Understanding stress vs. strain is fundamental for engineers working with material properties. However, a critical distinction exists between the stress-strain data obtained during tensile tests and the true stress-strain data required for accurate simulations in software like Ansys Mechanical.

In this article, we’ll uncover the essential differences, explain how to calculate true stress and strain, and explore why these concepts are indispensable for accurate elastic-plastic material simulations.

What is Measured and Calculated During Material Tensile Testing?

If you were to internet search for a material’s stress vs. strain data or look in the back of an engineering mechanics textbook, the stress vs. strain data provided is typically in the form of engineering stress and strain. Tensile testing for stress vs. strain is performed using tensile coupons like the layout shown in Figure 1.

This layout includes data that is measured as part of the test, where:

• P = the applied load
• A = the initial cross-section area
• l₀ = the initial extensometer length
• l = the new extensometer length after applying load P

The calculated stress and strain are:

σ_engineering = P / A

ε_engineering = (l – l₀) / l₀

These are engineering stress and strain because the calculation is performed using the initial cross-section area. However, as the tensile coupon is loaded the cross-section area reduces due to the Poisson Effect. For small values of stress and strain, the difference between engineering stress and strain and true stress and strain is low and approximated as equivalent.

Determining True Stress and Strain

There’s a handy pair of equations to calculate true stress and strain using the calculated values.

σ_true = σ_eng (1+ε_eng)

ε_true = ln (1+ε_eng)

These are simple to evaluate using the engineer’s second-best tool, Excel (the first being Ansys, of course).

Why is this Distinction Important?

You may be saying to yourself, “This doesn’t seem like that big a deal. Why are you telling me this?” It’s important to understand how simulation codes perform finite element calculations.

Let’s consider a hypothetical test procedure, where we take the tensile test coupon shown in Figure 1 and stretch it from 10mm to 12mm. This is a change in length, ∆l, of 2mm. Using the equation above for engineering strain, we can calculate an engineering strain value of:

ε_engineering = 2/10 = 0.2 mm/mm

Okay… straight forward. Let’s break that up into two steps on a second tensile test coupon. Step 1 will stretch the coupon from 10mm to 11mm and step 2 will stretch it from 11mm to 12mm; then we can simply add these two strain values to get the total strain. Pretty simple, eh?

ε_engineering = 1/10 + 1/11 = 0.191 mm/mm

What you should notice is that these two measurements do not produce identical strain values, despite both tests stretching the tensile coupon the same amount. So, what does this mean for simulation?

The second tensile test, where strain is calculated in incremental stages, directly resembles how strains are calculated in Ansys Mechanical simulation from incrementally applied loads. If analysts use engineering stress and strain as input to the plasticity material models in Ansys Mechanical, each additional increment in load represents error in the strain calculation.

Let’s redo the calculation above using true strain. The third tensile test coupon:

ε_true = ln (12/10) = 0.18232 mm/mm

And the fourth:

ε_true = ln (11/10) + ln (12/11) = 0.18232 mm/mm

As you can see, we calculate identical results using true strain. This behavior is desirable in Ansys simulation and is why Ansys Mechanical requires using true stress vs. strain as input for the elastic-plastic material models.

In fact, if you peruse the Ansys Help documentation you’ll find this note:

Hmmm… this just stated what I spent ~600 words saying. That’s alright; hopefully the illustrated examples with the tensile test coupons are helpful.

Where Else Can Analysts Learn About Ansys and Plasticity?

If you are interested in learning more about Ansys and plasticity in simulation, DRD has on-demand training content on our website. This particular topic is covered in our Nonlinear Structural Simulation course, in Chapter 3.

Ansys Mechanical Nonlinear Structural Simulation – DRD Technology

Released on July 23, 2024, Ansys Mechanical 2024 R2 introduces a powerful new native feature: Fluid Penetration Pressure. While this isn’t entirely new to Ansys, as it has long been part of Ansys APDL, it’s the first time this functionality is available natively in Ansys Mechanical. This feature provides engineers with an efficient way to simulate fluid interactions with structures without explicitly modeling the fluid in finite element analysis (FEA).

What is Fluid Penetration Pressure?

