When Is It just a Pretty Picture? Tips For a Better Structural Analysis
Finite element simulation has come a long way since days of punch cards and line printers. Nowadays, most CAD systems have some type of integrated simulation package and traditionally stand alone simulation packages tied into multiple CAD systems. The easy access to CAD data, increased capabilities of the tools, and “wizards” that walk users through the process have all contributed to the increased growth of simulation.
In the early days of finite elements, analysts would review pages and pages of printed tabular results. Now, with a click of a button we can see a beautifully contoured color plots, the finite element results can be visualized in the larger assembly, and we are now getting to the point with virtual reality where we can walk through our results and interact with the assembly. These capabilities make it easy to create stunning and very convincing pictures, but they also make it very easy to believe inaccurate results.
Anyone who has done simulation for very long has had that “oops” moment. This is where you have presented your results, the product is being manufactured, or the part may have even failed in service and you go back to the analysis and realize you made a mistake. If you are lucky no one gets injured or dies, and if you are really lucky the product has margin and no changes need to be made.
If you are not lucky, the consequences can be much worse. One such example is the Sleipner A offshore oil platform. In 1991 this platform was undergoing a controlled ballasting test when a failure occurred and it sank to the ocean floor. The Sleipner A was designed using extensive finite element analysis and it was performed using a reputable commercial code (Nastran). The failure investigation determined that the stresses in the ballast chamber were underestimated by 47% causing the design of the walls of the ballasts to be too thin to support the pressures.
To minimize the errors in a simulation the analyst needs to have a very good understanding of the loads and how they affect the model, and also of the assumptions made in the CAD and simulation tools. Finally, the analyst needs to understand the limitations of the technology being used.
Sources of Errors
The primary sources of errors in simulation typically fall into one of the following categories:
 CAD geometry/simplifications.
 Lack of understanding of the math/physics behind FEA.
 Lack of understanding of the real loads, materials, etc.
 Lack of understanding of the capabilities of the simulation tool.
Ben Lewis of Custom Machines recently held a webinar covering the simplification of CAD for FEA purposes. Ben deals with a lot of large complex assemblies and this webinar is a good reference on how to properly prepare your CAD data.
In the SimScale forum, power user Jousef (@jousefm) has written several articles on the fundamentals of the math and physics behind the finite element method. Jousef’s articles are great if you are new to simulation or need a refresher on the math behind the magic.
The rest of this article will focus on the Simscale tool, how it differs from other simulation tools and some tips on how to get more accurate structural analysis results. The topic will mainly be linear static, but the content should apply to other types of structural analysis as well.
Meshing
Once you import your geometry into Simscale the next step is to apply a mesh to that geometry. Meshing the geometry is simply taking a very complex part or assembly and filling it with simple to solve volumes called elements.
Let’s take a step back for a minute. In general, when creating a mesh you have the ability to create 1D, 2D, or 3D elements. A 1D element is a line or curve element and examples of 1D elements are Springs and Beams. 2D elements are used to mesh surfaces and you typically provide the thickness. 3D elements are used to mesh solid volumes. The examples table show various types of elements and the location of the nodes on each element. The first order elements are linear elements. This means that linear interpolation is used to calculate values between the nodes. The second order elements use quadratic interpolation to calculate values between the nodes. In general, secondorder elements provide better results.
Currently, Simscale only supports the tetrahedral elements. While this does pose some limitations which we will discuss later, many of these can be worked around by using more elements at the cost of model size and solution time.
