Inventor Nastran has three different types of finite elements that can be applied to a model. Each element type has its own set of pros and cons. They can also be combined to form an efficient and accurate stress analysis solution.
At a high level – in a similar way that a CAD model represents the digital version of your part or assembly for visualization, assembly instruction, or dimensioning – the elements represent the digital version that is to be analyzed. The various types of elements can be categorized by their shape – being either volumetric (solid elements), planar (shell elements), or lines (bar, truss, beam, pipe, etc.).
The image below shows a single solid element. At the vertices of the adjacent sides, where the heavy black dots are shown, these would be the nodes of the element. The nodes are where the degrees of freedom (DOFs) are defined. The DOFs of a node represent the possible movement of this point due to the loading of the structure. The DOFs also represent which forces and moments are transferred from one element to the next.
The type of element being utilized will characterize which DOFs a node has – up to six (three translation, three rotation), as shown below. Some analysis types only have a single DOF at a node, such as temperature in a thermal analysis.
Solid elements are used to mesh volumes of CAD parts – generally parts that might be considered chunky when considering their length to width to height. Typically machined and cast parts will be idealized as solid. Telling the program to generate a solid mesh of a CAD model can result in hundreds, thousands, or even a couple hundred thousand smaller solid elements to fill the volume.
Linear tetrahedron elements (image in red below) are mathematically more stiff and best to use for trend studies, where absolute results are not as important as relative changes. Parabolic tetrahedrons (image in green below), with ten nodes for each element, are excellent general-purpose elements suitable for most applications.
Shell elements are utilized when the thickness is much less than the dimensions in the other directions. For example, if the length of the part is 100 times greater than the thickness, a shell element is recommended. Sheet metal parts and components with a consistent wall thickness are typically idealized as shell.
In Nastran In-CAD, a shell mesh can be created from surface geometry. If you already have volumetric CAD geometry, it is possible to use tools on the Prepare panel – such as Offset Surfaces, Find Thin Bodies, and Midsurfaces – to create suitable surface geometry for meshing as shell.
Line elements are generally utilized to represent linear geometry. Common line elements include bar (truss), beam, and pipe. These are often used on large structures where displacement is more important than local stresses.
One of the line element's advantages is that the line segment represents the axis of the geometry. No elements need to be constructed in the orthogonal directions, so this type of model will typically be able to be done with many fewer elements (and solve much faster) than an equivalent shell or solid version of the geometry.
In discussing elements in the prior sections, it was noted that some of the element types (solids and shells to be specific) have meshing options that are able to be changed by the user to be either linear or parabolic. This dictates the element order. Linear elements are considered lower-order and parabolic are higher-order.
Linear elements have nodes at the corners only, and they have straight edges. A linear tetrahedral element, for instance, has four triangular faces, six edges, and four nodes. A parabolic solid tetrahedral has the four corner nodes, but also an extra node at the midpoint of each of the six edges – for a total of ten nodes.
By increasing the element order, linear to parabolic, the solver increases the number of Gaussian points used in the process, making it more accurate for an equivalent number of elements. Secondly, the parabolic elements can, with the appropriate mesh options, have curved edges to better represent curved geometry. Lastly, note that parabolic elements are computationally more expensive due to the increase in node count over a linear one.
Not all components require an Idealization. In some cases, they can be simplified to a point mass using the Concentrated Mass tool. This option is also listed under the Idealization drop-down menu from the Prepare panel. This is a great way to represent the weight of non-structural parts like batteries, fuel tanks, motors, etc.
Concentrated Masses are typically applied to pre-defined work points or sketch points using the Manual mode. However, the Automatic mode allows the user to select a solid body. The Concentrated Mass is then automatically created based on the provided density. A concentrated mass will only create a force once Gravity has been applied to the Analysis.
It can only be connected to the mesh using Rigid Body Connectors. Contacts will not work since they are only applied to faces and edges.
