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 judgment 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.
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 unnecessarily 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, to verify bending moment stresses.
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 immediately
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. 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.