Fluid pressure penetration is a method to capture impinging fluid on a structure, without explicitly modeling the fluid in the finite element analysis.

The fluid penetration pressure method employs information of contact status between contacting bodies to determine where the fluid pressure is applied. The benefit is that this is determined as the contact status evolves over the simulation time, so the region where pressure is applied changes as contact between bodies changes under loading.

Users provide a contact region for the searching algorithm, a starting location for fluid impingement, and the fluid pressure; the solver does the rest. Figure 1 provides a simple view of the starting point on the exterior surface of the structure and the ‘flow’ of the fluid outward.

Figure 1: Schematic of Fluid Penetration Pressure Behavior

What is the Application of Fluid Penetration Pressure?

As you perhaps have guessed, the application of fluid penetration pressure is in seals and gaskets for valves, hydraulic cylinders, coil-overs, etc. This allows determination of sealing surface leakage as the structure is loaded and deforms, both from the fluid pressure itself and additional loads in service.

Figure 2: Examples of Gaskets

If engineers can determine seal capability before selling the product, expensive redesign can be circumvented. Seals do not need redesign, re-machining of the sealing surfaces is lessened, and a potentially hazardous leak can be avoided.

Example Simulation with Fluid Penetration Pressure

Here we have a simple representation of a tube, sleeve and O-ring seal in a vehicle strut or coil-over. During the assembly process, the tube is pushed downward to interface with the O-ring. In service, fluid is pushing against the seal from the top in the shown orientation, annotated by the blue arrows in Figure 3. The sleeve is fixed in place.

Figure 3: Layout of Simulation with Fluid Impingement Load Direction

As stated previously, analysts need to supply a contact, a starting point, and a fluid pressure magnitude. In the 2D axisymmetric representation of the structure in Figure 3, frictional contact is defined between the three bodies. The Fluid Penetration Pressure object is defined as shown in Figure 4.

Figure 4: Example Use of Fluid Penetration Pressure Feature, Details, Load, and Graphics

As you can see, we’ve applied the fluid pressure in the second load step; the first load step is moving the tube downward.

I’ll leave you with these final output animations, and a recommendation to visit our website to get access to on-demand training.

We walkthrough this simulation example as part of our Ansys Mechanical Nonlinear Structural Simulation course. Follow the link here: Ansys Mechanical Nonlinear Structural Simulation – DRD Technology.

When solving complex models in Ansys Mechanical, several common errors may arise. In this blog, we’ll explore three frequent error scenarios—DOF limit exceeded, unconverged solutions, and element formulation errors—and provide solutions for each.

Error Scenario 1: DOF Limit Exceeded

This error indicates that at least one body in the model has reached a degree of freedom (DOF) limit, often due to rigid body motion (RBM). Mechanical will prompt you to check for insufficient constraints. This situation is typically a result of rigid body motion (RBM), and Mechanical will have a message suggesting the user search for insufficient constraints.

In a static analysis, every part in the model must be constrained so it cannot freely rotate or translate. RBM is a consequence of one or more parts being insufficiently constrained. Check that there are enough external constraints on the model (i.e. supports) to prevent RBM. Here’s how to resolve this:

• Ensure that all parts are constrained or connected to supported parts.
• Be attached to supported parts using contacts, joints, or other connections. Mechanical offers a right-click menu in the graphics area with an option that can identify missing connections (below).

If you are depending on nonlinear contacts (Frictionless/Frictional/Rough) to hold the model together, make sure they are initially closed. The Contact Tool is a great help for this. Be aware that nonlinear contacts will not prevent separation, and they may not prevent sliding either.

If you are not able to identify any parts that are underconstrained, try running a Modal analysis with the same supports as your static analysis. The animated deformation plots from the Modal analysis should help you identify what parts need constraints. Pay special attention to modes at 0 Hz or very close to it. The mode animation below shows one part moving without deforming the rest of the assembly, indicating that it is underconstrained. Be aware, however, that Modal analysis forces nonlinear contacts to become linear, so it may not identify all problems with nonlinear contacts.

Error Scenario 2: Unconverged Solution

In this scenario, you may see the line “Reason for Termination … Unconverged Solution” in the solution information, and there will be an Error message in Mechanical that reads, “The solver engine was unable to converge on a solution for the nonlinear problem as constrained.”

