*Choosing an element type for a structural Finite Element Analysis*

Dr. Jody Muelaner, Ph.D. CEng MIMechE

When performing structural Finite Element Analysis (FEA), it is often advised that thin-walled parts should only be meshed using solid elements if it is possible to use at least three elements through the thickness. When this is not practical, shell elements are advised. What usually isn’t explained is that this advice is based on the use of first-order elements, which are rarely used in modern FEA software. When second, or even higher, order polynomial elements are used, good accuracy can often be obtained using a single solid element through the wall thickness. What is often more important, is the number of elements approximating tightly radiused curved geometry. There are also many cases where shell elements can dangerously underestimate stress in key features. Weâ€™re going to use a number of simple parts and mesh convergence studies to illustrate these issues and provide the understanding required to select appropriate element types.

**Element types**

Before getting into the examples, letâ€™s take a moment to review a few basics of FEA element types. FEA can be used to simulate a range of physics-based problems including heat transfer, fluid flow, and electromagnetics, but structural analysis is the most common application and this is what we will focus on.

Problems can be represented in either two or three dimensions. One example of a two-dimensional problem is a plate loaded in plane stress, perhaps with a stress raiser such as a hole. In such a case, differences in the stress through the thickness of the plate can be ignored and it doesnâ€™t actually matter how thick the plate is, provided the load per unit thickness is correct. Another example of a two-dimensional problem might be an axisymmetric pressure vessel. We wonâ€™t consider one dimensional problems since the issues are very different to those of three dimensional problems. For most designers, running simulations directly from CAD models, a three-dimensional analysis will be carried out.

For a three-dimensional analysis, the elements themselves may be one-dimensional, two-dimensional or three-dimensional. Beams and bars are examples of one-dimensional elements, these elements are represented as a line. Although they may have a cross section associated with them, this is only used to determine their cross-sectional area and, in the case of beams, their second moments of area. Although the element itself is one-dimensional, it exists within a three-dimensional model meaning that the element can connect to other elements, or have forces acting on it, from the x, y or z direction.

The two types of elements considered in this article are shells and solids. Although a first order shell element is two dimensional, it can transmit bending forces as well as plane stress, allowing multiple shell elements to approximate three-dimensional structures, it should not be confused with the planar elements used in a two-dimensional analysis. Shell elements can be triangular or quadrilateral. Solid elements can be either tetrahedral or brick shaped.

Elements are represented mathematically as a polynomial and therefore have an order corresponding to the order of the polynomial. A first order triangular shell element has three nodes, one at each corner, and stress and strain can only be linearly interpolated between the nodes. A second order shell element has midpoint nodes on each side, giving a total of six nodes. Second order elements are also known as quadratic elements and allow stress and strain to be approximated using a quadratic function. A second order shell element does not have to be flat, its geometry can also approximate a curved surface using this quadratic function. It is also possible to use higher order polynomials to more accurately approximate curved geometry or changes in stress through the element.

**Example 1: Flat rectangular plate loaded in bending
**The first example used to compare the results from solid and shell elements is a simple rectangular plate loaded in bending. This simple model enables the plotting of simulation accuracy against mesh size. The rectangular plate is modelled with an elastic support at one end, a roller support at the other end and a distributed load over the entire upper surface. These boundary conditions avoid singularities and put the maximum stress in the middle of the plate, away from the supports. The image below shows the plate meshed with shell elements, one with a very course mesh and the other with a very fine mesh. The plate was flat in its unloaded condition and the curvature shown is a scaled representation of the deformation under load.

The simulation was run with second order triangular shell elements, with first order tetrahedrons and with second order tetrahedrons. These are referred to as simply shells and solids. A baseline simulation with five second order solid elements through the thickness was taken as the reference value. Each result was compared with this reference to see the percentage error in maximum von Mises stress and maximum deformation. These results are plotted against the mesh size, as a multiple of the plate thickness, in the charts below.

The results show that, when second order solid elements are used, a single solid element through the thickness is just as accurate as a shell element. Even solid elements which are considerably larger than the plate thickness give good results, in these cases there was a single element through the thickness but it had a larger aspect ratio so its plane dimensions were larger than the plate thickness. For solid elements which were three or more times the plate thickness the accuracy started to decline. Shell elements only give a significant advantage when the mesh is very course, with elements much larger than the plate thickness. First order solid elements are considerably less accurate, even with a very fine mesh, and for course meshes with only a single element through the thickness they give completely unreliable results.

This simple example seems to indicate that using higher order elements, as is standard with modern FEA software, it is not necessary to have multiple elements through the thickness. A 2-mm mesh will give very good results for a 1-mm wall thickness.

**Example 2: Bent plate demonstrating element size relative to radius**

The second example uses a rectangular plate which is bent in the middle with a radius at the bend. It was modelled with a symmetry plane. One end has an elastic support and the other end has a tensile force applied. Because the plate is bent this tensile loading attempts to straighten the plate resulting in a peak stress at the bend. Only second order solid (tetrahedral) elements were used in this example.

This scenario was simulated with a range of parameter values. The plate thickness was maintained consistently at 1-mm but the radius was simulated at values ranging between 1-mm and 40-mm. For each radius a reference simulation was run with four second order solid elements through the thickness and further refinement so that in the region of the bend, the elements were no more than 1/20th of the bend radius. Results were compared for global mesh sizes varying from 0.25 wall thickness (four cubic elements through the thickness) to three times the wall thickness.

The below chart shows the accuracy of each simulation plotted against the mesh size as a multiple of the wall thickness. It is clear that there is no correlation between mesh size and wall thickness. This remains true for elements up to three times larger than the wall thickness.

The next chart shows the accuracy of each simulation plotted against the mesh size as a multiple of the radius. In this case there is a clear trend. When the mesh size is 1/20th of the radius the errors were never more than 1%, however, when the elements were larger than the radius the errors were always more than 10%. For meshes that are 1/10th of the radius then errors are never more than 6% and typically much better than that.

**Conclusions**

The conventional advice for the meshing of thin walled structures is that shell elements should be used unless a solid mesh is able to achieve several elements through the wall thickness. With modern higher-order polynomial elements this advice is no longer relevant. A single solid element through the thickness will achieve results that are just as accurate as a shell element. This means that the considerable effort required to prepare geometry for shell meshing can be avoided. A more important consideration seems to be achieving a fine mesh to accurately model tightly curved sections of a thin walled structure, especially if high stress occurs at these areas. This indicates that curvature based meshing is a very useful tool for thin walled structures. Using higher-order solid elements together with a curvature based meshing algorithm, modern FEA software is able to achieve highly accurate results with very little pre-processing of geometry. However, caution must always be observed as there are many other ways that FEA can produce spurious results. Verification by physical testing remains highly advisable.