Now that we understand what elements SimScale uses we can look at the algorithms to actually mesh the model. SimScale provides four options for creating a structural mesh and you have to choose the option you want before setting up the mesh parameters. The four options are outlined below.
Tetrahedral Automatic. This is the most basic meshing algorithm. The user chooses a first or second order mesh and has five choices from “Very Course” to “Very Fine” for the mesh size. This method is very good for the initial analysis to check the geometry, and gives the user a good idea of what areas need more refinement. Tetrahedral Automatic generally does a good job refining the mesh in areas of high curvature.
Tetrahedral Parametric. Creates the same quality of mesh as Tetrahedral Automatic and has the same refinement in areas of high curvature. The main difference with Tetrahedral Parametric is that it allows the user to specify the global maximum and minimum element edge length. This gives you more control of the overall element size. For example, if you have a thin part and want to force multiple elements through the thickness you can do this by limiting the maximum element size to a fraction of the thickness. Or if you have a long part and you’re only interested in the stresses at the end you can increase the maximum element size.
Tetrahedral with Local Refinements. Is the same as Tetrahedral Parametric but it allows you to select edges, surfaces, or volumes to do a localized refinement. With this method, you specify a global minimum and maximum element size and then add a finer mesh to areas where you want more resolution.
Tetrahedral with Layer Refinements. This mesh is more like a tetrahedral CFD mesh. It starts with the Tetrahedral Automatic option but then it allows you to automatically add mesh refinement near the surfaces or faces of the mesh. The options are the total depth of the layers, the number of layers, and an expansion factor. While this does appear to produce good results it’s not an option I have used in my work.
SimScale Meshing Tips
Once you understand the four different meshing algorithms listed above, the meshing process is pretty straight forward in SimScale. The main areas to watch out for are more specific to the tetrahedral element and not SimScale. Here are a few areas to watch out for.
 One of the checks for the “goodness” of the tet element is called the aspect ratio. This is the ratio of the longest edge, over the shortest edge. In the areas where you want good results you want the ratio to be close to 1:1. In areas away from the areas of interest, the ratio can be up around 5:1 or slightly higher. The automatic mesher in SimScale does a good job at this and it performs an internal test for the aspect ratio. If you do not get the aspect ratio you like, the Tetrahedral with Local Refinements is a good way to change this around. In the postprocessing, you can also review the element aspect ratios.
 First order Tetrahedral elements tend to be overly stiff especially for bending problems. To account for this you need to use a finer mesh or use second order Tetrahedral elements.
 In general, secondorder Tet elements are recommended over first order Tet elements for linear static analysis. First order Tet elements work well for thermal analysis. For contact analysis, secondorder Tets can have difficulty converging.
 Typically long thin sections such as sheet metal are better meshed with shell elements. Since SimScale only has Tetrahedral elements your only option is to use solid elements. Thin sections under a bending load require about three to four linear elements through the thickness to resolve the stresses. Second order Tet elements can achieve this in one to two element through the thickness.
Solution Type and Solvers
Once you have a mesh created, the next step is to go to the simulation designer and set up the analysis. When you enter into the Solid Mechanics tab the first thing you notice is that you have two options for static analysis, two for dynamic analysis, and three for vibration analysis.
The reason you have a duplication of analysis types is because SimScale has integrated two solvers in their platform. One solver is CalculiX which is open source and developed by MTU Aero engines. The other solver is Code_Aster which is also open source and developed by EDF.
In the Tables below we will try to summarize why you would want to use each solver and why you would not want to.
Static Analysis
Static Analysis 
Static Analysis – Advanced 