This error occurs for nonlinear models. When a model is nonlinear, the solution affects the model’s stiffness, and the solver needs to iterate on a solution until the remaining error is within tolerance. There are three main factors that can cause a model to be nonlinear: material properties like plasticity, nonlinear contact types, and the Large Deflection option under Analysis Settings. One or more of these nonlinearities is responsible for the failure to converge. You will need to identify which nonlinearities are the cause.

The most helpful tool for troubleshooting a force convergence error is Mechanical’s Newton-Raphson Residuals. In the Details of Solution Information, set this to some non-zero value (2 or 3 is usually enough). The plots will only be created if a non-zero value was set before the analysis was solved. You may need to initiate the solve and let it fail again in order to get the Newton-Raphson plots. Adjusting the time steps to ensure it fails quickly is recommended. Before re-attempting the solve, you may wish to try the other troubleshooting steps in this section.

The Newton-Raphson Residual plots will show hotspots (red color) where the residuals are highest. This means you should look for conditions that are scoped to these elements. Often you will see high residuals on elements that are participating in a nonlinear contact region. If so, this contact region needs attention.

Possible solutions to a contact region with high Newton-Raphson Residuals include:

• Mesh refinement on the faces scoped in the contact region.
• Reducing normal stiffness of the contact region to a Factor of 0.1 or 0.01.
• Using a linear contact instead of a nonlinear one if acceptable.
• Using displacement-based loading rather than force-based loading to close a contact region that is initially open.

Aside from the Newton-Raphson Residual plots, there are a few other tools that can help narrow down the reason for non-convergence. Per the last section, make sure the model is fully constrained and rigid body motion is not possible. If any substeps have solved, create True Scale deformation plots for the solved time points and look for any unexpected behavior such as large deformations or assemblies separating. Plots of plastic strain can identify regions that are collapsing due to widespread yielding.

If you’ve reviewed the Newton-Raphson Residual plots and solved timesteps but it still is not clear what is causing the analysis to fail, a useful approach is to remove all nonlinearities from the model and make sure it solves. If it does, then add nonlinearities back into the model gradually. When you reintroduce a source of nonlinearity and the solve fails again, you can be confident that this nonlinearity is what needs attention before the solve can succeed.

Error Scenario 3: Element Formulation Errors

This reason for termination is often accompanied by the error message in Mechanical: “Element N Located in Body (and maybe other elements) Has Become Highly Distorted.” The element formulation error means that certain elements fail to meet criteria that are required to obtain a meaningful solution. Most often the elements have become so distorted that the analysis cannot continue. An ideal element is a cubic hexahedron or a tetrahedron with four equal sides. When elements have high aspect ratios, have highly skewed shapes, or even begin to turn inside out, they are liable to terminate the solver with this error.

The first step is to identify the elements that have the error. Look at the error messages in Mechanical and the Solution Information worksheet for specific element numbers. Then find where these elements are located in the mesh (this video shows how; use the element option instead of the node option).

There is also an option to create Named Selections for element violations under Solution Information. Set this to a non-zero value (2 is usually fine).

Using either the Named Selections or the Select Mesh by ID tool, observe the element shapes and locations. If they are highly skewed, it may help to improve the mesh in that area to get better quality elements.

Another important step is to find out how far the solver made it before the failure occurred, as described earlier. If no substeps solved, then there was a problem applying the initial conditions. Use the Contact Tool to identify contacts that have initial penetration. If you have any nonlinear contacts with initial penetration, use the Add Offset, Ramped Effects setting for those contacts, or Adjust to Touch if you wish to ignore the penetration. Elements in contact regions can easily get distorted when the penetration is removed with the No Ramping setting.

If you do have solved substeps, use the plots of the solved substeps along with the locations of the element violations. (Note again that results set to Display Time = Last are unconverged and are not meaningful.) Are these elements starting to distort just before the failed time step? Is there a lot of plasticity on these elements? If the elements are actually becoming distorted, you may need to improve the mesh to get better initial quality. In scenarios with a lot of plasticity, you may not need to solve the whole analysis if the solved time steps already show levels of plasticity that indicate failure of the product.

