LOADING

Type to search

Large Assembly Analysis with SOLIDWORKS Simulation 2021

CAD

Large Assembly Analysis with SOLIDWORKS Simulation 2021

Finite element analysis with SOLIDWORKS Simulation allows analyzing load cases and predicting the resulting stresses and displacements of a model directly within SOLIDWORKS CAD. The general process of setting up an analysis is the same for parts and assemblies, but as the number of components in an assembly grows, more care must be taken to ensure feasibility of an analysis.

This article will examine two case studies and describe techniques relevant for setting up any large assembly analysis, as well as some of the key relevant enhancements in SOLIDWORKS Simulation 2021 and other recent versions that make analyzing large assemblies much easier.

Example 1: Mold Base Solid Mesh Analysis

Consider the case of the injection mold in Figure 1 below. It’s important to establish a plan for the level of detail expected in an analysis before beginning study setup. In this analysis, the goal is to predict deflections and stresses around the mold cavities when subjected to the injection pressure and clamping forces.  

Figure 1. Case Study – Mold Base Analysis.

Contact interactions (formerly called “no penetration”) will be used sparingly at the interface between the mold halves. Contact significantly increases solve time, so the remaining plates will be assumed to be bonded. For loadings and restraints: one side of the mold is fixed, a clamping force is applied to the other side and a pressure is applied to the cavity faces exposed to the polymer.

Note: for this type of setup, it’s important that the clamping force is sufficiently large that it exceeds the clamp tonnage requirement, which can be estimated as the molding pressure multiplied by the 2D surface area of the cavities. Insufficient clamping force would cause the halves to separate and the solution would become unstable.

The pins and bolts in the assembly will be suppressed and replaced with the appropriate Virtual Connectors, a special type of simplified representation available in SOLIDWORKS Simulation to represent features such as pins, bolts, springs and welds.  

Geometry Preparation Tips

In an assembly with this many components, it’s worth creating a separate configuration just for analysis. SOLIDWORKS provides a variety of selection tools such as Select by Size to select small components or Select Toolbox to select all Toolbox components.

The most powerful method for identifying and suppressing small components is to use Assembly Visualization, pictured in Figure 2 below. This command is accessed on the Evaluate tab of the Command Manager and the column style display can be customized to sort by the volume of various components.

Figure 2. Assembly Visualization for small component suppression.

Shift-selecting components from the top selects the bulk of the small components that can be suppressed. If there are small components that are critical to the analysis, they can be Ctrl-selected to remove them from the selection before suppressing.

Calculating Mesh Sizes

The automatic defaults for mesh generation are often sufficient for creating a baseline mesh on many applications. But for a complex assembly, it may be necessary to manually determine mesh sizes. A foolproof workflow of determining the required mesh size is presented in Figure 3 below.

Figure 3. Simple Process for Meshing Success.

Open or isolate any parts that have small detailed features. Unnecessary detail can be suppressed or eliminated with extruded cuts or direct editing features such as Delete Face. Remaining detailed features must be resolved by the mesh. This means that, at minimum, the mesh size must be equal to or smaller than small edges and fillets.

Use the Measure Tool to size up the smallest features in the simplified model and use that measurement as an estimate for mesh element size. It’s best to apply a Mesh Control only in the areas where the refinement is necessary, then create the mesh.

Note that performing these steps at the part level has the benefit of fast mesh generation and the ability to quickly experiment with mesh sizes. Mesh controls and other features defined on “child” component studies like this can later be imported to the top level assembly using Import Study Features, described in more detail in Example 2 of this article.

These mesh controls can later be refined further for additional accuracy in prediction of local stresses. I would generally recommend waiting on any additional refinement until a baseline or “first pass” analysis is performed on the top level assembly to verify that the study setup is correct.

Mixing Mesh Quality

For solid mesh studies such as this one, SOLIDWORKS 2020 added the capability of mixed mesh quality.

Before this enhancement, it was necessary to choose on a global level between draft quality and high quality mesh. Draft quality mesh uses linear tetrahedrals that have many fewer nodes and degrees of freedom than high quality mesh, resulting in faster solution times with the tradeoff that it tends to underpredict stresses and displacements.

