SIMULIA

Debugging Abaqus Models

Thu, 12 Dec 2024 08:00:00 GMT

The following blog was authored by Ritu Singh, a mechanical engineer from Auburn University, Alabama, with six years of experience. She excelled as a senior design engineer for three years before transitioning to a writer and team lead for three years, specializing in creating accessible content. Currently, Ritu serves as an Advocacy Offer Marketing Specialist in Global Marketing at Dassault Systèmes for the SIMULIA brand, where she combines her engineering acumen with her writing skills to craft compelling marketing content. Introduction Debugging Abaqus/Standard models can be complex, especially when confronting convergence problems in structural simulation. This blog focuses on debugging Abaqus models, which refers to fixing convergence problems in Abaqus/Standard. Debugging can refer to a range of things, from building and fixing problems in a mesh to correcting basic modeling mistakes, misspelled keywords, and more. However, this blog aims to learn how to fix convergence problems in Abaqus/ Standard. FAQs Q: How can I find examples that use a certain feature in Abaqus to familiarize myself with its usage? A: You can search the online documentation or use the Abaqus findkeyword utility to find examples that use a certain feature. The input files associated with these examples are provided as part of the Abaqus installation, which you can fetch using the Abaqus fetch utility. Q: What is the Abaqus Verification Guide, and how can it help me learn to use a new capability? A: The Abaqus Verification Guide contains test cases that prove that implementing the numerical model produces the expected results for one or several well-defined options in the code. Running these problems when learning to use a new capability can help ensure you use it correctly. Q: What is the Job Diagnostics tool in Abaqus/CAE, and how can it help me debug my model? A: The Job Diagnostics tool in Abaqus/CAE allows you to monitor the progress of your analysis job and understand the convergence behavior of your job. It provides detailed information about each step, increment, attempt, and iteration of the analysis, which can help you identify and correct issues with your model. Q: What is the difference between average force and time average force in the Residuals tab of the Job Diagnostics dialog box? A: The average force is the force applied to the model at a given time step, while the time average force is the average value of the force over the entire analysis. The Residuals tab of the Job Diagnostics dialog box displays the values of both quantities for each iteration, which can help you identify the cause of convergence issues. Q: What is the Getting Started with Abaqus plug-in, and how can it help me run Abaqus examples? A: The Getting Started with Abaqus plug-in is a tool that allows you to run the examples described in the Abaqus documentation. It creates a model and a job for each example, which you can submit for analysis in the Job module and view the results in the Visualization module. The plug-in also fetches the input files associated with the examples and places them in the current directory. Understanding Convergence in Abaqus/Standard vs. Abaqus/Explicit Abaqus/Standard is the original Abaqus solver code, dating back to the early 1980s. It is a finite element solver code, also known as an implicit solver, with many capabilities. These range from general nonlinear static and dynamic simulations to linear simulations, including linear dynamics, heat transfer, acoustics, piezoelectric effect, and more. Abaqus/Standard uses an incremental, iterative approach for general simulations. It is built around the Newton-Raphson method, a numerical technique used to target convergence issues, requiring a comprehensive debugging strategy. This method’s successful completion results in so-called ‘convergence,’ while its failure leads to non-convergence. It is crucial to distinguish between these two states to address non-convergence effectively. In contrast, Abaqus/Explicit is a dynamic explicit package released around 1992. It is an explicit solver that operates on a fundamentally different solver technology. Abaqus/Explicit has various capabilities such as general nonlinear dynamic simulations, heat transfer, and acoustics coupled with structural, large deformation methods and robust contact algorithms suitable for complicated 3D contact models. A dynamic explicit analysis package, Abaqus/Explicit, does not use the Newton-Raphson method and, therefore, does not have convergence issues. However, explicit codes can face numerical stability concerns. Users facing severe convergence problems in Abaqus/Standard can consider switching to Abaqus/Explicit. Since the interface for both the solvers is notably similar, transitioning to Abaqus/Explicit can help mitigate convergence challenges encountered in Abaqus/Standard simulations. Example: Connector Spring The first example involves a one-element model with one connector element to which a force is applied. A nonlinear spring stiffness balances the force. The connector element is a Cartesian-Cardan connector. Its first component of relative motion has a nonlinear stiffness, while the other components of relative motion are constrained. Since the spring is nonlinear in one direction, this model is relatively straightforward and uses a static load step. This means we are going to test how far the spring stretches under the load. It is crucial to identify the critical model features when debugging a convergence issue: Connector element with a nonlinear stiffness Boundary conditions, including connector motion constraints Concentrated loads Static procedure. We must understand the features in the model even if debugging is not required. Understanding how to use the model features is as crucial as understanding the problems they can cause such as, Nonlinear springs may have non-monotonic force/deflection behavior Multiple constraints might interfere with each other. Follower loads may cause the need for the unsymmetric solver. The simulated process may be quasi-static, causing the static analysis’s failure. Knowledge of potential pitfalls is developed through both training and experience. This is true for almost any complicated human endeavor. Through training, one can circumvent relying solely on experiential learning while enhancing one’s ability to identify and address challenges effectively. In the following example, the model fails to complete as-is. The first thing to do is look at the status file. (You may prefer to use Job Diagnostic in Abaqus/Viewer, but I prefer text files.) The green text indicates a convergence problem. My log file contained an error code message, but these are lower-level, system-related problems that I would need to investigate separately. Here, we are facing a run-of-the-mill convergence problem. Once we have identified the issue of the analysis abruptly terminating, we must examine the message file. I prefer to first inspect the end of the file. I like to do this while I have the ODB open in Abaqus/Viewer with the deformed shape of the last saved result displayed. In this case, the message indicates that the required time is less than the minimum specified, which is a generic message. Often, error messages reiterate what’s already known. When I review the message file, I typically have a picture displayed of the model’s deformed shape just before the error occurred. However, since this is a single-element model, there’s not much to visualize. Now that I know the excessive cutbacks caused the error, I can backtrack through the message file, noting the critical nodes and elements and locating them in the deformed mesh. I need to identify patterns in the numbers so I ask questions to myself, such as: Does the same group of nodes consistently have the largest residuals? Does the same group of nodes consistently cause problems with the contact? Are the largest corrections at the same few nodes? Is the plasticity seemingly out of control in the same group of elements? Etc. The number patterns can help you identify the region of the mesh that is causing the problem. You can quickly locate these entities within the displayed mesh. Now, with the job interrupted abruptly; hopefully, you have some intermediate results saved. You must formulate a hypothesis to mitigate the issue. This hypothesis must align with the identified problematic mesh region and potential issues inherent to the model’s features. You must scrutinize known results through animations or contour plots of stress and displacement to refine this hypothesis. With a working hypothesis, the next step involves modifying the model to address the hypothetical problem. With luck, once you implement the fix, the issue will be resolved. However, if the problem persists or new complications arise, an incorrect hypothesis could be the cause. In such scenarios, especially when dealing with convergence problems, it is crucial to practice perseverance. In this case, the problems are observed at node two. This is expected as out of the two nodes, this is the only free-moving node. The mesh is in equilibrium, but there is a problem finding another equilibrium state with a slightly larger load. This leads me to hypothesize that there is something odd about the nonlinear stiffness. To gain further insight, we would need to implement a technique promoted in training: displacement-controlled loading. Instead of applying a load, we can stretch the spring with an applied boundary condition and observe the results. This model has simple force-controlled loading, which can be easily converted to displacement control. By applying a fixed displacement, we can modify the model and successfully complete the analysis. The force versus displacement plot shows that the non-monotonic force-deflection behavior hinders force ramping in a static procedure. This clearly exposes the problem that there is no equilibrium state close to the equilibrium state when the