Sometimes the elements do not seem to be visibly distorting in the solved time steps. In that case, they may be distorting due to a load being applied too suddenly or due to insufficient constraints. Think about whether there are new loads being applied in the time step that failed, or whether there are parts about to come into contact. Consider ramping loads more slowly or using displacements rather than forces to move parts into contact.

Nonlinear modeling in FEA is a deep subject, and not every scenario or possible solution is covered here. Even so, we hope this guide will provide a starting point that will help you solve complex models in Ansys Mechanical.

Understanding error messages is crucial, but to prevent them, identifying them is key. Don’t miss our blog on how to use Ansys Mechanical’s troubleshooting tools to resolve failed solves and produce accurate results. 

When you initiate a solve in Ansys Mechanical, the program attempts to find a solution based on the boundary conditions you’ve specified. However, not all problems will solve on the first attempt. This guide will show you how to use Ansys Mechanical’s troubleshooting tools to resolve failed solves and produce accurate results. 

How to Identify a Failed Solve

A failed solve is indicated by a red lightning bolt next to the solution. When this happens, Ansys generates error messages that explain what went wrong.

By clicking the Messages button, you can view a list of these messages categorized as Info, Warning, or Error. Warning messages should be read and understood, but they do not always indicate a problem. Error messages are generated when solving (or another action) fails to complete, and these messages explain what happened. You will need to address the cause of the error message before proceeding. Later in this article, we will recommend troubleshooting steps for the most common errors.

• Warnings: Indicate potential issues but may not affect the solve.
• Errors: Must be addressed as they prevent the solve from completing.

Using the Solution Information Worksheet

To further troubleshoot, search the Solution Information worksheet for terms like “error” or “reason for termination.” These messages provide specific details on why the solve failed. Understanding when the failure occurred (e.g., which load steps were completed) is also crucial for narrowing down the issue.

Use CTRL+F to search for “error” and read any error messages you find here. Sometimes there will be more detailed messages here. The last error message is usually the ultimate reason the solve failed.

Also search for the phrase “reason for termination.” If present, this line indicates exactly why the solve failed. Recommendations for interpreting some of the common reasons for termination are described later in this article.

Next, figure out when the solve failure occurred. It is important to know what load steps, if any, were completed before the solve terminated because that will narrow down the cause. For instance, if no time points were solved, the problem may be that the model is initially underconstrained. If the solve completed two load steps and failed on the third, you should look at any changes to the boundary conditions in the third load step.

Select Solution and view the Tabular Data as shown below. This shows that two substeps were solved, and the last successful step was t = 0.45s. The third row that shows Substep = 1e+006 represents the unconverged results and does not mean that t = 1s solved successfully. It can be very informative to create result plots set to the last converged substeps (t = 0.45s in the example below). The results at unconverged substeps are not physically meaningful and should generally not be used.

Once you understand the error that terminated the solve and the load step when the solve terminated, you can take corrective action to make the solve successful. The next steps will depend on the error encountered. For detailed advice, see DRD’s blog on troubleshooting steps based on the most common error messages.

Troubleshooting Tips 

• Check constraints: Ensure all parts are sufficiently constrained to prevent rigid body motion (RBM).
• Review boundary conditions: If the solve failed after completing a load step, inspect changes in boundary conditions.
• Create result plots: Use the last converged substep to identify potential issues. Unconverged substep results are not physically meaningful and should generally be ignored.

Want to dig deeper into advanced troubleshooting? Our blog on using Ansys Mechanical diagnostic tools covers additional tips to help you streamline your solving process

Metal additive manufacturing (AM) has surged in popularity due to its ability to create both prototypes and final production parts. However, this cutting-edge technology comes with challenges, primarily related to thermal strains, part distortion, residual stresses, and build failures. These issues arise from the intense heat transfer involved during the manufacturing process. Fortunately, Ansys Workbench Additive provides a solution by simulating these processes to help manufacturers predict and resolve these problems, ensuring successful part creation without costly trial and error.

The Challenges of Metal Additive Manufacturing

The thermal dynamics of metal additive manufacturing can cause significant issues, such as:

• Part distortion: As heat is applied during production, thermal expansion and contraction can lead to deformation.
• Residual stresses: Unrelieved stress within the material can lead to fractures or failures during or after manufacturing.
• Costly build failures: Without accurate simulation, manufacturers may waste time and resources on failed builds.

