Understanding a Finite Element Analysis (FEA) Report
As an ASME pressure vessel fabricator, you may be required from time to time to perform a finite element analysis (FEA) of the vessel. This may be because of some unusual geometric feature of the vessel, or perhaps some complex or cyclic loading conditions. If you are relying on an outside consultant to perform the finite element analysis, you will likely get some kind of a report documenting what was done. So, what can you typically expect in an FEA report and what does it all mean?
The amount of detail contained in an FEA Stress Report can vary depending on the project, consultant, and contractual requirements. A comprehensive report allows the reader the ability to evaluate and critique the analysis and assess the accuracy of the results to some degree. While receiving a comprehensive report may be considered ideal, the level of effort and costs associated with producing such a report may be beyond the project’s budget. As such, the documentation of the FEA may vary from a handful of stress plots and summary tables to a detailed report discussing every aspect of the analysis, results, and evaluation.
The goal of this article is not to describe how to perform a finite element analysis, but rather assist a pressure vessel fabricator in understanding the significance of the types of information contained in a typical FEA report.
The usual procedure for performing a finite element analysis is
Define material properties
Create or import geometry
Create finite element mesh
Apply loads and boundary conditions
Define analysis type, options, and then solve
Review and evaluate the results
Other than the most basic of reports, a typical FEA stress report will discuss all of the above topics in some detail.
Material Properties
The material properties required to perform a stress analysis include density, modulus of elasticity, and Poisson’s Ratio. If thermal effects are to be evaluated the coefficient of thermal expansion will also be defined. Heat transfer properties such as thermal conductivity and specific heat will be required if a thermal analysis was performed to determine thermal gradients. If the pressure vessel is subjected to temperature changes or a thermal gradient, temperature dependent material properties should have been used in the analysis.
Geometry
The report should discuss which components of the pressure vessel have been included in the model, those that have not, and any simplifications that have been made. The appropriateness of these inclusions, exclusions, and simplifications should be considered in reviewing the report.
The Finite Element Model
A discussion of the finite element model will usually be presented. This may include a description of the types of elements used in creating the model and should include some plots of the finite element mesh. The details of the finite element mesh are important in accurately predicting stresses. A poor mesh can under-predict the magnitude of the stresses giving erroneous results. Three-dimensional finite element models will be meshed with either solid or shell elements. With solid elements, one or more of the following types will be used: hexagonal (brick), tetrahedral, pyramidal, or prism elements. While some analysts have a preference for or bias against certain element types, they are all capable of producing accurate results if the quality of the mesh is good. Element shape and size are the greatest factors in getting a good mesh and accurate results. The ideal element shape for solid elements is one where all of the faces are regular polygons of the same size. As the faces become more warped and interior angles become excessively large or small, the accuracy of the results will be affected. Tetrahedral and other non-hexagonal elements have a greater tolerance for less than ideal shapes than hexagonal elements. These elements are often used in areas of complex geometry where meshing with hexagonal elements can be difficult. However, meshing with non-hexagonal element types often require a significantly larger number of elements compared to hexagonal elements which results in longer computer run times. Another aspect of meshing that can affect the accuracy of the results is how fast the size of elements changes from one region of the finite element model to another. Stress gradients are more significant in areas of structural discontinuities requiring a more refined mesh to accurately predict the results in these areas. If the model transitions from a refined mesh to a coarser mesh too quickly in these areas, the magnitude of the stresses may be under-predicted. Another consideration when evaluating the finite element mesh of a model of a pressure vessel created using solid elements is the number of elements through the thickness of the shell and nozzles. Bending stresses occur at structural discontinuities. An inadequate number of elements through the thickness of the components at these locations will under-predict the bending stresses.
The report may also reference whether the elements are linear or quadratic. Linear elements have nodes located only at the corners of the element. Quadratic elements have an additional node mid-way between each of the corners. This is sometimes referred to as the elements having mid-side nodes. The additional nodes and the formulation behind these element types will give more accurate results than linear elements of the same type and size. The use of quadratic elements, however, will result in longer computational run times compared to linear elements when solving the analysis since the results at the additional nodes will have to be calculated.
An FEA report should include several plots showing the finite element mesh so one can assess the quality of the mesh. This can sometimes be overlooked in producing an FEA report, especially when FEA is an add-on to a CAD package that may not show the element mesh unless specifically requested.
Loads and Boundary Conditions
The FEA report should provide enough information to confirm the proper loading scenarios have been analyzed and evaluated. A report will also typically provide information on the boundary conditions of the finite element model. Boundary conditions are how the model is constrained against translation and rotation at its extents. The behavior of components that may or may not come into contact with each other, such as at flanged connections, may also be discussed if applicable. While the definition of boundary conditions for analyzing pressure vessels is often straight-forward, it is important to know that boundary conditions can have a significant impact on the results. An example of how boundary conditions can affect results is evident when comparing beam equations. The deflections, bending moment, and stresses in a beam under load are significantly different if the beam is simply-supported or has fixed ends. Therefore, the appropriateness of the boundary conditions that have been defined for the analysis should be considered carefully.
Analysis Type and Options
In general, there are not a lot of options specific to stress analyses that are pertinent to analyzing pressure vessels. Outside of options related to solution convergence controls, the most common option that is sometimes used is including non-linear geometric effects. This can be important when small displacement theory is not applicable due to large deformations of the vessel when subjected to loading. Most pressure vessel analyses, however, do not typically require including non-linear (large deflection) effects.
Results and Evaluation
The most important part of the FEA report is the documentation of the results and their evaluation. Typical results will be displacements and stresses. Assuming an elastic-stress analysis has been performed, the stresses will be compared to allowable stress limits. In reviewing the results the following questions should be asked:
Do the results make sense? The displacements and stresses should seem reasonable.
Do the stresses away from structural discontinuities due to internal pressure agree with hand calculations?
Do the reactions make sense based on the weight and loading?
Are the areas of highest stress evaluated?
Are there any areas that are discounted in the evaluation? why?
If you have any questions, ask. Do not assume that just because the results meet the acceptance criteria that they are correct.