load is around 2.0. This behavior stems from the default amplitude setting in Abaqus static simulations, complicating force application. There are a couple of solutions that can be considered to address this problem: Interpolating a displacement corresponding to a load of 2.0 and rerun. Run a two-step simulation and switch to force control as shown below. Use the relatively new *STEP CONTROL option. This example showcases the broader complexities of nonlinear simulation debugging, highlighting the need for a methodical approach to identifying and resolving convergence problems. Example: Plate Through Ring The second example illustrates a convergence issue frequently encountered in finite element analysis using a thin elastic disk pulled axially through a rigid ring with an elliptical cross-section. The disk is supposed to be pulled entirely through, but the simulation fails, leading to the dreaded message indicating that the analysis has not been completed. This example highlights a common frustration due to the convergence problem during such simulations. Let us view the load step that I created. The step already uses displacement-controlled loading so there is no hope of solving the problem by switching to it. The important model features include: Quadratic brick element type C3D20RH Hyperelastic material General Contact Boundary Conditions Rigid body constraint Static procedure Once we have identified the model’s key features, the next step is to identify the pitfalls and understand how to use these features to produce a quality result. Understanding stability in the context of hyperelastic materials before using them in a model is vital since hyperelastic materials should be stable in the range of expected strain. We may encounter issues with contact. For example, we may need to activate the unsymmetric solver when faced with a convergence problem with the contact model in Abaqus/Standard. Contact may need the unsymmetric solver, especially if there is friction. We must avoid over-constraints and watch out for a conflict with the static procedure when simulating a quasi-static process like this one. The model makes it only partway through the step, prompting the message indicating the analysis has not been completed. There are numerous negative eigenvalue messages in this message file. Based on the residuals and the time average force, it is evident that the model is in an acceptable equilibrium state. Let us formulate a reasonable working hypothesis at this stage. We are using contact best practices. We have general contact, and the unsymmetric solver is activated due to friction. The hyperelastic material is stable. Because of their positions, there is no possibility of over-constraints. Numerous persistent negative eigenvalue messages exist. This, together with the animation of the partial results, leads to a hypothesis of buckling. We need a solution strategy to continue the post-buckling behavior and pull the disk through completely. Various techniques, such as the Riks method, static stabilization, quasi-static implicit dynamics, and explicit dynamics could help us resolve this problem. Let us switch from static procedure to quasi-static implicit dynamics in Abaqus/Standard. We allow for a very small increment size and increase the number of cutbacks. In some cases where the simulation moves along smoothly with a reasonably large increment size but buckling behavior is observed, we must transition to a small increment size. Sometimes, it may take a minimal increment and more than five cutbacks, the default number. When conducting implicit dynamics, it is crucial to consider time as physical and not a normalized quantity like in static analyses. The solution to this convergence issue lies in modifying the simulation procedure. The problematic region of the curve is navigated, allowing the simulation to be completed successfully. This example highlights the importance of understanding the simulation’s specific characteristics and applying tailored strategies to address convergence issues in complex finite element analyses. Example: O-Ring Compression and Relaxation The final example is a hyperelastic/viscoelastic O-ring being compressed and then relaxed. The green circular component in the image above represents the O-ring. In a static step, the rigid plate compresses the O-ring into a groove in an elastic material. The plate is held fixed while the seal relaxes in a second step using the *VISCO procedure. This model features include general contact, boundary conditions, and symmetry planes. When the analysis was run, the first step was not completed. The debugging process involves thoroughly examining partial results, animations, and the message file to identify the source of the problem. The message file indicates that while the equilibrium is good, there are problems with contact. Note the messages about sticking and slipping. The working hypothesis is that the O-ring is experiencing stick-slip behavior, which causes problems with the static procedure. A workaround is to use quasi-static implicit dynamics. In this case, switching the procedure makes things worse, which can happen. The message file indicates a contact problem with edge-to-face contact at nodes 4 and 4559, which are at the sharp edge of the groove. Let us view the edges that are in the general contact. We can visualize GENERAL_CONTACT_EDGES_3 in the contact domain using Abaqus/Viewer. We notice that there are unwanted edges on the symmetry boundaries. There are options in general contact in Abaqus/Standard to remove edges from the contact domain. Let us remove those and try again. Once the whole model is running, we can consider reverting to a static procedure. Making one change at a time works best so the procedure is not changed. We are changing the contact to eliminate the edges on the symmetry plane and switch the first step to a dynamic procedure. This gives me physical time and a viscoelastic effect. It also offers us an inertial effect. This means we must pay close attention to the time for this step. I am using a time of 0.1 for that step and a relaxation time of 30 seconds. Since the rate of loading for this small O-ring isn’t long compared to the relaxation time, 0.1 seems like a good time to use for that step. Although step 1 is successful, the simulation fails yet again. We get past the compression step and into the VISCO step, but then it fails. By analyzing the partial results, animations, and the last saved result in step two, a deformation pattern is observed in the reduced integration mesh. A plot of the seal’s deformed shape indicated the hourglassing of the C3D8RH elements. This is where perseverance is required. We can eliminate the reduced integration elements and put in fully integrated elements to eliminate the hourglassing effect. The next step is to switch the brick element to C3D8H and try again. Rerunning the simulation offers a complete result. The solution is now successful. We can work on model refinements at our leisure. I decided to refine the mesh and round the edge of the groove. Often, convergence is more accessible to obtain when the edge is rounded. The radius of the round should be large enough to allow the mesh to conform to it. If you need a sharper edge, use a more refined mesh. Once we implement these changes, the simulation is successful. This example has demonstrated the importance of persistence and adaptability in resolving convergence challenges. General Debugging Techniques and Strategies for Finite Element Models Debugging Abaqus/Standard convergence issues can be daunting. A checklist is crucial to identifying and resolving these challenges in your model. Here are the key steps to keep in mind to effectively debug a model in Abaqus/Standard: Know your model features and how to use them properly. Identify the potential pitfalls that your model features can cause. Apply all available information to form a hypothesis.Partial results are beneficial. Remember not to artificially limit the output while debugging. Read the error/warning messages and analyze the message file. Define a workaround for the hypothetical problem. It isn’t uncommon for initial attempts to fail. Perseverance is the key to completing the analysis. The last thing to remember is that through training and experience, one can understand the pitfalls of specific features. Training and experience allow users to sharpen their ability to hypothesize and implement practical solutions for convergence issues. Here is a list of recommended training classes and resources for further learning. Obtaining a Convergence Solution with Abaqus Modeling Contact and Resolving Convergence Issues with Abaqus Abaqus/Explicit: Advanced Topics Buckling, Post Buckling, and Collapse Analysis with Abaqus Any training class is beneficial. These educational resources are available on the SIMULIA website. I encourage you to explore these training opportunities if you are looking to enhance your problem-solving capabilities in debugging convergence issues with Abaqus/Standard. Conclusion In conclusion, debugging convergence issues in Abaqus/Standard is an intricate process that requires a deep understanding of the model’s features and potential problems. Training and experience assist in accurate hypothesis formulation to implement successful solutions. The Newton-Raphson method is central to the solver, and when non-convergence occurs, a systematic approach is employed to diagnose and remedy the issues. Partial results, error messages, and animations are invaluable in this process and guide modifications to achieve successful outcomes. Persistence is required as initial attempts may only sometimes resolve the issues. Eventually, a systematic and knowledgeable approach, backed by perseverance, is pivotal to mastering the debugging of finite element models in Abaqus/Standard. To learn more about mastering debugging in Abaqus/Standard, we invite you to access our recorded session here. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

