Overview:
In engineering and manufacturing, the durability of parts is a critical factor that directly influences the safety, performance, reliability, and cost-effectiveness of products. Determining how long a component can function under specific conditions without failure is essential for ensuring product longevity, minimizing maintenance, and preventing unexpected breakdowns. Using software such as Altair’s MotionView and Motionsolve, engineers can incorporate linear flexible bodies generated from OptiStruct to accurately determine the stresses and strain of the parts before yield. To accurately determine the stresses and strain of the part that overcomes yield. A co-simulation between MotionSolve and OptiStruct can be simulated to include non-linearity of the part. This article dives into the multi body dynamics and finite element setup of viewing the stresses and strain of lower control arm going beyond yield.
Release Version:
MotionView (2025 or newer)
MotionSolve (2025 or newer)
OptiStruct (2025 or newer)
Model Files
- MS_OS_FV_BUMP.zip (See attachments)
- Tire property file with cam contact ('fiala_tire_with_cam_contact.tpf') for bump simulation, any other suitable tire property files can be used
- Road property file with bump profile (Road_bump_OS.rdf)
- OptiStruct lower control arm fem file (LCA.fem)
- FE mesh model of lower control arm
- Initial velocity set as '-5000' (to be consistent with the MS model, when Co-Simulation starts)
- Dummy high stiff CBEAM to represent Vehicle Body (to accommodate bushing)
- Lower control arm bushing.
- MotionSolve_OptiStruct_Overview.docx: Documentation on setting up the MotionView model and running co-simulation
IMPORTANT Guidelines and Best Practices
- Add an Environmental Variable 'HW_MV_EXPERIMENTAL' with Value as 'OSFLEX' in the operating system.
Figure 1: Environment Variable Needed For Co simulation
- Only one OptiStruct instance can simulate with a MotionSolve instance. However, multiple OptiStruct flexible bodies can be used in the single instance
- Connections between MotionSolve and OptiStruct are accomplished using interface nodes
- The connection type of an interface node is always a spherical joint, meaning only translational displacements and forces are communicated between the two solvers. With a combination of spherical joints, it is possible to model other joints configurations
- To model a Fix Joint: Three spherical joints are needed in the MotionView model. In the OptiStruct model, the interface nodes cannot all be collinear. At least one interface node needs to be offset.
- To model a Revolute Joint: Two spherical Joints are needed in the MotionView model. In the OptiStruct model, the interface nodes are collinear.
- To model a Spherical Joint: One Spherical Joint is needed in the MotionView model
- To connect multiple spherical joints to the OptiStruct model, a CBEAM needs to be created that attaches to the interface nodes.
- When connecting several spherical joints with the OptiStruct system, those cannot be subject to a hard constraint on the OptiStruct side. In other words, they cannot be tied together to the same RBE2 or similar entities.
- Any MotionSolve body that is directly connected to a body in OptiStruct should have significant mass and inertia to avoid numerical instabilities. Conversely, this restriction is not required
- Compliant elements, such as springs, forces, bushings, and so on, that are connected or applied to the OptiStruct body must be defined in OptiStruct. For example, if a bushing acts between a body in MotionSolve and a body in OptiStruct, then the bushing should be modeled in OptiStruct between the interface node and the OptiStruct body. Alternatively, introduce a dummy body between MotionSolve force entity and OptiStruct body, this dummy body may introduce some numerical instabilities
- The global frame between MotionSolve and OptiStruct needs to coincide, the gravitational force needs to act in the same direction, and the Length, Force and Time units must match
- Unless the analysis type for MotionSolve is Static/Quasi-Static. It is highly suggested not to have the co-simulation start at the beginning of the MotionSolve Run (Example Time = 0.00 seconds). Initial settling can occur in the MotionSolve model that causes the misalignment between the MS and OS model that can cause numerical instability.
- The communication interval is based on the solver step size dictated by Maximum Step Size (h_max) in MotionSolve and Maximum Step Size (DTMAX).
Understanding the Model Definition in OptiStruct
The model setup assumes some familiarity with OptiStruct. An OptiStruct ready model called LCA.fem is available for reference.
Figure 2: Lower Control Arm In HyperMesh
A quick overview of the model. The lower control arm geometry is meshed and organized in the “PSHELL_1” component. The material properties are set to an elasto-plastic material with a yield stress of 300 MPa. The plastic properties are defined by “loadcol_1”.
Figure 3: PSHELL References
Figure 4: Plastic Properties Curve
To constrain the lower control arm to the vehicle body. A CBEAM was created with relatively high stiffness.
Figure 5: CBEAM Reference
Three RBE2 elements were created to connect the MotionView model to the flexible body. In addition, the vehicle will be running at a constant velocity of 5000 mm/s. An initial velocity (TIC) of -5000 mm/s is applied to the model.
Figure 6: RBE2 and TIC Reference
In the MotionView model the lower control arm is attached to the vehicle via bushings. Referring to the Guidelines and Best Practices. For co-simulation, it is preferred to model the bushings in the OptiStruct model to avoid numerical instability.
Figure 7: PBUSH Reference
Figure 8: PBUSH Values
Figure 9: References
Setup Procedure for the MotionView Model And Co - Simulation
The following procedure has been recorded, please refer to the YouTube here:
The Tutorial steps are outlined in MotionSolve_OptiStruct_Overview.docx
Results
After running the co-simulation, the stresses on the nonlinear flexbody can be observed in HyperView.
Figure 10: Linear Flexbody Results
Figure 11: Nonlinear Flexbody Results
Conclusion
In conclusion, analyzing a nonlinear flexible body offers crucial insights into how complex systems behave under real-world conditions. By capturing the effects of large deformations, material nonlinearities, and dynamic interactions, such analysis enhances design accuracy, safety, and performance. It allows engineers to optimize structures more efficiently, reduce unnecessary material use, and predict potential failure points early in the design process. Ultimately, incorporating nonlinear flexibility into simulations leads to more reliable, cost-effective, and high-performing products across a wide range of industries.
Authors
Christopher Fadanelli, Senior Solution Engineer – System Integration
Ananth Kamath Kota, Global Technical Manager – Systems Integration
