset, and thicken mesh elements.
• Apply appearances and render.
• Detect interference.

Mesh File Graphics Body Import Example

In this example, we will demonstrate some of the tools that can be used with a mesh file imported as graphics bodies. One body will be converted to a mesh solid body, and another will be formed into surfaces to be knitted together into a SOLIDWORKS solid body with the steps below:

1. Import an STL file as 2 graphics bodies

   

2. Select the rectangular graphic body and click on the "Convert to Mesh Body" command

   

3. In the "Convert to Mesh Body" Property Manager, make sure that the desired body is selected. 
4. Check "Group facets into faces" to let SOLIDWORKS attempt to create individual faces instead of one continuous face. 

5. Click "OK" to finish the command.

   

6. The graphics body has been automatically hidden, and a mesh solid body has been added to the Solid Bodies folder. This solid body is not the same as the standard SOLIDWORKS geometry, and it can be manipulated with the tools listed above in the How Can Graphics Bodies from Mesh Files Be Used section

   

7. Next, we will be converting the second graphic body into surfaces and then into a solid. Click on the Mesh Modeling > Surface From Mesh command. 

   

8. In the "Surface From Mesh" Property Manager, we can use the Paint Select tool to paint over the facets we want to form into a surface. Alternatively, we can manually select the facets to group in the viewport. 

9. Click "OK" to create the surface body 

   

10. Repeat "Surface from Mesh" on the sides of the model that can be defined as one of the four types. Here, we cannot make the two surfaces that are the inner and outer arc of this model, but we can form the other four planar surfaces.

    

11. The rest of the steps would go into surfacing techniques. To summarize, we knitted the surfaces together and used the Boundary Surface command to create the missing surfaces. Then another knit allows us to create a solid.

    

Additional Mesh Tools in ScanTo3D

Users with SOLIDWORKS Professional or Premium have access to ScanTo3D. It allows users to convert the mesh file to surfaces and SOLIDWORKS solids with guided tools. Since a mesh is made of essentially 3-4 sided planar surfaces, the imported file will not be a smooth continuous surface, but rather 100s or 1000s of smaller surfaces. The ScanTo3D toolset can also help users create a workable solid from supported mesh file types *.3ds, *.obj, *.stl, *.wrl, *.ply, *.ply2.

Please see the following videos that go through the ScanTo3D operations from meshes to surfaces to solids:

• SOLIDWORKS: Working with Scan and Mesh Data
• An Overview of Scan to 3D in SOLIDWORKS

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.