Optimizing Battery Range and Thermal Comfort in Electric Vehicles

Thu, 05 Dec 2024 08:00:00 GMT

Introduction The electric vehicle (EV) industry is making great strides towards sustainable mobility, pushing the boundaries of what’s possible with clean energy. Although EV sales currently account for around 16% of the global market, they’re expected to rise sharply to 50% by the end of 2035 (see figure 1) as manufacturers work to overcome significant challenges like manufacturing challenges such as material availability for battery and electric components, as well as availability of charging infrastructure, to vehicle thermal challenges such as battery range and thermal comfort, cost of EVs to be on par with ICE vehicles, model proliferation, multi-physics engineering development, range anxiety etc. Among the most pressing of these are battery efficiency and occupant comfort, particularly under varying climatic conditions. Figure 1: Global EV sales forecastSource: https://ev-volumes.com/news/ev/evs-forecast-to-account-for-two-thirds-of-global-light-vehicle-sales-in-2035 In colder climates, for example, EVs lack the waste heat from internal combustion engines that would otherwise help heat the cabin. This leads to increased power consumption by climate systems, which in turn reduces battery range. This blog explores how Dassault Systèmes employs cutting-edge simulation technologies and advanced computational tools such as Computational Fluid Dynamics (CFD) and 1D system modeling to accurately simulate and optimize these complex interactions and thereby improving both battery efficiency and cabin comfort in EVs. Motivation: Why Thermal Management is Key for Electric Vehicles Thermal management directly impacts an EV’s performance, as it influences both the efficiency of the battery and the comfort of passengers. In comparison to ICE vehicles, EVs must expend additional energy to heat the cabin, which can reduce range by more than 15% in hot or cold conditions and the range can drop by up to 40% in extreme weather conditions (see Figure 2). Figure 2: Winter range for popular EV modelsSource: recurrentauto.com Thermal comfort is particularly relevant to drivers in extreme climates who rely on climate control features like seat warmers, cabin heaters, and defrosters. These features consume a significant portion of the EV’s battery power, creating a trade-off between energy used for passenger comfort and energy available for range. Challenges in the EV Thermal Management Landscape Real-world applications come with their own set of challenges. Extreme temperatures, complex thermal interactions, and fluctuating driving conditions all impact energy consumption in ways that require ongoing refinement of EV designs. For instance, urban stop-and-go traffic cycles and high-speed highway driving affect airflow and cooling needs differently, meaning that a single HVAC configuration is unlikely to suit every scenario. Beyond comfort, EV designers also face the task of balancing battery health and efficiency. Batteries perform optimally within a specific temperature range. Excessive heating or cooling can accelerate degradation, affecting long-term performance and lifespan. Advanced simulations like those used in this study help identify the optimal trade-offs between battery protection and energy efficiency. The Role of Advanced Simulation: To tackle this challenge, Dassault Systèmes has leveraged a co-simulation approach that integrates detailed 3D CFD models with system-level models. This approach allows engineers to simulate how heat moves through the vehicle and how energy is used by the climate system, helping to optimize both comfort and efficiency. Methodology: A Multiscale Approach for Better Range and Comfort A study conducted by Tesla shows that in electric vehicles, optimizing one of the components individually results in 15-25% improvement in e-drive efficiency, whereas optimizing the overall system as a whole improves the e-drive efficiency by 40%. Range is a problem, which should not be looked at through a single component in the system, but as a vehicle overall. An advanced virtual twin can effectively assist in determining the optimal size of the HVAC system while enabling early-stage predictions for battery life, vehicle range, and passenger comfort. This study utilizes a co-simulation approach combining system-level and 3D CFD models i.e., by merging the results from 3D thermal optimization into overall system to optimize the efficiency to capture complex, multi-scale interactions and enhance overall vehicle performance. Through the integration of 3D CFD with Finite Element Analysis (FEA) thermal models, this approach provides precise predictions of passenger comfort levels and battery temperature distribution. Furthermore, by incorporating Dymola system behavior models, real-world driving scenarios for all vehicle systems can be simulated. 1D system simulation is performed with Dymola and the heat exchanger inlet temperatures are determined and provided as input to the 3D CFD simulation. As a next step, 3D CFD simulation is performed with PowerFLOW / PowerTHERM and the cabin outlet temperature is provided back to the 1D system model as input and the cycle repeats (see Figure 3). This approach benefits from the detailed response trends provided by 3D CFD analysis, facilitating quick adjustments via 1D models to optimize vehicle performance. Figure 3: Coupled 3D CFD – 1D system Model simulation process Additional 3D CFD analyses assess Underhood airflow, allowing engineers to characterize how external air affects the HVAC heat exchangers under various conditions. This airflow data is then applied to the 1D HVAC system analysis to establish realistic boundary conditions. Figure 4: Coupled 3D CFD – 1D system Model simulation System Model The first step is creating a 1D model of the HVAC system using Dymola, which assesses energy consumption, cabin temperatures, and vehicle range under different drive cycles, vehicle aero changes and HVAC modes. This model helps determine the size and power needs of the HVAC system to balance thermal comfort with battery efficiency. Dymola Modelica library offers a wide variety of predefined models and libraries that make our life easier in modelling the system models, like… Realistic drive cycles for various speeds (for e.g., high and low WLTP drive cycles) Battery library to model range, ageing, time to charge and cooling HVAC library to model driving modes, flow rates and thermal exchange Driveline and Chassis to model aerodynamic properties of vehicle Figure 5: 1D system Model of an EV 3D CFD for Localized Thermal Comfort Using CFD simulations, one can analyze how heat moves through the cabin, affecting each passenger’s thermal sensation alongside the temperature of electronic components like display monitors, mobile rest etc. This level of detail provides a realistic view of representation of different modes for different climatic conditions and comfort across different body areas and helps inform design decisions for optimal airflow and heating distribution. Figure 6: 3D CFD Cabin simulation of an EV Underhood Cooling Airflow Analysis A separate 3D CFD model simulates airflow around the vehicle’s heat exchangers, which are part of the HVAC system. This analysis captures how external air impacts cooling and heating, allowing for realistic boundary conditions and ensuring that all HVAC components operate efficiently. The initial step involves using detailed 3D CFD analysis to characterize the external airflow that reaches the front end of the HVAC system’s heat exchangers under various vehicle operating conditions. A drive-cycle-specific Design of Experiments (DoE) approach is applied to select sample points that comprehensively represent these conditions based on their frequency of occurrence. This process, illustrated in Figure 7, defines the entire approach for characterizing airflow beneath the hood. Figure 7: Underhood cooling airflow characterization Next, CFD simulations are conducted for each sample point to determine the heat exchanger’s inlet mass flow rate and back pressure. A response surface model is then constructed using 2D linear interpolation to estimate values between these sample points. This model provides realistic boundary conditions for the 1D HVAC system analysis, allowing further simulations with accurate inputs for the heat exchangers. Real-World Application: Analyzing Drive Cycles and Compressor speeds for Optimal Efficiency and Comfort A transient coupled 1D-3D simulation was conducted on a compact passenger EV. This vehicle features a battery pack of 384 prismatic cells with a total capacity of 15.6 kWh. The HVAC system is designed to cool the cabin in summer and serve as a heat pump during winter. For this analysis, the focus was on a cold-weather scenario, simulating a drive in -10°C ambient temperatures for 30 minutes physical time, driver and passenger human comfort model and 60% face, 40% foot HVAC flow split mode. The Worldwide Harmonized Light Vehicles Test Procedure (WLTP) drive cycles were used, as it reflects typical urban and highway driving patterns globally. The simulations explored two different drive cycle speeds, a regular drive cycle and an additional low-speed WLTP cycle to represent city driving, allows for realistic evaluation of the HVAC system under variable conditions. Three different compressor speeds high, medium and low were analyzed in the study, with particular attention on the HVAC system’s energy consumption, as it directly impacts passenger comfort. Additionally, the expected range for each configuration was estimated by analyzing the battery’s state of charge at both the start and end of the drive cycle. Figure 8: Regular and low-speed WLTP drive cycles Results The thermal comfort levels achieved are comparable across all three scenarios. After 10 minutes, occupants feel comfortable in each case. The high compressor speed scenario reaches comfort level 0 in 4.5 minutes, the medium speed in 6 minutes, and the low speed in 6.5 minutes. After 10 minutes, the low-power scenario offers the same level of comfort as the high-power scenario while consuming 50% less energy. Further analysis indicates that overall comfort is primarily influenced by the comfort level of the body’s breathing sensation. This breathing sensation is less affected by design variations among the three speeds compared to other body parts, resulting in a smaller-than-expected overall change in comfort. Figure 9: (a) Overall comfort for different compressor speeds Medium and high compressor speeds consume 33.5% and 50.2% more energy compared to low speed. Moreover, at low compressor speeds, the battery drained more slowly, providing a range increase of up to 21% under some drive conditions. This test showed that reducing HVAC power can significantly enhance range without sacrificing passenger comfort. Figure 10: (a) Energy savings (b) Range difference High Speed: Achieves maximum comfort quickly but consumes more energy. Medium Speed: Balances comfort and energy efficiency. Low Speed: Consumes the least energy, with only a slight delay in achieving optimal comfort. Conclusion: Paving the Way for Smarter EV Design As electric vehicles become more prominent, tools like co-simulation are essential in crafting a user-friendly and competitive product. By blending 3D CFD with 1D system modeling, manufacturers can optimize a vehicle’s thermal performance and ensure it meets consumer expectations for both range and comfort. Together, these simulations allow engineers to fine-tune vehicle parameters, such as compressor speed, in response to different driving cycles. For instance, reducing the compressor speed in the HVAC system can lead to significant energy savings without greatly impacting comfort levels. This holistic approach promises a range of benefits: Improved Range: Strategic HVAC adjustments can preserve battery life and extend driving range, reducing range anxiety. Enhanced Comfort: Precision simulations ensure that passengers enjoy a comfortable cabin experience, even in extreme climates. Energy Efficiency: Optimized HVAC systems lead to lower power consumption, helping to meet energy targets. As simulation technology advances, EV designers are increasingly able to predict real-world outcomes in a virtual environment. By adopting these methods, the automotive industry is poised to make electric vehicles not only a viable alternative to traditional cars but a preferred choice for eco-conscious drivers worldwide. The workflow presented here also exemplifies Dassault Systèmes’ approach to MODSIM, integrated modeling and simulation and supports the company’s long-term strategy to bridge the gap between designers and simulation engineers, ultimately speeding up the product development process. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