The global choice meant that draft quality was generally reserved exclusively for validating study setup on a crude first pass analysis.

Now that high quality mesh can be applied selectively to areas of interest, there is the possibility of carefully incorporating draft quality into regions that are sufficiently distant from the area of interest.  The two mesh qualities are color coded by default, and visible in Figure 4 below.

Figure 4. Completed Setup for First Pass Analysis.

Note that the presence of any shell or beam elements will remove the mixed mesh quality capability.  Care must still be exercised to ensure that the mesh refinement is adequate.

This study resulted in 1.5 million degrees of freedom and solved in under 30 minutes on an entry level workstation laptop. The results for stress and displacement, shown at an exaggerated deformation scale, are visible in Figure 5 below.

Figure 5. First Pass Results for Stress and Displacement.

The utilization of contact interactions between the mold halves is what is likely responsible for the solve time being as long as it is, but the 1.5 million degrees of freedom total leaves plenty of headroom for additional mesh refinement or reintroducing more high quality mesh later on.

The exaggerated deformation presented is useful to verify the loading setup conditions. In this case, it can be seen that the load and fixture scheme employed is probably not accurately representing the real life loading inside the injection mold machine.

This is because in reality the mold assembly will be squeezed between large and extremely stiff platens, which would greatly restrict the ability of the base plates to deform.  A more realistic analysis could be performed by using a new restraint scheme, or by modeling rigid bodies to represent the molding machine platens and squeezing the mold assembly between those.

Setup problems such as this can be more quickly determined using a “first pass” analysis rather than waiting hours for a very refined mesh study to solve. In fact, it probably could have been identified by running a globally bonded study, which would have solved in only a few minutes.

Example 2: Gantry Shell Mesh Analysis

Consider the example of the gantry crane pictured in Figure 6 below. While not inherently necessary for such an application, this model was purpose built with simulation in mind.

Figure 6. Case Study – Gantry Analysis.

In the case of the truss, geometry like this would often be represented as weldments in SOLIDWORKS, which would automatically convert into beam elements in the simulation. However, in this case, the truss was modeled using surface bodies, which will automatically convert into shell mesh.

The shell mesh provides greater detail and prediction of local stress concentrations than would be possible using a beam mesh. It also enables the use of contact interactions between the trolley, which will slide along the frame. Contact is also defined on the rollers at either end of the gantry. The remaining geometries such as the trolley and end rails were meshed with the default solid mesh. A Remote Load/Mass is used to represent the weight of the payload. These are useful to represent the effects of excluded components or other cantilevered loadings.

Simplification such as shell mesh definition requires additional setup compared to running an exclusively solid mesh study. Shell thickness, offset and orientation must be defined for the relevant surface bodies, and frequently it is necessary to manually define local contact interactions.

This process is expedited by using the Import Study Features command, which was added in SOLIDWORKS 2018 and is visible in Figure 7 below.

Figure 7. Import Study Features.

Import Study Features allows defining the simulation setup on a study of a child component, and then importing this setup up to the top level. Features to import, such as material/shell definition, mesh controls, loads and fixtures, can be selectively filtered.

Perhaps the most useful feature is “Propagate … to all instances” which will automatically pattern the imported features to the relevant component instances in the assembly.

Import Study Features also allows for rapid re-use of components which may need to be analyzed in different top level assemblies.

The heavy use of shell mesh on this study and the limited contact areas allowed it to solve quickly. It was easy to test alternate configurations with the trolley at various distances along the gantry.

Figure 8. Gantry Analysis Results.

The results of the analysis with an off-center trolley are depicted in Figure 8 above. The analysis totaled 850k degrees of freedom and solved in just a few minutes.

Productivity Shortcuts & Simulation API

Setting up simulations on larger projects often involves repetition of monotonous tasks such as defining many loads and fixtures. SOLIDWORKS Simulation allows for keyboard shortcuts, mouse gestures and shortcut bar customization for simulation to help speed up the process.

Pinning contact and connector menus so they remain persistent on the screen is another way to save time. Outside of the “Import Study Features” mentioned earlier, there are limited means to pattern loads or connectors.

