SOLIDWORKS Simulation includes many helpful features that reduce simulation setup and run time. Many of these features are automatic, and it may be tempting to accept the SOLIDWORKS defaults when setting up a new study to get quick results. However, the auto-generated mesh type settings are always worth reviewing before getting too far.
Using correct mesh types goes a long way in reducing run time and improving results accuracy. This quick tutorial will explain the differences between each mesh type and how to incorporate each mesh type into an example SOLIDWORKS Simulation static study.
Mesh Overview
In finite element analysis (FEA) software such as SOLIDWORKS Simulation, a mesh consists of part geometry broken down into consistently shaped discrete elements that stress calculations can be performed on. The more refined a mesh is, the more elements it has and the more accurate the analysis will be. However, the more elements there are, the more calculations are performed and the longer the simulation time will be. An ideal level of mesh refinement would be enough elements to get results within a reasonable margin of error from an equivalent highly refined mesh but not so many that the simulation takes an unreasonable amount of time to complete.
The following mesh types supported by SOLIDWORKS Simulation serve to utilize mesh elements efficiently so less elements are needed to achieve accurate results. Correctly applying mesh types can therefore reduce simulation time without sacrificing accuracy.
Solid Mesh
A solid mesh is automatically created for any part body where requirements for shell or beam meshing are not satisfied. This mesh consists of 3D solid elements. This mesh type is best utilized for bulky bodies, with few or no thin walls. If a part has varied thicknesses or it is easy to fit more than one row of elements in the thinnest section, the part is likely a good candidate for a solid mesh.
Shell Mesh
A shell mesh is automatically created for any sheet metal or surface bodies with uniform thickness. This mesh consists of 2D elements populated on the mid-plane of the part with part thickness taken into account as a separate parameter. Because 3D elements are not needed to define the part thickness, it takes significantly fewer elements to achieve a good quality shell mesh than a good quality solid mesh. This could make a huge difference in run time, especially for larger area sheet metal parts.
Beam Mesh
A beam mesh is automatically created for any structural member body and can be applied to any part. This mesh consists of “beam elements”, which are just individual lines each defined by two end points and a cross-section. This is visualized in the mesh as cylindrical surfaces to clearly see mesh resolution. Like a shell mesh, a beam mesh significantly reduces the number of elements required to achieve a good quality mesh, making it easier to keep run time down.
When a beam mesh is employed in a multibody part or assembly, SOLIDWORKS Simulation imprints the cross-section onto connecting bodies.
Completing A Static Study with All Mesh Types
After setting up a static study with a solid, sheet metal, and structural member part, SOLIDWORKS Simulation will automatically select solid, shell, and beam mesh types, respectively. If set up correctly, you should see the following icons under Parts. If the study includes a beam mesh, you will also see a new field called “Joint Group” which can be used to view beam endpoints.
To illustrate that non-solid mesh types will not affect part interactions, try running Interaction Viewer.
For bodies with solid and shell mesh types, you can specify interactions, fixtures, and loads as normal. However, beams are more restricted. Beams only support bonded interactions, fixtures applied to joints (end points), and loads applied to joints, whole bodies, or reference points. The options are clearly specified in each configuration window.
In the example, we specified a force load at the far end joint of the beam and fixed the bottom face of the solid part. With those and the mesh specified, the next step is to simply run the study.
The automatically generated Displacement and Strain plots display on all parts. However, the Von Mises Stress plot is not displayed on beams. This is because SOLIDWORKS processes different stresses for solids and shells than it does for beams.
- Solids/Shells
- Von Mises
- Normal
- Shear
- Etc.
- Beams
- Axial
- Bending
- Shear
To display a stress plot on a beam, Beams needs to be selected during stress plot configuration. There is an option to render the beam profile, rather than the mesh profile, if that is desired.
Mesh Analysis Compared with All Solid Mesh Types
The above example utilized a mesh with 16,885 elements. That level of refinement resulted in 0 elements with a Jacobian ratio greater than 10 and 0 elements with an aspect ratio greater than 5, which indicates 100% good quality elements. The higher the percentage of good quality elements in a mesh the better. Generally, above 90% can be considered acceptable, so this is an ideal mesh refinement, probably more refined than it had to be. However, due to the simplicity of the geometry, the mesh generation and solution both took only 2 seconds to complete, so the extra refinement is not an issue.
A mesh with the same element size parameters using all solid mesh types produces 20,078 elements, where 0 elements have a Jacobian ratio greater than 10 and 73 elements have an aspect ratio greater than 5. While this mesh is composed of 96% good quality elements, this illustrates that even with more elements, using all solid mesh types does not produce the same quality as when shell and beam mesh types are used. In studies with a greater ratio of sheet metal or beam parts to solid parts, this disparity in quality can become significantly more pronounced.
Below, the all-solid mesh was refined until there are 0 poor quality elements as in the shell and beam mesh type study. This produces 145,918 elements – nearly 9 times the number of elements than in the original study. In this case, the mesh generation and solution each took 9 seconds to complete, or 4.5 times longer than the original study took in total. With geometry this simple, the difference in solution time is trivial. However, processing time can quickly get out of hand for more complex geometries, especially with many more sheet metal or beam parts.
Troubleshooting
Most issues when working with non-solid mesh types are due to incorrect model preparation for simulation.
Shell mesh types can only be used for sheet metal bodies with uniform thickness or surface bodies. If importing a non-native part file intended to be sheet metal, the part will need to be converted to sheet metal to be processed with the correct shell mesh type. Also, any features that may affect sheet metal part thickness, such as non-thru extruded cuts or countersinks, need to be removed. Beam mesh types can be used for any parts, though they are automatically configured for structural members. If importing a non-native part or you would like to use a beam mesh for a solid or sheet metal part, you may right-click the part in the study and select Treat as Beam. When doing so, double-check that joints are in the correct locations.
Something else to keep in mind for beam meshes is that any cutouts or holes applied to a structural member will be ignored in the mesh. This is because beam meshes only consider end points and cross-section. If there are any such features along the beam that are critical for analysis, then the part may be a better candidate for a solid mesh. To apply a solid mesh to either a shell or beam mesh, right-click the part in the study and select Treat as Solid. Similarly, you can select Treat as Sheet Metal or Treat as Beam for parts treated as solids.