Build a Better Battery Cell with Simulation-driven Engineering

Tue, 26 Nov 2024 16:28:56 GMT

Introduction Batteries are becoming increasingly important in our daily lives, from smartphones to electric cars to large-scale power grid storage. As electrification becomes more widespread, batteries with higher capacity, lower cost and weight, longer lifespans, and the ability to meet strict operating conditions and safety standards will be needed. Companies that can meet these requirements will have a significant competitive advantage. The process of developing an improved battery begins at the cell level. Cells are the fundamental units of batteries, comprising electrodes and electrolytes. A battery pack is formed by connecting multiple cells, often with added structural, thermal and control elements. Simulation helps engineers to enhance battery cell design and develop new cell technology. In this blog post, we will introduce the Battery Cell Engineering workflows from SIMULIA on the 3DEXPERIENCE® platform and demonstrate how they can be utilized to create high-performance battery systems. Challenges of Battery Engineering When developing a battery system, engineers must consider many competing design requirements. The following examples are from electric vehicles, but other industries have similar needs: Capacity (driving range): The battery should have the maximum possible capacity to minimize the frequency of recharging and extend the overall lifespan of the device. Charge time: The faster the battery charges, the sooner a driver can return to the road. Weight: A lighter battery leads to quicker acceleration and improved energy efficiency. Longevity: The car battery is a costly component. A longer lifespan reduces maintenance costs and increases resale value. Temperature: Charging and discharging produce significant heat inside the battery, requiring it to be cooled in hot weather and warmed in cold weather. Safety: The battery must withstand the stresses and vibrations of use and remain safe even in a crash. To achieve all these design goals and find the best trade-offs, engineers need to understand not only how the cell behaves in the lab but also how it will perform during real operating conditions Recent advancements in the battery industry have also made development more challenging. Suppliers and manufacturers create a more intricate supply chain as the industry expands. Developing battery cells, manufacturing at scale and integrating them into vehicles or devices can involve numerous players, each operating at different levels of detail, from the molecular to the system. Established cell manufacturers face competition from startups and joint ventures with other industries, such as automotive and energy, are increasingly common. Cell manufacturers are exploring new technologies such as solid-state electrolytes and sodium ion cells. Why Simulate Battery Cells? Test on a Virtual Twin Without a Prototype Simulation enables engineers to meet these challenges. With simulation, engineers can analyze battery performance without a physical prototype using a virtual twin. This digital representation of the battery includes all the relevant data—such as geometry, electrode and electrolyte properties and their interactions—needed to represent its real-world behavior accurately. Virtual twins need to capture the complex geometry of battery cells, such as layered cylindrical (“jellyroll”) designs. The 3DEXPERIENCE Battery Cell Engineering solutions help design the layered 3D battery cell geometry and convert them into detailed, realistic simulation-ready models. After simulation, every aspect of the cell, such as temperature distribution or ion concentration, can be visualized in 3D. The virtual twin can be analyzed at any stage of development, from very early in the design phase to before constructing a physical prototype. This allows for comparing different concepts and optimizing design parameters to ensure that the design will meet the requirements before committing to a specific design. The risk of potential failure, costly rework, and project delays are minimal. Optimize Electrochemistry for Efficient Performance The performance of a battery in charging, storage and discharging is determined by its electrochemistry. This complex multiphysics, multiphase phenomenon is determined by the 3D structure of the cell and interplay between the electrode and the electrolyte. Analyzing these with testing is time-consuming and measurement limitations inherently constrain the insight provided. The Battery Cell Engineering solution provides an extended, 3D porous electrode theory (PET) based on the Newman model to simulate the cell’s performance in real-world situations. This models the electrochemistry within the cell, considering both micro-scale and macro-scale details. The different aspects of physics – structural, thermal, electrochemical and pore pressure – are considered together. Engineers can analyze factors such as charge/discharge behavior at different charge rates under different mechanical and thermal conditions. As the simulation is in 3D, users can also assess and predict three-dimensional behaviors such as thickness deformation and stress caused by swelling. Ensure Safety in Real-world Scenarios Battery cells are designed to store high energy densities in a portable way, such as inside a smartphone or an electric car. As a result, they are exposed to many difficult and dangerous scenarios—extremes of heat and cold, bending, impact and penetration. Battery cells need to withstand these hazards—if they fail, they should fail safely. Simulation can safely replicate dangerous real-world scenarios within a virtual environment. Events such as nail penetration, car crash or thermal runaway can be studied without the cost and risk of constructing and destroying a physical prototype. Make Batteries a Better Investment with Longer Lifespan and Reliability Batteries age over time (calendric aging) and through repeated use (cyclic aging). Calendric aging occurs, for example, when a battery is stored out of use, while cyclic aging takes place each time the battery is charged or discharged. The expense of the battery significantly influences the cost of an electric vehicle and one of the primary causes for the rapid depreciation and increased cost of ownership of electric cars is battery aging. Electric vehicles will become a more attractive investment for drivers and fleet managers if battery cells can last longer. The Battery Cell Engineering solutions on the 3DEXPERIENCE platform provide comprehensive workflows to simulate these aging processes. It can model various battery aging mechanisms, such as formation & growth of the SEI, lithium plating, and dissolution of the cathode. By analyzing these effects, engineers can optimize the battery’s lifespan and produce more reliable batteries that customers demand. Explore Battery Science Down to Cell Chemistry Optimization Battery Cell Engineering on the 3DEXPERIENCE platform combines SIMULIA multi-physics simulation workflows with key capabilities from BIOVIA for scientific chemical and material engineering and CATIA for design and modeling. Together, these support battery engineers in designing, analyzing, optimizing and validating battery cells using 3D virtual twins. All process stages take place in the same environment: the 3DEXPERIENCE platform, which provides a single source of truth for all the battery cell engineering data. Designers, analysts and other stakeholders can share information and collaborate reliably and securely. Unified modeling and simulation (MODSIM) helps to left-shift the analysis process so that cell designs can be optimized earlier and potentially identified and resolved, ensuring a more consistent, error-free and accelerated design cycle. The highly detailed 3D Newman modeling in the Battery Cell Engineering tools on the 3DEXPERIENCE platform is the key to creating realistic simulations of the cell’s thermal and electrochemical behavior. These simulations provide the highest quality predictions about the cell’s performance and age, including any impacts from its use in different conditions. Microstructural simulations enable deep analysis of material characteristics within the electrodes. Meanwhile, mechanical simulation is used to test the cell’s behavior in events such as thermal stresses, mechanical indentation or nail penetration so that engineers can design for optimal safety throughout the cell’s lifespan. Conclusion From smartwatches and phones to electric cars and grid storage, battery performance is crucial to the success of devices large and small. This performance is determined at the battery cell level by the electrochemistry and multi-physical interactions within. Developing an efficient, safe and competitive battery requires understanding the cell’s complex three-dimensional behavior. Dassault Systèmes provides a full Battery Cell Engineering solution on the 3DEXPERIENCE platform. This solution integrates the best design and simulation solutions into a workflow. Using these tools, battery designers can analyze battery performance accurately from the comfort of their desks without having to build physical prototypes. With the Battery Cell Engineering solutions on the 3DEXPERIENCE platform, battery cell manufacturers can enable collaboration between all stakeholders and left-shift analysis in the development cycle. Potential safety and efficiency problems can be resolved early without extensive re-designs that cause delays and cost overruns. With simulation, battery cell manufacturers can develop innovative and competitive new products while cutting R&D costs and time-to-market. For more information, see the on-demand webinars: https://events.3ds.com/battery-cell-engineering-faster-modsimhttps://events.3ds.com/future-aircraft-development-modsim Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