Solver 
CalculiX 
Code_Aster 
Reason to use 


Reasons to avoid 


Dynamic Analysis
Dynamic Analysis 
Dynamic Analysis – Advanced 

Solver 
CalculiX 
Code_Aster 
Reason to use 


Reasons to avoid 


Vibration Analysis
Frequency Analysis 
Modal Analysis 
Harmonic Analysis 

Solver 
CalculiX 
CalculiX 
Code_Aster 
Reason to use 
Calculates: Eigenfrequencies Eigenmodes Effective Model Mass 
Calculates: Eigenfrequencies Eigenmodes Dynamic Response

Calculates: Structural response to periodic loads

Reason to avoid 



SimScale Structural Analysis Type Tip
 The Static – Advanced and Dynamic – Advanced analysis types do require slightly more input for setup but they are the recommended solvers due to their more robust loading and boundary conditions.
Loads and Boundary Conditions
Loads and boundary conditions are the tools you use to translate reality into a computersolvable model. How well you define them, how well you understand the results you want, and how well you understand the actual loads and boundary conditions, will in large determine the accuracy of your model.
For example, let’s say I have the structure in Figure 1. If I am interested in the maximum stress in the horizontal beam, I can use the model in Figure 2 and this will give good stress results. However, If I am also interested in the maximum deflection, this model will be wrong. While the chosen boundary condition does allow for the correct stress, it is too rigid and causes errors in the displacement. This is a very simple example of how results can be correct and/or incorrect based on assumptions and boundary conditions.
Now that we have an idea how boundary conditions and our assumptions can affect the results, let’s walk through analysis tree that Simscale set up when we chose our desired analysis type.
In the Domain section, there is an option for Contacts. In this area, you can define Bonded contacts, Sliding contacts, or Cyclic Symmetry contacts. In many CADbased simulation packages, you can simply select the surfaces you want contact between without really thinking about it. SimScale uses more traditional terminology of Master and Slave surfaces. The master surfaces should be the larger, flatter, and stiffer surfaces and they should have the coarser mesh. The Slave surfaces are obviously the opposite of the Master surfaces.
Bonded contacts are just as the name implies, all of the Slave surfaces are fixed to the master surfaces just like it was a single part. The sliding contact constrains the Slave surfaces (nodes) to slide along the Master surfaces. The cyclic symmetry contact allows you to only model a segment of a fullyrevolved part or assembly.
Simscale Tip: For Bonded contacts the surfaces do not need to be touching. There is a tolerance option in the settings. Contacts follow the linear assumption of small displacements.
If you have selected the Static – Advanced analysis type and set nonlinear to true, you will also see an option for Physical Contacts. Physical contacts allow you to model the actual load path through joints, parts coming into contact, or penetration. Physical contacts need to be a separate topic.
We will not discuss material properties, this area should be selfexplanatory.
In the Initial conditions section, SimScale allows you to define an initial displacement or an initial stress. These options can be used to put a prestress for example.
The loads and boundary condition area are pretty straightforward and comparable to other packages. If you are using the Static – Advanced analysis type the loads can be entered as a value, table, or formula.
While SimScale does not support Spring elements it does have an Elastic Support boundary condition which can simulate one node spring to the ground element.
Finally, SimScale offers a remote displacement and a remote force. These act as an RBE2 or RBE3 multipoint constraint. When these are set to undeformable, the remote point is rigidly attached to all nodes on the surfaces. When these are set to deformable the transmitted displacement/load becomes a weighted average.
SimScale Loads Boundary Conditions Tips
 SimScale does not attach loads and boundary conditions to the CAD geometry the way other simulation packages do. The loads and boundary conditions are applied to the mesh. So, when you remesh the model, you will need to attach your boundary conditions again.
 SimScale does not support local coordinate systems for applying loads or boundary conditions. All loads and boundary conditions are applied in the global cartesian coordinate system.
 If you want to apply a global gravitational acceleration, click on “Models”. I had to look for this several times.
Postprocessing
SimScale has an online postprocessor but they also recommend ParaView for postprocessing running on your local machine.
The online postprocessor is getting better all the time but it does have a few things to be aware of.
SimScale Postprocessing Tips
 If you are familiar with a lot of other simulation packages, once you complete your analysis you have a wide range of results you can view and calculate including reaction forces, maximums and minimums, and probing. With SimScale you need to set up and request all desired outputs prior to running the solution. If you run your solution and decide you want the reaction forces, you will need to rerun your analysis.
 SimScale does not support local coordinate systems in postprocessing. All results are viewed in the global cartesian coordinate system.
Conclusion
With any simulation package, just because your simulation converges or you can produce a museum quality contour plots, does not mean your results are good. You need to understand the simplifications to the CAD, theory behind the FEA, the loads, and the limitations of the tools.
Most importantly you need to question your results. Make sure you back them up with hand calculations and/or a convergence study.
Do you want to learn more about how to get accurate results from your finite element analysis? Register for my webinar for free and learn the essentials of static and dynamic structural analysis for a better understanding of the different solvers, loads, constraints, contacts, and tips for getting the right results.