Ansys HFSS simulation tools empower RF engineers to design complete systems in a virtual environment, streamlining the entire development process. With the ability to tackle electrically large EM problems, engineers can efficiently design antennas, include platforms, and even simulate larger environments—all without extensive physical prototyping. This not only saves time but also accelerates the overall development timeline.

How Does Ansys HFSS Handle Electrically Large Problems?

Ansys HFSS offers a variety of solver types, enabling engineers to solve electrically large problems within practical timeframes and computing constraints. For smaller domains, HFSS’s Finite Element Method (FEM) provides high-fidelity solutions. However, as the problem space grows, a full-wave Method of Moments (MoM) solver becomes essential for reducing computational load. For even larger problems, HFSS utilizes ray tracing and physical optics methods, ensuring that even the most extensive simulations are feasible.

What is the Power of Hybrid Solutions in Ansys HFSS?

The real strength of Ansys HFSS lies in its hybrid solution capabilities. By combining FEM for smaller components and MoM or ray tracing for larger structures, HFSS offers a comprehensive approach to RF system simulation. This hybrid method ensures accuracy and efficiency, allowing engineers to simulate complex systems with unparalleled precision.

How Does High Performance Computing (HPC) Enhance Ansys HFSS

Ansys HFSS leverages High-Performance Computing (HPC) to push the boundaries of what’s possible in RF simulation. By parallelizing calculations across multiple CPUs and GPUs, HFSS can handle larger, more complex problems. These calculations can be distributed over a network of computers, enabling engineers to solve massive electromagnetic problems with unprecedented speed and accuracy, whether using local assets or cloud-based resources.

Why Choose Ansys HFSS for Large-Scale RF Simulations?

With its advanced solvers and HPC capabilities, Ansys HFSS is the go-to solution for RF engineers dealing with complex, electrically large problems. Whether you’re designing antennas, integrating platforms, or simulating vast environments, HFSS provides the tools you need to achieve your goals efficiently and effectively in a virtual space.

Wonder how else to optimize antenna simulations with Ansys HFSS? Continue reading our previous blog…

What Are the Key Benefits of Using Ansys HFSS for RF System Design?

When it comes to selecting the right engineering simulation tool for motor design and analysis, the choices can be overwhelming. Three powerful tools from Ansys—Motor-CAD, RMxprt, and Maxwell—are often at the forefront of the conversation. But how do these tools differ, and more importantly, how do you determine which one to use for your specific project?

Let’s break down the features and strengths of each tool to help you make an informed decision.

Motor-CAD: Multiphysics Simulation for Early-Stage Design

Motor-CAD is a versatile simulation tool designed for the initial sizing of electrical machines. Its multiphysics approach allows users to simulate electromagnetic, thermal, and mechanical behavior in the early stages of design. Here’s what sets it apart:

• Fast calculations and streamlined data inputs for rapid iterations
• Ability to explore a wide range of motor topologies
• High-fidelity 2D/3D analysis for advanced loss effect assessment
• Intuitive, template-based setup that simplifies design and reduces the need for specialized teams
• Electromagnetic-thermal-control coupling simulation, allowing for more comprehensive analysis

Motor-CAD is ideal for projects that require fast prototyping with a detailed focus on how advanced loss effects will impact the overall design. It also integrates smoothly with Ansys Maxwell and other physics solvers for more in-depth analysis as the design progresses.

RMxprt: Analytical Tool for Fast and Efficient Design

RMxprt is designed to provide quick analytical solutions for rotating electrical machines. This tool is best suited for the initial design workflow, offering:

   • Fast analytical results to get a quick overview of design feasibility

   • Automatic generation of both 2D and 3D Maxwell-ready models

   • A robust set of design information early in the process, enabling a seamless transition to more detailed simulations

If speed and simplicity in the first steps of motor design are a priority, RMxprt can quickly deliver a reliable design ready for more detailed simulations in Maxwell.