Workflow: Modeling and Simulation of a Tower Crane

Fri, 22 Nov 2024 17:34:03 GMT

Introduction A tower crane is a modern form of a balance crane with the same basic parts. Fixed to the ground on a concrete slab (and sometimes attached to the sides of structures), tower cranes often give the best height and lifting capacity and are used to construct tall buildings. The conditions under which the crane operates determine its general dimensions very largely. The height is fixed by the height of the tower it is constructed and the radius at which the maximum load is to be lifted, as determined by practical considerations and the construction site. During the design of these cranes, static loads are generally considered based on utility requirements/load-carrying capacity, but forces and torques on components resulting from motion simulations can also serve as useful input for detailed structural analysis. Below is a concise overview of a tower crane workflow, highlighting the tools and processes used. Workflow Overview 1. 3D Modeling: – We created detailed 3D models of each component using 3DExperience CATIA: – Part Design App for individual components. – Assembly Design/Mechanical Systems Design App for assembling the crane. 2. Dynamic Simulation: – Using the assembled model, we employed the Motion Analysis App to create mechanisms and perform dynamic simulations, analyzing the crane’s movement and interactions. 3. Structural Analysis: – To analyze the structural integrity of the hoist: – We used the ‘transfer loads’ command from Motion Analysis to generate a simulation object that includes load data. – This object is compatible with structural analysis apps like Structural Model Creation and Mechanical Scenario Creation, where we finalized couplings and computed structural simulations. 4. Cable Modeling: – Since the Motion Analysis app currently lacks the capability to simulate cables: – We utilized Simpack to model the cable elements. – We exported our assembly from 3DExperience to Simpack using the connector, which converts the model into a format compatible with Simpack, complete with mass and inertia data. 5. Enhancing the Simpack Model: – In Simpack, we extended the model to include: – Pulleys for cable support. – Connections and excitations to represent motors. – The cable element itself. – This allowed us to simulate the full behavior of the Tower Crane, including cable dynamics. We reviewed results and animations within Simpack to analyze crane performance. To view the full workflow, visit the SIMULIA Community post, which includes a PowerPoint presentation and a video that provide a more detailed explanation of the workflow and findings. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

SIMULIA Executive Corner: Modeling and Simulation Trends

Tue, 19 Nov 2024 15:50:18 GMT

Q: What industry challenges are driving the need to increase the use of modeling and simulation (MODSIM)? A: When I travel and meet our customers at their locations and at our events, I hear similar challenges among them. Certainly, time, cost, global economics, and environmental regulations are driving the expanded use of modeling and simulation across all industries. Product development companies aim to build fewer (or zero) prototypes to reduce time, costs, and waste while reducing the risk of product failure during operation. Product development organizations are also looking for solutions to improve process efficiencies, decision-making, and product quality throughout the design process, leading to growth in the use of simulation earlier in the development cycle. Other important areas that will benefit from simulation solutions include sustainability (CO2 emissions, green energy, etc.), battery development, new materials innovation, and connected cyber systems. Q: What are some of the industry requirements for simulation? A: Each industry has unique requirements, and a diverse range of industries are empowered to leverage robust multiphysics/multiscale simulation applications to solve their challenges. For example, theTransportation and Mobility industry requires more simulation to develop vehicles that meet fleet emission mandates. This requires managing the development of multiple powertrain configurations across their vehicle lineup, including internal combustion engines, hybrids, hybrid plug-ins, full-electric vehicles, and research for hydrogen power. Connected vehicle systems, including Driver Assistance and fully autonomous vehicle developments, also demand more simulation within the electronics and mechatronics fields. The Aerospace and Defense industry is being influenced by the need for sustainable aircraft and the growth in low-orbit satellites for communications, geo-mapping, and climate forecasting. The growth in the number of satellites and space programs requires reliable electronics and lightweight yet durable reusable launch vehicles. The Life Sciences & Healthcare industry is growing in medical device and implant development to meet the demands of aging populations. The Infrastructure & Energy industry is looking for alternative and new energy sources that must be developed and maintained to handle the increasing demands for charging electric vehicles, computational power for expanding AI applications, and electrical transmission grids for powering businesses and homes. There are industry requirements to explore CO2 capture and storage solutions and meet plant maintenance and fitness for services requirements, in which modeling and simulation play a critical role. The High-Tech industry’s growth in semiconductors and mobile devices requires simulation to improve processor (chip) designs and performance, including those related to size, design space, wireless transmissions, electronic interference, heat, moisture, and drop-testing, among other functional performance requirements. The Consumer Packaged Goods industry is in demand for green, recyclable packaging, which is driving growth opportunities for analyzing the complex behavior of metals, plastics, paper, glass, and fluids and related manufacturing processes to reduce material usage and improve the reliability of packaging during manufacturing, storage, and shipping. Q: What do you see as Technology Trends in simulation? A: Our customers want to improve their product development through Digital Transformation Initiatives. Unified Modeling and Simulation (MODSIM) is a critical part of that transformation. MODSIM unifies modeling and simulation on a common data model within a single user experience on the 3DEXPERIENCE platform. The goal is to consider the whole product development process and break down barriers. The movement away from working in silos to a more integrated approach is more the norm in today’s landscape. Advances in Artificial Intelligence and Machine Learning (AI/ML) is not just a trend in the simulation industry, but is a cornerstone of how we will use simulation in the future. I believe this will drive increased use of simulation by requiring substantial use of simulation to train and validate the AI/ML models, now and in the future. AI/ML models will continually need maintenance and additional training, which will further drive the use of simulation. And, simulation models will provide data for virtual validation to AI/ML in the same way that simulation and physical testing are used in the verification and validation processes today. The trend of using the 3DEXPERIENCE cloud platform is growing within small and large organizations. I’ve heard end-users report that they highly value access to our Software-as-a-Service and high-performance computing on the 3DEXPERIENCE cloud platform. This acts as a “kick starter” on the cloud, allowing them to perform simulations from any computer anywhere, at any time. Plus, it gives them access to more computing capacity than they have available on their local computers or networks (especially in smaller companies that have not invested in local compute clusters). By using the 3DEXPERIENCE cloud platform product development organizations can run more simulations at higher fidelity while reducing the cost and maintenance of on premise computing infrastructure. Organizations must understand that digital transformation is more than accessing simulation software or high-performance computing resources on the cloud. It’s also about connecting people, processes, and data. All of the required design and simulation applications and the associated functional requirements and results are available on 3DEXPERIENCE on-cloud to all stakeholders, such as designers, industry process specialists, simulation experts, and manufacturing teams. This enables them to collaborate on their projects securely, in real-time, across global time zones, which improves efficiencies, reduces manual errors, and helps them confidently accelerate innovative products to market. As we start to wrap up 2024, I’m looking forward to connecting with our customers at upcoming events, including India in November and the MODSIM Summit in early 2025, to discuss how we can innovate the future together. There are many challenges as industries change and technologies grow, but simulation continues to evolve and transform. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

