Featured Case StudyThe Norsea Gas Terminal in Northern Germany plays a vital role in the connection of pipeline systems coming from the North Sea to the natural gas distribution network throughout Germany. Built in...Stay
- ANSYS Software
Featured Case StudyRelying on ANSYS Composite PrepPost helped EADS Innovation Works to develop lightweight composites in aircraft design. ANSYS Composite PrepPost provided simple pre- and post-processing of composite...Stay
- Resource Library
- News &
Adopting Adaptive Meshing
If you perform nonlinear structural finite element analyses with large displacements, then you are probably very familiar with the “element has become highly distorted”, or similar, warning message. This warning indicates that due to excessive deflections, the shape of the elements in the mesh have significantly changed from their original shape, and this distortion is reducing simulation accuracy and causing convergence issues, eventually leading to analysis termination. This behavior is common when modeling soft materials like rubber, simulations of metal forming, or when elements accumulate plasticity, creep, damage, or even cracking simulations. A simple example of a highly distorted mesh due to excessive deformation is shown in Figure 1.
Figure 1: Highly Distorted Mesh in Metal Forming Model
This situation is especially frustrating, since it typically takes a lot of time and effort to create a well-shaped mesh in complex parts, and yet your original awesome mesh ends up distorted, and the analysis often errors out before completion. So, it’s back to the drawing board, perhaps starting over with trying to create a mesh with element shapes that might anticipate the upcoming distortion. Wouldn’t it be nice if finite element codes could just adjust the mesh on the fly during the analysis to keep the elements from distorting too much?
Finite element codes with mesh nonlinear adaptivity features will automatically modify the mesh according to specified criteria during solution, requiring no user-intervention. There are typically two different approaches for modifying the mesh:
1. Element splitting with morphing.
2. General remeshing.
Element splitting is performed by simply dividing the original elements into elements having some fraction of the edge length of the original elements. This type of mesh refinement is typically not used to repair a distorted mesh, but is more commonly used to improve solution accuracy and capture local behavior in more detail. An example of mesh adaptivity applied to the modeling of rubber is illustrated in a previous blog. In some cases, element splitting is followed by morphing to try to improve the element shapes. Examples include local necking, local buckling, and high stress concentrations. Figure 2 shows an example of a crack simulation where the mesh is split to obtain a finer mesh in the region near the crack tip.
Figure 2: Element Splitting Near Crack Tip
General remeshing is performed by completely eliminating the existing mesh in the selected region, and then creating an entirely new mesh to improve quality. This technique is preferred when element distortion is causing convergence issues. An example is shown in Figure 3, showing the same model in Figure 1 employing adaptive meshing using the general remeshing approach.
Figure 3: General Remeshing of Metal Forming Model
There can be several different criteria that govern how, when, and where the mesh is updated in an adaptive meshing application. For example, in ANSYS, the four main criteria are:
4. Mesh-quality based.
Energy-based criteria track the magnitude of the strain energy to determine when element splitting should occur. This approach is used to refine meshes to achieve better accuracy in regions of high stress concentrations. Position-based criteria are used in cases of very large deformations where it is not known initially which elements should be remeshed, such as may be the case for a rubber seal. A region in global coordinate space is identified, and any element that falls within that region is included in the adaptive meshing. Contact-based criteria use mesh adaptivity to split contact elements based on the specified number of contacting elements to ensure accurate results at contact interfaces. This approach could automatically ensure a fine mesh in a contact region as discussed in a previous blog on obtaining accurate contact stresses. These three criteria all typically use the element splitting technique.
Mesh-quality criteria base the remeshing on the element’s maximum corner angle or the element skewness. General remeshing is necessary to perform adaptive meshing for these cases.
There are significant challenges to incorporating and performing nonlinear adaptive meshing. Since the application is a nonlinear analysis, the element stiffness matrices are not constant as in a linear elastic problem, so in addition to creating the new mesh, the updated stiffness characteristics and previous load/stress/strain history must be mapped from the previous to the new mesh. At each point in the analysis where remeshing occurs, a restart is required since the analysis has been interrupted. And, as is the case with any finite element procedure, the adaptive meshing settings, such as the input values for the various criteria, as well as the frequency and location for remeshing, may not provide an acceptable and successful solution without some tweaking or iterating on the input quantities.
Post-processing is also more difficult since each time adaptive meshing is performed, a new mesh is used, and thus nodal results cannot be tracked from the start of the analysis. In some codes such as LS-DYNA, different result files are generated for each mesh. In other codes, like ANSYS, one result file is maintained, but displacements represent those from the start of each new mesh.
However, even though nonlinear adaptive meshing is not foolproof, it can still be used to obtain more accurate results, and can even get hard-to-converge problems to complete, for many cases. A recent example is an analysis of a metal forming billet problem that we use in some of our nonlinear finite element training courses. A rectangular billet is compressed using a rigid die, resulting in plastic strains in excess of 90%. Without adaptive meshing, it is very difficult to get a complete solution, and even partially-solved solutions can generate very different results based on minor changes to the analysis settings, due to distorted elements forming under the die. Activating mesh-quality based nonlinear adaptive meshing generates a complete solution with a well-shaped mesh throughout, as shown in the animation in Figure 4.
Figure 4: Animation of Metal Forming Analysis with Mesh-Quality Based Adaptive Meshing
Do you use nonlinear adaptive meshing in any of your applications? If so, please share your experiences in the comments.
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Chris Mesibov
by: Peter Barrett
- Engineering Consulting
- ANSYS Software & Support
- ANSYS Training
- About Us
- News & Insights
1579 Straits Turnpike Suite 2B
Middlebury, CT 06762
- ANSYS Software