## Defining Element Types in Abaqus

There is a phrase among finite element analyst user community. Those who have been in the industry since a while must have heard of it at some point in their career.

**GARBAGE IN….GARBAGE OUT**

It means that if the data being fed into the input deck is not correct or appropriate, the solver is very likely to give incorrect results, and that’s if it does not fail with errors. Many of us believe that getting some sort of result is better than getting fatal errors, which is not correct. **Fatal errors give clear diagnostic messages to the user that allow him to correct the input deck.** However, getting erroneous results sometimes makes a user feel that the simulation has been successful even though the results may be far from reality. Such situations are hard to predict and correct, as the underlying cause is not clearly visible.

**One such situation arises when the user inadvertently chooses an element type that is not capable of capturing the actual physical behavior of the part or assembly with which the element is associated.** The incompatibility may lie with respect to element material, element topology, element dimension, or the type of output associated with the element. The objective of this post is to highlight the capabilities and limitations of some lesser known element types available in the Abaqus element library to promote their proper usage.

# Planar elements

These elements are further classified as either *plane stress* (**CPS**) or *plane strain* elements (**CPE**). The plane stress elements are used to model thin structures such as composite plate. These elements must be defined and can deform only in X-Y plane. For these types of elements:

s*zz *= t *xz *= t *yz *= 0

The plane strain elements are used to model thick structures such as rubber gaskets. These types of elements must be defined and can deform only in X-Y plane. For these types of elements:

e*zz *= g*xz *= g*yz *= 0

# Generalized plane strain elements

These elements are referred to as *CPEG elements* in the Abaqus element library. They are used to model structures bounded by two planes that are either parallel or at an angle to each other. The planes can move with respect to one another. The thickness gradient in X-Y plane is assumed to be small.

# Axisymmetric elements

Abaqus has a library of *axisymmetric continuum elements* (**CAX**). These elements are good to model axisymmetric structures subjected to axisymmetric loadings. The (**r**) and the (**z**) directions coincide with the global X and Y axis respectively. The structure is assumed to be symmetric about the (**z**) axis. The point loads are defined as the total loads integrated around the circumference and the distributed loads should be provided as loads per unit surface area.

This category of elements also contains *axisymmetric elements with non-axisymmetric response* (**CAXA**). These elements are suitable to model structures that are symmetric in geometry but are subjected to asymmetric loadings, such as threaded connectors. These elements are currently not supported by Abaqus CAE.

Abaqus also has *axisymmetric continuum elements that can model torsional, as well as axisymmetric deformation* (**CGAX**). These elements are for axially symmetric structures that can twist about their symmetry axis. The elements can be used in nonlinear analysis that include, e.g., finite rotations. A typical application is the inflation loading on a tire. A circumferential component of deformation arises due to the anisotropic nature of the tire’s construction. The problem remains axisymmetric: the deformation does not vary as a function of position along the circumference. These elements are supported by Abaqus CAE.

# Cylindrical elements

*Cylindrical elements* (**CCL**) are intended for modeling structures that are initially circular but are subjected to general, non-axisymmetric loading. A primary advantage is that a coarse, yet accurate discretization of the structure is possible. That is illustrated in this tire model, where each cylindrical element spans nearly 90 degrees. Cylindrical elements can be considered as true continuum elements defined in 3D space, and they are fully compatible with other continuum elements. Regular solid elements can be connected directly to the nodes of the cross-sectional plane of cylindrical elements. For example, any face of a C3D8 element can share nodes with the cross-sectional faces (faces 1 and 2) of a CCL12 element. All material models as well as geometric non-linearity is supported by CCL elements.

# Infinite elements

*Infinite elements* (**CIN**) are used in conjunction with standard elements to model very large or infinite structures. A family of planar, axisymmetric and three dimensional elements are available. These elements are not supported by the Abaqus CAE pre-processor.

**BEST PRACTICES**

It is often required to avoid some non-physical phenomenon taking place in the analysis as a result of numerical instability. These include, but are not limited to, phenomena such as hour glassing, shear locking, volumetric locking, and checker boarding. At the same time, it is often required to select elements that can precisely capture complex material behavior, such as full incompressibility often encountered in rubber materials and severely plastic deformations. Accurate contact stresses at surfaces are often desired as well. The table below shows the recommended element types, as well as element types that should be avoided for a certain classes of problems.

Leave a comment if you have any questions or additional thoughts. We are here to help.