Simulate Electrostatic Discharge on a Virtual Twin

Thu, 14 Nov 2024 17:51:46 GMT

ESD contact discharge is usually tested in the lab by physically connecting a high-voltage probe to a prototype of the device under test (DUT) at a specific location, such as a connector pin. Additionally, a non-contact test is carried out by placing the probe at varying distances from likely discharge points on the DUT. These tests must be repeated for every possible connection & discharge path, making ESD testing time-consuming and expensive. It can also be difficult to understand the root causes of failure from the limited output of an ESD test. Many prototypes can be damaged or destroyed in the testing process. Virtual testing with simulation can accelerate ESD analysis, reducing development time and cost. Both the test equipment and the DUT are created and connected in the virtual environment, with waveforms generated to replicate the real-world tests. 3D visualization of simulation results shows the exact path of currents through the device, helping engineers understand the causes of ESD problems and develop design mitigation strategies. Challenges of ESD Analysis and Mitigation ESD is a significant risk for electronic devices: Sensitive low-voltage electronic components such as integrated circuits (ICs) can easily be damaged by high-voltage pulses. Even if catastrophic damage does not occur, permanent damage may occur, reducing the life of the device or cause unexpected behavior. ESD occurs when a static electric charge is generated on an object and then discharges to earth via an electronic device. This often happens if a human user picks up an electric charge from friction with their clothing, the floor or furniture, and can also come from moving machinery such as vehicles or conveyor belts or from electrostatic induction from other charged objects. ESD test of a smartphone, showing the propagation of currents from discharge at the charging port For ESD to occur, there must be a path between the charged object and the ground through the device. This path can be either direct contact or close proximity contact in which case an arc through the air gap will form. In dry air, static charges can build up more readily, with faster rise times, and higher peak amplitudes, while in humid air, non-contact discharge can form with longer arcs, more slowly rising with lower peak amplitude. The large number of variables in conditions, contact type and arc type mean that analyzing ESD risk requires a long series of physical tests on a significant number of expensive prototypes. Tests have to occur late in the product cycle when detailed prototypes are available. If issues during ESD testing are found, there are a number of steps required that may cause delays and impact the scheduled release date. Steps include understanding the causes of any failure and redesign and rework of the device to mitigate the issue for the next prototype. ESD testing on modern devices can be particularly complicated as additional components are now integrated into a single device, such as a system on chip (SiP). The ESD protection for each individual IC must be harmonized with the system-level ESD protection (SEED). Ensuring safe voltages and currents at all ICs can require trade-offs in terms of component placement, informed by a large number of tests. Benefits of Electrostatic Discharge Simulation Simulation offers a faster alternative to testing. Unified modeling and simulation (MODSIM) makes it easy to turn CAD geometry data into a simulation-ready virtual prototype of the DUT and the test equipment set-up. An excitation at the tip of the virtual generator creates an ESD pulse, and the simulation calculates its propagation through the device. 3D field monitors can visualize the exact path of currents flowing through the device, and virtual field probes can be placed anywhere in the virtual space, including inside the device. Surface currents in an ESD test on an Ethernet system, comparing two different diode placements. Evaluating ESD susceptibility virtually means that problems can be identified and resolved even before construction of the first prototype. This approach enables engineers to get the design right first time, saving on prototyping costs and reducing the risk of project delays caused by issues discovered during testing. The SIMULIA ESD Simulation Solution CST Studio Suite contains state-of-the-art electromagnetic solvers for simulating complex components and systems accurately and efficiently. ESD is inherently a transient phenomenon, and it can be simulated effectively using the 3D Time Domain Solver. The Time Domain Solver also offers highly efficient 3D meshing that is robust enough to deal with poor CAD geometry. Complex geometries are represented accurately and virtual tests can be run rapidly. Design of Experiments (DoE) capabilities allow automated testing of various scenarios with clear visualization and comparison of large datasets. The ESD susceptibility analysis workflow starts with building the DUT’s virtual twin. 3D geometry and PCB or IC layouts from standard CAD and EDA tools can be imported into the virtual environment and converted into simulation-ready models with automatic clean-up and meshing. Pre-defined ESD-specific templates, such as 3D models of ESD generators and ESD pulse excitations, available from the CST component library, help users define their simulation set-up. The ESD generator models have been developed and validated to comply with international standards such as ISO 10605 and can accurately model real-world ESD test set-ups. Users can build representations of standard tests that replicate the set-up found in the lab. ESD simulation representing a test set-up as defined by ISO 10605. Both contact and air-gap ESD generators can be simulated. In the case of an air gap (in other words, where voltage breakdown in the air causes an arc, an electromagnetic simulation is first performed to calculate possible arc paths at different voltages using Paschen’s law, and to generate a SPICE model that represents the non-linear electromagnetic properties of the arc. This then forms the basis for the time domain simulation of the ESD pulse, with true transient co-simulation combining the SPICE circuit model with the 3D simulation model. Close up of the ESD simulation set up, showing the DUT on the left and the ESD gun probe on the right, with an element representing the spark. The simulation produces several ESD KPIs and a 3D visualization of electromagnetic fields and surface currents around the device. Using virtual probes, users can view voltages at any point in the structure throughout the duration of the pulse. Users can generate all the KPIs that a physical test would provide, and some that would be impossible to measure. Conclusion Electrostatic discharge (ESD) can cause errors and device failures and affect the safety and reliability of a device market. Successfully bringing an electronic product to market means meeting legal ESD regulations and ensuring that a device is protected from ESD exposure. Electromagnetic simulation can be used to analyze ESD risk on a device without the cost of building and potentially destroying physical prototypes. A virtual twin contains all relevant data about the product and can be used to accurately represent product behavior in a virtual test using simulation. Engineers can quickly build a virtual twin of their product from the design data thanks to the unified modeling and simulation (MODSIM) approach enabled by Dassault Systèmes tools on the 3DEXPERIENCE platform. With virtual testing, engineers can understand ESD risk from the earliest stages of design and can develop protection and mitigation strategies for individual components or the entire device. Virtual testing helps prevent problems being discovered late in development when rework is expensive and risks delaying the entire project. It also reduces the risk of device failures after launch and the cost of recalls. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

