Overview of element types
Choosing the element type
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.
Basic element (and node) information
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
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.
- The sum of the solid elements describes the shape of the resultant geometry.
- While the shape is described by the elements, the material property is still a required user input.
- Generally, there are several solid shapes that FEA packages could utilize. Autodesk Inventor Nastran uses all tetrahedron shaped elements to auto-mesh solid bodies.
- Linear tetrahedrons – four nodes (three DOF per node)
- Parabolic tetrahedrons – ten nodes (three DOF per node)
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
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.
- The shell element is a planar element representing the mid-surface of the geometry and so results in fewer elements than a solid element mesh as elements don’t need to be created for the volume.
- The material property is still a required user input, but also the thickness must be assigned.
- Shell elements can be created of either triangular or quadrilateral shapes.
- Linear triangular shell – three nodes
- Parabolic triangular shell (shown below) – six nodes
- Linear quadrilateral shell – four nodes
- Parabolic quadrilateral shell – eight nodes
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
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.
- The material property is still a required user input, but also the cross section needs to be defined – which can be on the simpler side (e.g., diameter and wall for a pipe) to more complex (e.g., an I-section beam).
- Only linear beam and bar element options are available within Inventor Nastran. Each segment of line contains two nodes (one at either end of the line segment). A span of beam (e.g., between two supports) can be divided into several segments.
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.
Understanding the element order
Linear and parabolic
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.
Concentrated Mass
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.