# Mesh Density

Mesh Density

When performing an FEA analysis, the goal is generally to obtain results which are accurate while taking the least amount of time. The amount of time that a study takes to solve is directly related to the number of degrees of freedom in the study. With second order solid tetrahedral elements there are 10 nodes per element, each with three translational degrees of freedom. Each degree of freedom has an associated equation which must be solved for displacement. For second order triangular 2-D shell elements, there are 6 nodes, and each node has 6 degrees of freedom, three translational, and three rotational.

The first unknown in linear static FEA that is solved is the displacement of each node. Based on this, the stresses and strains are calculated. The stress values at nodes in an FEA study are calculated at Gauss, or Quadrature points in the element, and then averaged with the stress values from the surrounding elements (http://pathfinder.scar.utoronto.ca/~dyer/csca57/book_P/node44.html). While the displacements are solved explicitly at the nodes, the stresses are an averaged value and if there are insufficient stress values present in an area, the stress value averaged at the node can be inaccurate.

How many elements are necessary to obtain an “accurate” result? This depends on several things, such as what degree of accuracy you need as well as the geometry itself. (More on the geometry in my next post). However I will say that stresses near sharp corners or boundary conditions (fixtures, connectors, etc) can be inaccurate. The recommended starting point for “accurate” results according to SolidWorks is two second order tetrahedral elements across the thickness in all directions. However this is just a starting point, and you will have to decide for yourself whether the results obtained are sufficiently refined for your needs. This also means that in areas where you are not interested in the stress results that you do not necessarily need two elements across the thickness, reducing computation time.

Let’s examine the relation of number of elements across the thickness versus stress:

Figure 1: A thin plate with a hole in it. There is a “sensor” placed at the location where the highest stress in the plate will occur

Figure 2: Standard fixtures and a tensile load are applied to the plate. The global element size is set to a value which is larger than the thickness of the plate, resulting in just one element across the thickness and skewed elements (aspect ratio>1).

Figure 3: If you examine the cross section of the plate, you can see that there is only 1 “triangular edge” along the thickness.

Figure 4

Figure 5: The plate is re-meshed with a target element size of 1.50mm. Although the thickness is 2.5mm, because the elements are not forced to keep an aspect ratio of 1 (An aspect ratio of 1 results in a perfect equilateral triangular tetrahedron), there are two elements across the thickness.

Figure 6

Figure 7: checking the results at the sensor point, we find that the stress value has increased by almost 10%

Figure 8: The mesh is further refined to 0.75mm

Figure 9: Three elements across the thickness

Figure 10: Increase in stress value by halving the mesh size results in a 0.7% increase in reported stress values.

Thickness of Plate = 2.5mm | Element Size | Number of elements across thickness | Von Mises Stress (Mpa) | % Increase in Stress |

Case # | ||||

Case 1 | 4.372 mm | 1 | 395.8 | N/A |

Case 2 | 1.5mm | 2 | 432.5 | 9.27 |

Case 3 | 0.75mm | 3 | 435.6 | 0.72 |

As we can see, the difference between a single element across the thickness and two elements across the thickness is almost 10%. However further refining the mesh to include three elements across the thickness results in only a 0.72% increase in reported stress value.