General Motors Puts the Spring in Suspension with Simpack

Tue, 05 Nov 2024 14:35:11 GMT

Challenge Find a more efficient, accurate way to model the complex configurations and multibody dynamics of leaf spring vehicle suspension systems. Traditional approaches were intricate, challenging and resource-intensive, making it difficult to model tailor-made suspension for different vehicle programs. Solution Create a multibody dynamics modeling tool using the SIMULIA Simpack solution, with support from the Dassault Systèmes SIMULIA team. Results Increased efficiency – simulations that used to take a day can now be done within an hour Fast, accurate simulation results delivered by Simpack’s robust solver Confidence in supporting future vehicle innovation Sometimes old ideas are the best ones, but that doesn’t mean it’s simple to apply them to new designs. Take the leaf spring, for example. It’s one of the oldest forms of vehicle suspension, dating back to the horse-drawn carriages of 17th-century France, and it’s still in use today. “Leaf spring is a super-old technology, but it is very cheap to make and provides a really good suspension system for vehicles,” said Ameya Apte, vehicle dynamics and load simulation engineer at General Motors (GM). Essentially, leaf springs consist of long, flat steel plates that are curved into an arc and stacked together in a pack. A second and even a third pack might be added, each containing different shapes and quantities of leaves. That opens the door to endless configuration possibilities. “Different leaf spring configurations provide different suspension rates for a vehicle,” Apte explained. “A smaller vehicle would need a smaller leaf pack with fewer leafs, while a larger vehicle would generally need a larger leaf pack with more leafs. Basically, the amount of load that the rear axle carries is what primarily affects the leaf design. It depends on what kind of ride and what kind of handling you want from the vehicle.” Simulation is essential to fully analyze the different ways the leaves of each spring interact with each other. “If you’re looking at the stresses inside a leaf, it’s practically impossible to do that in a test, but you can do it in simulation,” Apte said. “Similarly, if you want to measure the force between two leaves you can put in a load transducer, but that also modifies the model itself.” But from a simulation modeling perspective, factoring in those multibody dynamics was a complex and resource-intensive task. As a result, modeling tailor-made leaf springs for each vehicle program could be time-consuming, error-prone and difficult to standardize as a process. “Leaf springs have been around for hundreds of years, so people might think it’s a simple technology to model, but the opposite is true,” Apte said. “One challenge with leaf springs is that the leaves themselves articulate with the suspension, so there is friction between them that needs to be modeled. In addition, the bushings attached between the chassis and the leaf springs also have frequency-dependent properties that must be modeled.” Carmakers typically use finite element analysis solutions to model and simulate the complex geometries, materials and physics involved in vehicle design. But for GM’s leaf springs, Apte wanted a multibody dynamics tool that would support the more efficient modeling of these complex systems. He and his team used SIMULIA technology to create the tool they needed. “The tool that we developed allows us to make leaf springs that are standardized and tailor-made for different applications,” Apte said. “Users simply type in the parameters they want for the spring – such as the number of leaves in a pack, how they are distributed across the primary, secondary and auxiliary pack, their shapes, tapering and so on. With that information, the tool will create a model that can be used to predict vehicle dynamics performance and loads.” Two key ingredients contributed to the tool’s success. One was the comprehensive support provided by SIMULIA’s technical, back-end and R&D teams. The other was SIMULIA Simpack – a technology for developing and simulating high-fidelity multibody systems. Apte was particularly impressed with Simpack’s solver, which was miles ahead of other tools he had worked with. “With Simpack, you practically do not have to modify solver parameters to get a model to run,” Apte said. “You might modify parameters to increase or reduce run times or get better fidelity in some part of the simulation, but you generally don’t need to do it to run a model. That robust solver is very useful because it allows us to look at the results, understand the physics happening behind them and then send the model out to our design engineers.” As well as supporting more efficient leaf spring simulation, the tool also delivers accurate results, so Apte and his team can simulate with confidence. “If a simulation for leaf springs takes a day to do with FEA tools, with Simpack it can be done within an hour,” Apte said. Looking ahead, Apte believes the solver he has in this tool will stand the test of time, even as the industry continues to evolve and new technologies emerge. “I think the physics solvers that we have now will be supercharged, rather than eradicated, by disruptive technologies like artificial intelligence and blockchain,” Apte said. “The time it take to get a new vehicle to market has reduced significantly over the decades, and we see a potential to reduce it further with new tools. In the long term, learning these new tools and imagining a future where we can combine them to create the right applications will be a huge part of our job.” Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.

Packaging OEM Magazine Interviews Dassault Systèmes

Mon, 04 Nov 2024 18:53:07 GMT

Packaging OEM magazine recently interviewed Ray Wodar, global director business consulting for the CPG & Retail industry at Dassault Systèmes, about how CPG brand manufacturers can accelerate eco-friendly and sustainable packaging designs. Here’s a brief Q&A with Ray’s responses to four (of a total of 11) critical questions regarding sustainable packaging efforts in the industry: 1. Beyond materials, what needs to be considered when creating a sustainable package design? “When creating a sustainable package design, several factors beyond just the choice of materials need to be considered to minimize environmental impact and enhance overall sustainability. The design should be optimized to minimize the size and weight of the package to decrease material usage and excess packaging while still effectively protecting the product. A lighter product will also reduce transportation emissions in the supply chain. A thorough evaluation of the entire supply chain will help understand the environmental impact from production through to transportation and distribution. This includes considering how far materials and finished products need to travel and the associated carbon footprint of that journey. Considerations for end-of-product-life are critical as well. This involves designing for disassembly (if applicable), providing clear recycling or disposal instructions, and considering the lifecycle impact of the packaging once it has been discarded. Using materials that are widely accepted by recycling systems or that can biodegrade in industrial composting facilities is critical. For a brand manufacturer, the cost profile of the package will be very important so that tradeoffs between material cost, weight, and quality can be properly balanced to provide the consumer a great value while managing internal product margins.” 2. What are the regulatory pressures associated with sustainable packaging? “Regulatory pressures related to sustainable packaging are increasingly influencing how companies design, produce, and manage packaging. These pressures come from various levels of government and regulatory bodies and can vary by region. Many regions are implementing extended producer responsibility (EPR) programs that require producers to take responsibility for the entire lifecycle of their packaging, including end-of-life disposal and recycling. Companies may need to manage or contribute to the costs of collection, recycling, or disposal. Several countries and states have introduced bans or restrictions on single-use plastics and certain types of packaging. Regulations might limit or prohibit the use of plastic bags, straws, or other single-use plastic items, pushing companies to seek alternative materials or packaging solutions. Governments are starting to set targets for waste reduction, recycling rates, or the reduction of packaging waste. Companies are often required to meet these targets or face penalties. For companies operating globally, international regulations and agreements, such as the European Union’s Packaging and Packaging Waste Directive, can affect packaging design and sustainability practices.” 3. How can 3D modeling software help? “3D modeling software enhances the design process by providing a detailed, interactive platform to explore and optimize sustainable packaging solutions, leading to more effective and efficient design outcomes. 3D modeling software allows designers to create detailed visual representations of packaging designs. This helps in visualizing how sustainable materials and design choices will look and function in the real world before physical prototypes are made. Before creating physical prototypes, 3D models can be used to simulate how the packaging will behave under various conditions. This includes testing durability, functionality, and fit, which helps in optimizing the design for better performance with sustainable materials. More advanced 3D modeling tools can also integrate with lifecycle assessment (LCA) software to evaluate the environmental impact of packaging designs. This helps in understanding the potential environmental footprint of different design choices and materials.” 4. In a circular economy, does recycling of the package come into the design process? “Yes, in a circular economy, the design process is significantly influenced by how the package will be recycled. The principles of a circular economy aim to minimize waste and make the most of resources. This requires considering the entire lifecycle of a product, including its end-of-life stage. Key considerations in the design process for packaging in a circular economy include choosing materials that are recyclable and can be separated easily from other components. Biodegradable or compostable materials might also be considered.” Read the full interview from Packaging OEM magazine HERE Also, explore deeper on the MODSIM topic for packaging and download a free ebook on our website.

