Updated: Dec 9, 2020
Have you ever found yourself wondering which Abaqus element formulation is most suitable for your analysis? With the vast options provided within Abaqus Standard and Abaqus Explicit, novice and experienced users alike often find themselves asking this very question, and for good reason: selecting the appropriate element type with respect to your simulation objectives is vitally important for obtaining accurate results. In this blog series, we aim to highlight some of the key aspects one should consider when determining the optimal Abaqus element formulation for a given analysis.
Article 2: Understanding Element Dimensionality in Abaqus
As we discussed in Article 1 of our Element Selection in Abaqus blog series, comprehending the fundamentals of element behavior is critical when choosing the appropriate element type(s) for your analysis. However, in many cases, there may be several acceptable finite elements capable of representing the physical phenomena being simulated. So, which element should you use?
As a general rule, most experienced analysts will tell you that you should select the simplest element that is capable of capturing the physics being simulated. With that in mind, the first place to start when planning your finite element model is by determining the appropriate dimensionality. The Abaqus element library contains the following for modeling a wide range of spatial dimensionality:
One-dimensional elements (1D)
Two-dimensional elements (2D)
Three-dimensional elements (3D)
Before we delve into the details, it is first important to differentiate between spatial dimensionality and element dimensionality. Although the formal nomenclature may differ based on your solver of choice, for the sake of this discussion, spatial dimensionality will refer to the actual space being simulated in your Finite Element Analysis (FEA) model; element dimensionality, on the other hand, refers to the number of dimensions required to define a specific element type. As an example, let us consider a traditional B31 Beam element in Abaqus: the element dimensionality is 1D since the element is defined by only two nodes (a vector); however, the spatial dimensionality is 3D because the element section properties account for the cross-sectional dimensions. To further drive home this point, let us next consider a traditional triangular shell element (S3): the element dimensionality is 2D since the element’s nodes all lie on a single plane; however, much like the example above, the section properties define the shell element thickness, which means that the spatial dimensionality being simulated is actually 3D.
One-dimensional elements (1D), sometimes referred to as “link” or “line” elements, can be used to transmit loads or fluxes along the length of the element (in either two- or three-dimensional space). Commonly used for modeling long-membered structures, one-dimensional elements are geometrically defined by two nodes; the cross-sectional area, or shape, is provided mathematically via user input and element behavior can be calculated accordingly. One-dimensional elements often offer a convenient means for modeling large structures (e.g. a truss bridge) as they provide an exceptional representation of the system stiffness and displacement as well as an accurate understanding of global stresses at a minimal computational cost. However, it should be noted that one-dimensional elements are not suitable for modeling complex geometries or predicting localized stresses (such as those occurring at a stress concentration, like a notch or hole).
Two-dimensional elements (2D), as indicated by the name, are represented geometrically in two dimensions and can be either triangular or quadrilateral. Triangular elements, of course, will be comprised of three corner nodes while quadrilateral elements will contain four corner nodes (with three or four mid-side nodes, respectively, if they are second-order elements). Although the element dimensionality is always planar, these elements can be used to represent either 2D or 3D space. As discussed above, the traditional Abaqus shell element is a good example of 2D element dimensionality being used to represent 3D spatial dimensionality.
More traditionally, though, the nomenclature “two-dimensional elements” has been used to refer to elements that are used to simulate 2D space. The most common of these elements are plane stress and plane strain elements, which we alluded to in Article 1 of this blog series and discuss in slightly more detail below:
Plane Stress Elements
Used when thickness is small relative to in-plane dimensions
Stresses are a function of planar coordinates alone
Out-of-plane normal and shear stresses are equal to zero
Plane Strain Elements
Used to represent thick plates or sections
Strains are a function of planar coordinates alone
Out-of-plane normal and shear strains are equal to zero
So what does this actually mean? Simply put, plane stress elements can be used to represent very thin structures because the out-of-plane contribution to stress is assumed to be insignificant; as a result, the three-dimensional problem can be simplified to a two-dimensional problem in which the stress state is represented entirely by the in-plane stress. Conversely, plane strain elements can be used to represent thick structures because the out-of-plane strain is assumed to be constrained by the bulk material and, therefore, has a negligible impact on the overall strain state (which, once again, reduces a three-dimensional problem to a two-dimensional approximation).
Three-dimensional elements (3D), often referred to as solid elements, are the easiest to conceptualize because the element dimensionality and the spatial dimensionality are one and the same. Modeled in the global X,Y,Z space, solid elements are often used when the geometry or loading conditions are too complex to be adequately represented with fewer dimensions. Because three-dimensional elements exist in 3D space, the resulting stress and strain states are also three-dimensional. In other words, when it comes to three-dimensional elements, what you see is what you get (mostly).
Cylindrical elements are a special class of solid elements which are used to model structures with circular or axisymmetric geometry that are subjected to non-axisymmetric loading. Because cylindrical elements capture the curved shape of circular objects, they are able to provide more accurate predictions than traditional linear, solid elements with substantially less mesh refinement. A classic use case for cylindrical elements can be observed in the tire industry: footprint and steady state rolling analyses commonly utilize cylindrical elements because the solution over most of the tire is nearly axisymmetric (outside of the contact zone). This allows analysts to use a relatively coarse cylindrical element mesh that is much more economical than conventional solid elements.
Axisymmetric elements, as the name suggests, can be used to model bodies which are rotationally symmetric about a central axis; but, conventional axisymmetric elements can only be used under axially symmetric loading conditions (although it is worth noting that advanced element formulations do exist for modeling axisymmetric geometry subjected to nonlinear, asymmetric deformation). Due to the loading and geometric axial symmetry, the 3D spatial dimensionality of a body can be modeled using 2D element dimensionality. Put more simply, because the stresses are independent of rotational angle for axisymmetric problems, such models are comprised of a single two-dimensional plane (element dimensionality); however, the solution provided represents three-dimensional space (spatial dimensionality). A common example of an axisymmetric problem is a thick-walled, cylindrical pressure vessel subjected to internal pressure.
Although the number of variables which must be considered when selecting an appropriate finite element in Abaqus may initially seem overwhelming, the process is actually quite simple and, over time, becomes second-nature. By carefully considering the physics of what you are simulating as well as the runtime constraints and desired analytical outputs, there are a number of “rules” which CAE analysts can employ for modeling various phenomena. Stay tuned for future installments of our Element Selection blog series for more tips and tricks that can be used when determining the elemental makeup of your Finite Element Analysis (FEA) model!
Whether you’re an experienced Abaqus user or a complete beginner, Fidelis can help you get the most out of the software with bespoke support and fully integrated simulation solutions. Call or email us today to learn more about our offerings.