In this course, we discussed the various tools and techniques used to obtain a numerically accurate result while performing a stress analysis. Let’s summarize the key points from each lesson.


Specifying an Appropriate Element Size for Stress Analysis 

  • Specifying an appropriate element size for finite element meshes is critical to obtaining accurate results in a reasonable amount of time.
  • High gradients through the element of derived quantities such as stress or strain is a good first indication that the element size may be too large.
  • Multiple tools can be used to specify the element size to achieve the typical end goal of a mesh-independent solution, where the results do not change with further increases in mesh density.
  • While the proper element size may not be known before the solution, there are multiple postprocessing settings available (such as results averaging and nodal differences) to check the appropriateness of the element size specified.
  • Mesh refinement could be done by using not only various manual mesh size controls, but also through more automated ways such as convergence or parameterization.


Understanding the Importance of 3D Element Shapes and Order 

  • A geometry can be meshed with elements of various shapes and orders. Hexahedral and tetrahedral elements are the most widely used element types.
  • Shape functions of an element determine its order. Linear elements have nodes only on the vertices of an element, while second-order elements also have mid-side nodes.
  • Linear tetrahedral elements should be avoided in linear stress or dynamic analysis as they suffer from shortcomings such as being constant strain elements and being prone to volumetric and shear locking.
  • Tetrahedral elements can be used to define a finer mesh in the regions of interest and a coarse mesh away from it as it can smoothly transition from a coarse mesh to a finer mesh.
  • Ansys Mechanical uses second-order elements by default and meshes sweepable bodies with hexahedral elements and complex geometries with tetrahedral elements. These default options suffice for most stress analyses.


Understanding and Dealing with Artificially High Stresses 

  • Understanding situations where artificially high stresses arise and addressing them can better equip us to utilize simulation tools and interpret results properly.
  • Typical cases where we generally observe artificially high stresses are from point loads and constraints, re-entrant corners, over-constrain of the model, and sharp corners in contact.
  • Artificially high stresses can grow without bounds as the mesh is refined, which can lead to confusion as to what result should be reported.
  • In structural finite element analysis, displacement and rotation values at each node will always converge to a unique solution as the mesh is refined, but stress and strain values may not converge to a unique solution with a finer mesh.
  • Cases of high stress such as (stress risers/concentrations) should not be ignored, and these cases should not be confused with the stress singularities we might see in the case of a re-entrant corner.


Obtaining Accurate Stress Using Surface Coating

  • The finite element method is generally quite accurate in predicting body stress when a model is well-defined, but stress on a surface may need special treatment due to the extrapolation that is used to obtain stress value on the nodes.
  • Surface coating technology is an efficient way to obtain accurate surface stresses because it places shell elements of a specified material on the selected face(s) of the model.
  • By choosing the appropriate options, the surface coating elements can also be used to model real coatings where thickness is needed.
  • Surface coating can efficiently improve the result accuracy in cases where a coarse mesh in the normal-to-surface direction is experiencing inaccurate surface stresses due to extrapolation.


Using Adaptive Convergence with Ansys Mechanical

  • In adaptive convergence, the system response converges to a repeatable solution with decreasing element size for a well-defined model. Hence, the result no longer changes with further mesh refinement.
  • Adaptive convergence requires the problem to be solved multiple times with different levels of mesh discretization (i.e., it starts with a coarser mesh and moves to a more refined mesh).
  • Adaptive convergence is a tool to help us understand the influence of mesh in the numerical accuracy, but it cannot compensate for incorrect input, such as improper boundary conditions.
  • Adaptive convergence should be used as a learning tool to understand where local mesh controls are needed or to verify if the current mesh is sufficient, as this will help to define a better mesh for future models to ensure the numerical accuracy - or mesh independence - of our solution.


Performing Submodeling in Ansys Mechanical

  • Submodeling is a method used in finite elements to perform accurate analysis in critical regions or regions of interest without solving the whole model hence, with better efficiency.
  • Submodeling is based on St. Venant’s principle, and it can be used for both structural and thermal analyses in Ansys Mechanical.
  • Submodeling leads to easier parametrization of the design, which comes along with local design changes. It also helps in modeling localized nonlinearity that might not have been captured in the global model.
  • While using submodeling, care must be taken in placing the cut boundaries away from regions of sharper gradients.
  • Submodeling can also be used for running various design iterations by including smaller details such as fillets of different radii.