Halloween Treat: Pumpkin Smash using Abaqus from Fidelis

Thu, 31 Oct 2024 08:00:00 GMT

This blog post was originally published in October 2020, but smashing pumpkins never gets old! We’ve got a special Halloween treat! Guest blogger Rob Hurlston from Fidelis is sharing his ductile damage tutorial for a pumpkin smash. Hope everyone has an enjoyable and safe Halloween! We all love Halloween. The cooler weather, the candy and, of course, the pumpkins. So, in the spirit of the season, we at Fidelis decided we’d try to recreate the never-gets-old feeling you get when you see a pumpkin smash into pieces on the ground having been dropped from a great height. And what was the first tool we thought about in order to pull this off? Abaqus of course! We settled on a 5m drop, which is equivalent to something like a second-story window – hence something we can all recreate at home if we feel the need to carry out an impromptu correlation study. With this being a highly dynamic event, we utilized Abaqus’ explicit solver and, to ensure the pumpkin actually smashed when it hit the ground, we took advantage of the ductile damage feature. Typically, this methodology might be reserved to predict failure in metallic components of a car or airplane, but a little creative tuning of the parameters allowed us to generate reasonably true-to-life behavior of the classic pumpkin drop. For some background, the ductile damage method allows us to prescribe a reduction in both yield strength, Dσ, and elasticity, (1-D)E, as strain increases beyond a predefined threshold (see figure). Eventually, the element reaches zero load carrying capability and is effectively removed from the analysis. The full workflow tutorial to replicate this analysis within the Abaqus CAE graphical user interface (GUI) is included in this video, but we’ll summarize the important parts here in the order that they were executed: Parts and Assembly First of all, we must create the parts . A solid revolved hollow sphere of diameter 600mm and wall thickness 25mm represents the main body of the pumpkin. To ‘carve’ the face, the ‘Create Cut: Extrude’ feature should be employed – and you can go wild, freehand, with the sketching tools. I even gave my pumpkin a snaggly tooth. A solid extrude is generated for the stem and that is combined with the pumpkin body using the ‘Merge/Cut Instances’ process within the Assembly module. Finally, a discrete rigid shell is defined for the ‘floor’ and the parts are arranged (translate; rotate) such that the pumpkin begins its journey from a round 1x it’s diameter from its landing zone. Property As mentioned earlier, the properties for the pumpkin were somewhat tuned, but we tried to base them in some sensical assumptions. Density, for example, was taken from measured data at 4.8 g/cm3 (or 0.48×10-9 tonnes/mm3). Other parameters can be seen below: Elastic: Young’s Modulus = 20MPa, Poisson’s Ratio = 0.3 Plastic : Yield Stress (MPa) Plastic Strain 2 0 3 0.1 Ductile Damage: Fracture Strain = 1×10-5, Stress Triaxiality = 0, Strain Rate = 0 Damage Evolution: Type = Displacement, Softening = Linear, Degradation = Maximum, Displacement at Failure = 5×10-5 mm Step The step is, of course, Dynamic Explicit in nature, so the step type should be selected accordingly. Time is set to 1 second and mass scaling defined to give an increment time target of 1×10-6 s. Interaction A couple of interactions must be defined for the analysis to work. Firstly, we need to apply a Rigid Body Constraint between the discrete rigid floor and a predefined control node or Reference Point. Then we can apply General Contact to the entire assembly – and don’t worry about contact parameters, the Abaqus defaults are fine for this analysis. Load (And A Predefined Field) When the pumpkin lands, we don’t just want it to bounce back into space, we want it to flop and fall, and so we must prescribe Earth’s gravity to the analysis. That means a Load of type Gravity and value -9,800 mm/s2 in the direction of the y-axis. Further, we don’t want to have to extend the analysis further than is necessary, so we define the velocity that the pumpkin would be travelling had it been dropped from a height of 5m in the form of a Predefined Field. In this case, that is -9,900 mm/s. It’s not just ‘loading’ that is defined within the Load module of CAE. Boundary Conditions also need to be specified here, and in this case, all we need is an Encastre condition on the Reference Point of the discrete rigid surface that we made earlier. That will ensure that the floor stays exactly where it is throughout the entire analysis. Mesh The pumpkin geometry that we’ve produced is too complex for the mesher to assign a hexahedral mesh, which is – fittingly – why it shows up as orange initially. For this analysis, we’re fine with a sloppy tetrahedral mesh and so we select Free Tet in the ‘Assign Mesh Controls’ window. With a global mesh size of 25mm, the part is ready to be meshed. The discrete rigid must also be meshed, and we let CAE do all the work here, simply clicking the ‘Mesh Part’ button and moving on. It should be noted that the STATUS Field Output is required so that the spent elements are removed from the visualization of the analysis and we should output results at 200 evenly spaced intervals. At this point, we’re ready to launch the analysis! Hopefully you can have a bit of fun with this ghoulish tutorial, and maybe take something away that helps you in future simulation efforts, particularly in the form of explicit analysis that includes ductile damage. As a provider of all of SIMULIA’s simulation products, as well as a CAE services provider that puts them to good use, we’d love to hear from you about your software and simulation needs! Robert Hurlston, EngD, PGDip, MEng, is a Principal and Chief Engineer and co-founder of Fidelis. Throughout his career, he has worked on and led on a diverse array of projects across a range of industries. This has allowed him to sharpen his analytical proficiency, particularly in the fields of linear and nonlinear stress analysis, dynamics, fatigue, and optimization. Rob has a strong background in materials, with a specialty in metallurgy and structural integrity engineering. His industrially based doctorate and subsequent post-docs in nuclear materials engineering saw him accumulate over a decade of real-world experience in collaboration with Serco, the University of Manchester (UK), and their partners. Rob has presented much of his work at a number of prestigious international conferences and has also published several journal papers. Rob holds a first-class master’s degree in materials science and engineering and a postgraduate diploma in enterprise management, along with his doctorate, all of which were completed at the University of Manchester. He is a big soccer fan and an avid golfer. He also enjoys skiing, hiking, and playing the guitar, as well as spending time with his family.

SIMULIA User Experience Research Program

Thu, 24 Oct 2024 15:32:47 GMT

The SIMULIA User Experience Research Program gathers feedback from people who use SIMULIA applications. Participants have the opportunity to share their experience using our applications, evaluate ideas for possible future enhancements, or test recently released features. Participants influence SIMULIA R&D by shaping our understanding of their work, enabling us to enhance and innovate our applications better. In 2023, people from 16 organizations participated in the Research Program. Research topics included data organization, selection challenges, managing simulation storage, and using sensors. We always have a variety of research projects underway and are constantly looking for users to participate. Who Participates? People who use simulation applications! We talk with them about their daily work. We either: Discuss their daily work in detail, to learn about the strategies they use to accomplish their work tasks, or Ask them to try using a mockup we’ve made of potential future application functionality, to see whether the ideas in the mockup would help them to do their work. Simulation information suppliers, consumers, or evaluators: We talk with them about the information they supply to inform the simulation work, how they use the information produced by simulation work, or what they look for when evaluating simulation work outputs. About the Interviews Each research interview is a meeting of one participant and one researcher, either over Zoom or in person. A colleague of the researcher is also present to take notes. The interviews are scheduled at the participants’ convenience The participant does not need to do any preparation for an interview The time commitment is 1-2.5 hours, depending on the topic Everything seen and heard during these meetings is confidential, and all participant information is carefully protected. Research Topics for Q4 Here’s an overview of the topics we are researching in Q4. Managing simulation data: Testing ideas for new ways of organizing and reviewing simulation data, for both Fluids and Structures simulations, and a new Feature Manager. We are looking for: Fluids simulation experts doing internal flow, external flow, or multiple rotating frame (MRF) simulations, using 3DEXPERIENCE or SOLIDWORKS FLOW Plastics designers familiar with mold flow Structural simulation experts doing any type of structural simulation, and eitherFamiliar with SIMULIA 3DEXPERIENCE apps (Structural Model, Mechanical/Structural Scenario, Physics Results Explorer) Roles: SYE, SSU, SRD or similar Users of other pre/post software like Ansa, HM, Ansys, etc New streamlined fluid simulation workflows: Testing new workflows and functionality for increased productivity. We are looking for: Fluids design engineers, including new CFD users as well as more experienced users, doing interior or exterior Flow simulations on component or small system models Either watertight or non-watertight geometries Single Domain or Multidomain & Heat transfer Familiar with Solidworks Flow, FMK, Star CCM+, or Fluent Linear static structural analysis: Testing ideas for a new tool to help people understand the quality of their linear static simulation results. We are looking for: Designers or design engineers who create, run, and inspect the results of simulations for linear static structural analysis(Preferred) Actively use FE structural simulation products, ideally the Linear Structural Validation app provided with the SIMULIA Structural Designer (SRD) role, or the Linear Structural Scenario app provided with the SIMULIA Structural Engineer (SLL) role. Use SOLIDWORKS Simulation for linear static analysis Collaboration on design decisions using simulations: Learning what information is important to capture while doing simulation work, and how it is used when collaborating to make product design decisions. Also, how information about key decisions is preserved to grow a company’s “best practices”, and shared with both new and experienced engineers. We are looking for: Design engineers or simulation analysts who do any kind of simulation that is being used to inform product design decisions While doing simulation work, capture important information on paper or digitally Create file-based reports/proposals, or use Physics Results Explorer, Physics Simulation Review or 3D Markup to create reports/proposals Managers or other people who use the guidance from simulation work to collaborate on or make product design decisions 3DEXPERIENCE Adoption: We are always interested in talking with new users (< 1 year of experience) to better understand the challenges people encounter when transitioning to using 3DEXPERIENCE. Participate! If you think you might be interested in participating or know someone else who might be a good candidate, contact the SIMULIA User Experience Research Program at SIMULIA.usability@3DS.com for more information. Interested in the latest in simulation? Looking for advice and best practices? Want to discuss simulation with fellow users and Dassault Systèmes experts? The SIMULIA Community is the place to find the latest resources for SIMULIA software and to collaborate with other users. The key that unlocks the door of innovative thinking and knowledge building, the SIMULIA Community provides you with the tools you need to expand your knowledge, whenever and wherever.