Plate with Semicircle Nothes

Overview:

This report outlines the findings of a finite element model experiment using SolidWorks Simulation 2012. The experiment was conducted to verify the validity of Solid Works software solution. The 3D model used in this experiment was a plate with two semicircular notches. The plate was fixed at one end, and a tensile force of 100 KN was applied at the other end in the x-direction. To authenticate the simulation result, the maximum stress obtained from the software was compared to the analytical result calculated utilizing the stress concentration factor. Overall, the maximum stresses obtained from the simulations were between 312 MPa to 313 Mpa, which was very close to the analytical calculated stress of 310.44 MPa. The axial displacement was determined by the software to be 0.2195 mm which came remarkably close to the analytical solution of 0.2 mm. These results concluded that the FEM conducted by the SolidWorks Simulation software was reliable.

In addition to the validity of the FEM solution, the effects of mesh sizing and refinement were explored and analyzed. First, different global mesh sizes were used and the results were examined. These results demonstrated that the high load created a maximum stress within the notches. To further refine the mesh, a varying local mesh control size was used on the surface of the notches. The mesh experiment concluded that the mesh size and refinement played a pivotal role in the finite element analysis and computing time.

Finally, the mesh experiment was repeated using the curvature based mesh. This type of meshing automatically mapped the shape of the curved geometry. The results were similar to those obtained with the standard mesh. However, a slight increase in computing time was experienced due to the increased number of elements added near the notches.

Procedure

3D Model and Analytical Results

The model used in this experiment is a plate with two semicircular notches. The plate's dimensions are shown in the following Figure 1. The material in the simulations is set as AISI 1020 steel with a Young's modulus of 2 x 1011 Pa.

Figure 1. Plate Dimensions in mm and views.

When subject to an axial load, the notches create a stress concentration area within the plate. The approximate maximum stress is found by calculating the normal stress and multiplying it by the stress concentration factor. The calculated maximum axial stress is used as the reference value in this experiment.

The normal stress in the middle of the plate is:

σ_normal=F/A=(100000 N)/((0.1 m-0.04 m)∙0.01 m)=166.67 MPa

The stress concentration factor is found using the empirical formula:

K_e=3.065-3.370(2R/H)+0.647(2R/H)^2+0.658(2R/H)^3

K_e=3.065-3.370(0.4)+0.647(0.4)^2+0.658(0.4)^3=1.862632

The analytical maximum stress is:

σ_max=K_e σ_normal=1.862632 ∙166.67 MPa=▭(310.45 MPa)

The reference displacement can be found using the Young's modulus.

δ=FL/AE=(100000 N ∙0.4 m)/(1x〖10〗^(-3) m^2 ∙2x〖10〗^11 Pa)=0.0002 m=▭(0.2 mm)

Simulation set up

The 3D model of the plate was modeled in SolidWorks with the dimensions shown in Figure 1. The completed model is shown in Figure 2. In order to run the simulation, the following boundary conditions were applied. The left side of the model was fixed and the right side was applied with a tensile load of 100 KN. The boundary conditions are shown in figure 3. The next step of the simulation was to set up the mesh. This step proved to be the most important part of the simulation since the mesh type and size greatly affected the simulation outcome.

Figure 2: 3D model of plate with semicircular notches.

Figure 3: Boundary conditions

1st order mesh and 2nd order mesh

The first two types of mesh used were the 1st order and 2nd order mesh. The first order mesh, called draft quality in SolidWorks, supports linear interpolation. A coarse global mesh size of 14.58 mm was set. The overall mesh is seen in Figure 4. The mesh utilizes tetrahedral shape elements, each with 4 nodes. Each node is connected with a straight link. This type of node connection causes a problem when the mesh encounters curved geometry. As seen in Figure 5, the 1st order mesh replaced the curved edges of the notches with linear edges. The first order mesh inaccurately meshes the geometry and yields an erroneous maximum stress as seen in the results of section Table1.

Figure 4: 1st order mesh

Figure 5: 1st order mesh

When the geometry is meshed with a 2nd order mesh, known as high quality in SolidWorks; the mesh looks smoother. The 2nd order mesh is seen to further mesh the curved edge of the notches. By looking at Figure 6, we can see how the mesh is more curved at the edge of the notch as opposed to Figure 5, 1st order mesh.

Figure 6: 2nd order mesh

The second order mesh, as seen in section 3 Table 1, provided a closer maximum stress value of 280.80 MPa to the reference value of 310.45 MPa. This value while inaccurate tells us that further meshing of the geometry should include a 2nd order mesh with added refinements.

Global element refinement

To further refine the mesh, the elements of the mesh were raised by increasing the mesh density. In other words, the elements sizes were decreased to accommodate more elements. This technique is called global element refinement. In order to accurately see the effects of element refinement we made several new studies. Each new study was meshed with a finer quality than the previous study. The following Figures 7, 8, and 9 demonstrate the mesh density of three of the five studies.

Figure 7: Coarse mesh, global element size is 14.584 mm

Figure 8:Medium mesh, global element size is 7.8389 mm