One solution is to use the SOLIDWORKS Simulation API. The macro recorder is capable of recording simulation actions and outputting a VBA macro with the appropriate API calls. These can form the basis for automation to quickly generate simulation setups and perform detailed results post-processing.

Figure 9 below shows an example VBA macro integration with Microsoft Excel, which coordinates with SOLIDWORKS Simulation to setup and run a study and then extract the results.

Figure 9. Microsoft Excel Simulation API Example.

A variety of useful downloadable Simulation API examples are posted in a SOLIDWORKS blog article.

Simulation 2021 Enhancements

The examples portrayed throughout this article took advantage of a number of the performance enhancements in SOLIDWORKS 2021.

Performance Enhancements

The Blended Curvature Based mesher was rearchitected for the 2021 version, and now produces much better aspect ratios, as well as generating large meshes very efficiently. In SOLIDWORKS Simulation Professional and higher, the BCB mesher is multi-threaded very well. 

When meshing large assemblies, the 12-thread CPU in my laptop frequently maintained 100% utilization, as depicted in Figure 10 below, and the mesh generated much faster than in previous versions. 

Figure 10. BCB Mesher Multi-threading in Simulation Professional 2021.

There’s a similar story in terms of solver performance. The FFEPlus solver has substantially improved performance in 2021, primarily due to improvements in multithreading, as visible in Figure 11 below.

Performance increases have also extended to the Intel Direct Sparse solver and results post-processing which can both manage much larger data sets effectively.

Figure 11. FFEPlus Solver Performance in 2021. (Image from SOLIDWORKS Help Files.)

One of the great things about SOLIDWORKS Simulation is that even the base simulation packages are able to analyze large problems effectively – there are no hard restrictions on problem size in terms of components or node/element count.

Performance by Package Level

Up until 2021, all versions of SOLIDWORKS Simulation also offered similar performance in terms of mesh and solve time. With the 2021 version and the substantial rearchitecting of the meshers and solvers, for the first time there is a difference in performance gap between the different packages.

SOLIDWORKS Premium and the SOLIDWORKS Simulation Standard are limited to single-core meshing for the new Blended Curvature Based mesher. The solvers for SOLIDWORKS Premium and Simulation Standard are limited to 8 cores / 16 threads – admittedly still a generous limit that is unlikely to be bumped into on a run-of-the-mill system today.

SOLIDWORKS Simulation Professional and higher packages offer unrestricted multi-threading for both meshing and solving. With the advent of affordable many-core CPUs, this distinction will mean better quality of life for performing large assembly analysis with the higher level simulation packages in the future.

Interface Changes

Figure 12. New Settings for Mesh & Contact in 2021.

Interface changes also made their way into Simulation 2021. In the context of large assemblies, one of the most useful options is the ability to quickly toggle all part definitions to solid mesh, as visible in the left of Figure 12 above. This is a great diagnostic tool or fallback to troubleshoot faulty beam or shell conversion, or for cases where the additional detail of solid mesh is required.

Weldments can also then be batch converted to beams, and sheet metal parts to shells.

In the Simulation options, there are many more contact settings exposed that were previously inaccessible to the user – including a gap range for global bonding which can be adjusted to automatically bond over small gaps.

A new feature is stabilization for contact areas. This is said to produce much more accurate stress distributions for certain contact problems, as illustrated in the right of Figure 12 above.

For more detailed information on the Simulation 2021 enhancements, consider taking a look at these SOLIDWORKS Help files.

For an additional resource, consider viewing the associated live presentation this article was based on, which explores shortcuts and the setup process of these analyses.

Conclusion

This article examined two case studies of large assembly analysis in SOLIDWORKS Simulation, discussing the planning process as well as a number of useful simplification and setup techniques.

Enhancements to SOLIDWORKS Simulation for 2021 and recent years have greatly improved the viability of setting up large simulation studies.

Additional resources were presented to learn more about What’s New in 2021 and the Simulation API.

Check out the whitepaper Design Through Analysis: Simulation-Driven Design Speeds System Level Design and Transition to Manufacturing to learn more.