FEA Tips for the new Analyst

KISS: Keep it Simple Stupid! Always start simple and build in the complexity as needed. Have a clear understanding of what you are trying to model and what the results should reasonably be before building any FEA model. Begin an analysis with hand calculations and use engineering judgement to predict the load path. Next build simple models to validate your hypothesis. Last , build a complex model to fully understand all the system interactions. If you can not explain it, do not trust it !

Material and Element Properties: The most common error is not changing the default values for the Material . For linear static analysis, the stresses are independent of the Elastic Modulus; however the displacements are proportional to the modulus. So if you are getting unusual displacements, but correct stresses then it certainly means there is something off with your modulus of Elasticity. Also check beam cross sections, shell thicknesses and mass properties for concentrated mass elements, i.e lumped masses. Double check the total mass of the model is what you expect. Most pre-processors should be able to provide this information for selected elements. This is important when you are applying gravity g-loads and/or doing a frequency modal analysis.

Understand the different degrees of freedom of elements: Solid elements just have 3 degrees of freedom per node, i.e the three translations. Shell and Beam elements have 6 degrees of freedom per node, i.e 3 translations and 3 rotations. What this means is you can apply torque loads and rotational displacements to shell and beam elements. More importantly you need to be very careful when connecting shells and beams to solid elements. The shells and beams will be able to rotate along the nodes where they are connected to the solid elements. This can cause a pivot point, or rigid body mode in your model if there is nothing to stop the shell/beams from freely rotating along the connection point/edge with the solids.

Mesh Conservatively: Always use the fewest number of elements and nodes to accurately capture what you are looking for. Large models are difficult to debug and take unncessarily long to solve. The average model often needs to be solved five to ten times before all the errors are corrected. So don't naively think you will just need to solve the model once and have correct results on the first shot! Therefore, always strive for small model sizes so you can be efficient and explore many design iterations.

Perform Equilibrium Checks: Double check your applied loads with your reaction forces. Use simple beam bending stress equations, i.e Mc/I to verify bending moment stresses are in the ball park. Perform internal force calculations at various cross sections of your model. This is possible using our substructure analysis script, however, you will need to check with your specific post-processor if this can be done.

Study the Deformed Shape: The first thing you should check is the deformed shape! It is common for the analyst to spend hours trying to understand why some stress results look strange. However a quick look at the deformed shape would often immeadiately tell you what the problem is, i.e unconnected regions, incorrect material properties, incorrect loads and boundary conditions, incorrect contact pairs, rigid body motion etc.

Singularities: Make sure you have properly restrained all 6 rigid body modes. You can do this by having a minimum of three points on your model contrained with one xyz fixed node, one xy fixed node and one z fixed node. Also understand that stresses will approach infinity at sharp corners and boundary condition nodes. The finer the mesh at these locations, the higher the stress.

Understand software warnings: Make sure you understand ALL warning and errors issued by the FEA solver. Prove to yourself that ignoring a warning will not affect the accuracy of your results.

Unconnected Regions: Check for coincident nodes to make sure mating surfaces are connected as you intended. Also perform a free-edge element check to ensure elements are connected properly to each other. This is most useful when checking your 2D shell elements connectivity to each other. A highlighted free-edge will quickly indicate any edges that are not 'welded' or joined to any other element.

Shell Normals: Check that 2D shell normals are all in the same direction . This is important for your post-processing. If some elements are 'upside down' then the stress contours will not be continuos. When you display stresses, you will get incorrect results for the upside down elements since the contour plot will be showing the stresses for their opposite side. Remember shell stresses are plotted for either top or bottom surface, where the top surface is the side with the positive normal.