Maxwell: Advanced Electromagnetic Field Simulation

Ansys Maxwell is the go-to solution for detailed electromagnetic and electromechanical analysis. It features:

• • •     •  Customizable modeling for various electromagnetic devices
    •     •  Automatic adaptive meshing for accurate field simulation
    •     •  Advanced high-performance computing technology for simulations
  • • Maxwell excels when you need a detailed, high-fidelity simulation of electromagnetic fields and their interactions within electromechanical systems. It’s particularly useful when your design is transitioning from initial prototyping to comprehensive validation.

Each tool brings something unique to the table. Here’s a quick summary:

• Choose Motor-CAD when you need a multiphysics approach and want to explore various motor topologies and advanced loss effects in the early stages.

• Choose RMxprt when you need fast, analytical results and a seamless transition into more complex simulations.
• Choose Maxwell when your design requires detailed electromagnetic field analysis and a deeper understanding of coupled-physics behavior.

Learn More: 

Are you ready to take your motor design process to the next level? Watch our recent webinar, where we’ll dive deeper into Motor-CAD and explore its unique features that make it a leader in the field. 

With the rapid increase in devices that rely on wireless communication and data transfer, RF engineers face challenges far beyond analyzing the performance of a single antenna. Modern devices often incorporate multiple antennas, each operating within specific frequency bands. This complicates the RF engineer’s role, expanding their task from understanding the behavior of a single antenna to managing the interactions of multiple antennas on the same platform. The coupling effects between these antennas must be considered, particularly when RF engineers are integrating third-party antenna designs rather than creating them from scratch.

What advantages does Ansys HFSS offer for multi-antenna and large problem space design?

Ansys HFSS is a powerful tool that provides several advantages in tackling the challenges associated with multi-antenna systems. It features a robust parametric antenna design toolkit and a comprehensive component library. This allows antenna designers to either start from a unique design or use an approximate model for system integration and placement studies. Moreover, HFSS’s ability to create “Encrypted 3D Components” enables designers to incorporate high-fidelity models from third-party suppliers into platform simulations without revealing proprietary design information, ensuring accurate RF simulations.

How does HFSS handle the complexities of electrically large problem spaces?

One of the standout features of Ansys HFSS is its hybrid solve technology, which combines finite element (FEM), method of moments (MoM), and shooting and bouncing ray (SBR+) solution domains within a single simulation. This technology is particularly effective in solving electrically large problem spaces, such as those involving multiple antennas and platform integration. By leveraging this technology, RF engineers can efficiently simulate complex scenarios where multiple antennas interact with the placement platform, leading to more accurate and efficient design processes.

How do RF engineers mitigate crosstalk and spurious emissions in multi-antenna systems?

In multi-antenna systems, RF engineers must address issues like crosstalk and spurious emissions, which can occur due to the proximity of antennas on the same platform. Solutions may include optimizing antenna placement, applying tuned filters, adjusting radio channels, or modifying antenna architecture. Ansys HFSS allows engineers to calculate coupling coefficients between antennas with the platform in place, accurately accounting for the constructive and destructive field effects caused by the platform’s presence. These calculations are crucial for optimizing the overall system performance.

What role does Ansys EMIT play in optimizing multi-antenna systems?

Ansys EMIT is a powerful antenna system simulation tool that utilizes the coupling coefficients calculated by HFSS to predict the performance of multi-antenna systems. EMIT’s radio model library, along with feedline components such as filters, can be employed to optimize system performance and address Co-site Interference issues. By conducting these optimizations in a virtual environment, RF engineers can refine their designs before moving on to physical prototyping, saving time and reducing costs.

How do HFSS and EMIT contribute to cost-effective RF system design?

Watch now

Webinar 2: How Do You Simulate Multi-Antenna Systems and Large Problem Spaces with Ansys HFSS?

Watch now

Webinar 3: How Can You Optimize Ansys HFSS Performance with High-Performance Computing (HPC)?

Watch now 

What Makes Antenna Design and Wave Propagation So Complex?

The physics of wave propagation from an antenna is inherently a 3D phenomenon, and as such the engineering calculations underpinning or describing these devices can be quite difficult to formulate in an analytical form. Ansys HFSS facilitates solution of the full-wave electromagnetic field problem in any arbitrary 3D geometry by way of a conformal finite element method. Furthermore, adaptive mesh procedure employed by Ansys HFSS results in the most accurate solution for the lowest computational cost required to resolve the propagating field solution.

