What is Convergence in Finite Element Analysis?
A typical engineering design involves prediction of deflections/displacements, stresses, natural frequencies, temperature distributions etc. These parameters are used to iterate on material parameters and/or geometry to optimize their behavior. Traditional methods, like hand calculations, involved idealization of physical models using simple equations to obtain solutions. However, these approximations oversimplify the problem and an analytical solution can only provide conservative estimates. Alternatively, FEM and other numerical methods are meant to provide an engineering analysis that takes into account much greater detail — something that would be impractical with hand calculations. FEM divides the body into smaller pieces, enforcing continuity of displacements along these element boundaries. More information on “how FEM works” and “how to learn FEM” can be found in the earlier SimScale articles.
For those using FEM, the term “convergence” is often heard. Most linear problems do not need an iterative solution procedure. Yet, mesh convergence is an important issue that needs to be addressed. Additionally, in nonlinear problems, convergence in the iteration procedure also needs to be considered. So what does this mean? In this article, we address issues that are related to this term.
To read a more general article about FEA, we’d like to refer you to our SimWiki where we discuss the big topics in Engineering Simulation in detail.
Mesh Convergence: h- and p-refinement
One of the most overlooked issues in computational mechanics that affect accuracy, is mesh convergence. This is related to how small the elements need to be to ensure that the results of an analysis are not affected by changing the size of the mesh.
Fig 01: Convergence of quantity with increase in degrees of freedom
As shown in Fig. 01, it is important to first identify the quantity of interest. At least three points need to be considered and as the mesh density increases, the quantity of interest starts to converge to a particular value. If two subsequent mesh refinements do not change the result substantially, then one can assume that the result has converged.
Fig 02: Mesh refinement of a structure
Going into the question of mesh refinement, it is not always necessary that the mesh in the entire model be refined. St. Venant’s Principle enforces that the local stresses in one region do not affect the stresses elsewhere. Hence, from a physical point of view, the model can be refined only in particular regions of interest and further have a transition zone from course to fine mesh. There are two types of refinements (h- and p-refinement) here as shown in Fig. 02. h-refinement relates to the reduction in the element sizes while p-refinement relates to increasing the order of the element.
However, here it is important to distinguish between geometric effect and mesh convergence. Especially when meshing a curved surface using straight (or linear) elements will require more elements (or otherwise mesh refinement) to capture the boundary exactly. As shown in Fig. 03, mesh refinement leads to significant reduction in errors.
Fig 03: Reduction in error with h-refinement of the curved surface
Such a refinement can allow an increase in the convergence of solutions without increasing the size of the overall problem being solved.
Convergence in Presence of Singularities
After reading the above section, it feels safe to assume that once the stress converges in a particular part of the structure, using the same element size elsewhere should lead to converged solutions. However, this is not a valid assumption.
Most models have corners, both internal and external, where the radius is assumed to be zero. This is also the case in the presence of cracks. Here the stresses are theoretically infinite. Now can you guess why airplane windows do not have corners but are rounded at the edges?
Fig 04: Increase in stresses, towards infinity, with mesh refinement around a singularity
In the presence of the singularity, the mesh needs to be refined around it. However, the more the mesh is refined, the more the stress continues to increase and tend towards infinity, as shown in Fig. 04.
Hence, in the presence of fillets, it is generally more reasonable to assume an actual radius and then refine the region using a sufficient number of elements. For more details on mesh singularities, we could recommend a recent article on the SimScale blog titled “Mesh Size Influence on Mechanical Stress Concentration”.
Convergence During Locking
One of the other commonly encountered nonlinear problems is related to locking — namely, the volumetric and shear locking effects. Volumetric locking is commonly encountered in problems related to incompressibility in hyperelasticity and plasticity problems. Alternatively, shear locking is generally encountered in bending dominated problems.
Fig 05: Standard problem with internal pressure being considered for testing volumetric locking
Fig. 05 shows a standard problem to test incompressible effects — here a small pipe with internal pressure is considered. Such applications are commonly found in various environments, including human arteries. Only a quarter of the model needs to be considered due to the symmetry in the problem. Now, as the Poisson ratio tends to 0.5, the bulk modulus tends to infinity and thus the material demonstrates incompressibility. Here, second order elements are preferred or, in other words, a p-refinement is required. Fig. 06 shows the behavior of different element types with an increase in the Poisson ratio.
Fig 06: Convergence in volumetric locking problems.
Similarly, Fig. 07 shows a simple beam bending problem where a moment is being applied on the free end. The deflection at the free end of the beam is considered, and this problem even has an analytical solution for comparison. Fig. 07 shows the convergence of the deflection for different kinds of elements.
Fig 07: Shear locking in beam bending problem and convergence for different elements
How to Measure Convergence
So now that the importance of convergence has been discussed, how can convergence be measured? What is a quantitative measure for convergence? One way to measure it would be to compare with analytical solutions or experimental results.
Fig 08: Definition of errors
As shown in Fig. 08, several errors can be defined for displacement, strains, and stresses. These errors could be used for comparison, and they would need to reduce with mesh refinement. However, in a FEM mesh, the quantities are calculated at various points (nodal and Gauss). So in this case, where and at how many points should the error be calculated?
Fig 09: Error norm and comparison with the element size
Hence, alternatively, norms are defined such that the averaged errors over the entire structure or part of the structure can be calculated. As shown in Fig. 09, the error norms can also be compared to the size of the element. Here “c” is a constant of proportionality, while “h” is the element size, as defined in Fig. 09. Hence, several errors such as L2 and Energy error norms can be defined as below:
However, in real practical applications, a nondimensional version of the same is more useful to assess the actual degree of error. Therefore, here the root-mean-square value of the norms, as defined below, is used to plot the reduction in error.
The final topic is, at what rates do these errors ideally decrease. If we are using a linear or quadratic or cubic elements, how does one judge if the error is decreasing at the right speed or otherwise the quality of algorithms coded? As shown in Fig 10, the L2-norm error decreases at the rate of p+1 and energy-norm at the rate of p.
Fig 10: Convergence rates for different error norms
I hope this article has given a comprehensive overview of convergence, convergence rates and ways to judge these aspects in an FEA simulation. Convergence plays an important role in the accuracy of solutions obtained using numerical techniques like FEA and needs to be comprehensively analyzed in any given problem.
Want to learn more about industrial applications of FEA? This case study shows a stress analysis of a wheel loader arm performed with the SimScale simulation platform.