Ansys HFSS can be used to predict the behavior and performance of virtually any radiating antenna structure. This fact, coupled with the powerful RF-centric antenna parameter focused post-processing features, allows the antenna designer to fully embrace the approach of “virtual prototyping” and optimize antenna performance in the virtual space, prior to physical prototyping.

How Does Platform Placement Affect Antenna Performance?

Stand-alone antenna behavior is not the sole concern of many RF engineers. Even if the RF engineer is not designing an antenna from concept, antenna performance when placed “on platform” can significantly deviate from the published antenna specifications provided by the antenna manufacturer. The antenna loading and field warping resultant from the radiating or receiving devices proximity to larger platform structures must be taken into account when devising the RF system performance. In addition to antenna component design, the effects of platform placement can be predicted with equal accuracy to the antenna design problem using Ansys HFSS. The large bodies associated with the platform can be included in the simulation. For electrically large platforms, Ansys HFSS can also incorporate “hybrid field solution” methods such that less computationally intense approaches such as Method of Moments (MoM) and/or ray tracing/physical optics approaches can also be used on large domains of the computational space.

By utilizing a virtual prototyping approach in the RF platform design workflow, Ansys HFSS allows for compressed design cycles, fewer design iterations, and reduced physical prototyping iterations. Ultimately, this translates to a reduced development cost.

What if you have many antennas near each other? Will they interfere with one another?  Continue reading on our following blog….

Ready to Deepen Your Understanding? Join Our Three-Part Webinar Series!

In this series, we’ll cover:

Webinar 1: How can you effectively design and simulate antennas with Ansys HFSS? Watch now 

Webinar 2: What strategies can be used for simulating multi-antenna systems and large problems? –

Date: September 10, 2024, Time: 9:00 AM – 9:45 AM (CDT)

Webinar 3: How can you optimize Ansys HFSS solver technologies? 

Date: September 17, 2024, Time: 9:00 AM – 9:45 AM (CDT)

Register now to secure your spot! By registering, you will receive confirmation for the first webinar immediately and reservation emails for subsequent sessions at a later date. Don’t miss this opportunity to gain valuable insights and optimize your antenna designs.

What is Ansys Forming?

Ansys Forming is an end-to-end tool for sheet metal manufacturing process simulation; it has truly redefined how sheetmetal forming is being done using our trusted LS-DYNA solver. It has a newly developed graphical user interface that allows engineers to easily, accurately and efficiently setup the simulation, solve the job and analyze the results. The advantage of our Ansys Forming software is that most of the parameters are already predefined and user is interactively guided through a streamlined step by step process. Ansys Forming only needs the knowledge of the sheetmetal forming process. In a nutshell, Ansys Forming is a one stop shop for all metal stamping needs and it offers an optimal performance delivering a good balance between speed and accuracy.

In Ansys Forming “Deep drawing” is the process we are trying to simulate. The forming process is typically performed on a press and the parts are formed between 2 dies as shown above. This is a time intensive process and the procedure requires machinery and specialized tools. Through Ansys Forming we are able to simulate gravity loading simulation, conduct formability analysis, account for springback prediction and compensation, conduct press and roller hemming, perform clamping simulation, account for hydroforming, etc. as shown on the graphic below. In Forming simulation, the desired shape is extracted through plastic deformation w/o undergoing any advanced machining processes such as milling. With Ansys Forming we can optimize the process before the actual tool is manufactured. It reduces the cost to manufacture the tools and reduces the time to market for OEM’s. It guarantees the manufacturability of the parts and ensures parts come out right the first time.

What are some common applications of Ansys Forming?

Most of the applications for Ansys Forming are found in the following industries ranging from Automotive OEMS, suppliers manufacturing fenders, doors, hoods and various parts and accessories of the automobile to Aerospace manufacturing various parts of the entire aircraft including wings, fuselage, etc. from Consumer appliances such as refrigerators and washing machines to food and packaging industry manufacturing cookware, canned products, etc. the application is quite widespread.

Join us on July 30, 2024, at 9:00 AM for our exclusive webinar and discover how Ansys Forming can revolutionize your sheet metal manufacturing process!