Tutorial 1: Model of a Single Slab

In this example, a model of a single slab founded on two base layers and subjected to a combination of axle and thermal loading will be created, solution generated, and the results of the simulation interpreted. The example covered here is identical to the solved project "single_slab" that is installed with EverFE2.23.

Model Creation and Geometry. Begin by starting EverFE, selecting New from the File menu, and creating a blank project with metric units. You will now be in the Geometry panel with the default single-slab model. The only change that you need to make is adding an elastic subgrade layer by checking 2 layers in the Base and Subgrade sub-panel; the thickness of the base layer should be 150 mm and the subgrade thickness should be 300 mm. At this point, save the model using the Save As option under the File menu under the name "Example_1". The EverFE window should now appear as shown below in Figure 1.

Figure 1: Geometry Panel During Model Creation

Material Properties. Now, click on the Material tab to display the Material panel. The default material properties for the slab (E = 28000 MPa) and base layer (E = 5000 MPa) will be maintained; however, change the subgrade elastic modulus from 200 to 300 MPa, which might be typical for a good gravel subgrade or sub-base. The other change that we will make is revising the Slab/Base Interface properties. Make sure that the Bonded Base checkbox is not selected, which implies that the slab and base are unbonded, and the Initial Stiffness and Slip Displacement parameters are both zero, which implies that there is no shear stress transferred between the slab and base. Change the Initial Stiffness to 1 MPa/mm and the Slip Displacement to 0.1 mm, which will result in shear stresses where there is contact and relative slip at the slab-base interface. The EverFE window will now appear as shown in Figure 2.

Figure 2: Material Panel During Model Creation

Axle and Thermal Loads. We are now ready to define loads. Click on the Loading tab to bring up the loading panel, which will show no loads on the model. Click on the Dual Wheel Tandem button to create the corresponding axle load. Only the right half of the axle will appear in the plan and elevation views, since the center of gravity of the axle is automatically located at the coordinate origin. Center the entire axle at the center of the 4600 mm long slab by changing the (x, y) coordinates of the axle from the default (0,0) to (2300,0). Alternatively, you can move the axle to the desired location using a mouse click-and-drag operation. All other axle parameters (Load, L, W, etc.) will remain unchanged from the default values.

Now, let's define a bilinear thermal gradient. Set the parameter "# of Temp. Changes" to 3, and define temperature changes 1, 2 and 3 as -5, -3, and 5, respectively. This defines a bilinear thermal gradient, where -5 is the temperature change at the top of the slab, -3 is the change at the mid-thickness of the slab, and 5 is the change at the bottom of the slab. The loading panel will now appear as shown below in Figure 3.

Figure 3: Loading Panel During Model Creation

Meshing. Since only a single slab is being modeled, the Dowel and Interlock tabs are inactive. Click on the Meshing tab to open the meshing panel. This will cause white lines to be overlaid on the plan and elevation views indicating the default finite-element mesh, which has 12x12 elements in plan, 2 elements through the slab thickness, and 1 element through both the base and subgrade layers. For now, no changes will be made to the default mesh parameters, although mesh refinement will be considered later in this example. The meshing input panel will appear as shown below in Figure 4.

Figure 4: Meshing Panel During Model Creation

Solve. Now, we are ready to generate a solution. Click on the Solve menu and select Run the Shown Analysis, which will execute the finite-element solver. There is no need to save the project before running, since it is automatically saved when the analysis is started. While the model is running, a small frame with a white background will appear that displays details of the progress of the finite-element solution. This particular project requires about 60 seconds to run on a Dell Optiplex with a 2.80 GHz Pentium IV.

View Displaced Shape. Note that the title of the EverFE window now displays Current Project: Example 1 (A Solution Exists). The Visualize menu is now active, and the model results can be displayed. Start by selecting Displacements from the Visualize menu. This will bring up a dialog box; simply click OK, and a few seconds later (after the solution has been loaded into memory) the EverFE displacement visualization sub-panel will appear. Click on the Show the Base checkbox at the top left of the panel, and then click the View Displacements button. This will bring up a window with a white background and a picture of the displaced shape of the slab and base layer as shown below in Figure 5. Note how the slab has separated from the base at the corners under the action of the bilinear negative thermal gradient. The view can be rotated and zoomed. Do not close the visualization window shown in Figure 5, as this will also end your EverFE session. However, you can minimize the window to reduce screen clutter.

Figure 5: Displaced Shape of Slab and Base

Stresses are generally the critical result of any analysis. To view stresses, select Stresses from the Visualize menu. This will bring up the stress visualization panel shown below in Figure 6.

Figure 6: Default Stress Visualization Window

View Stresses. The x-y plane at the top of the slab is the default plane for stress viewing, and the maximum principal stress is also selected by default. The scaling parameter is set to local, and the Color Map is selected. Clicking on the View Stresses button will bring up the visualization window shown below in Figure 7.  The view shown in Figure 7 is a plan view looking down the z-axis; however, the view can be scaled and rotated in three dimensions. The maximum stress is 0.341 MPa, which occurs the the top center of the slab.

Figure 7: Maximum Principal Stresses on Top of Slab

To view stresses on other planes within the slab, change the Horizontal plane to any value between 3 (the bottom) and 7 (the top), either by typing a number in the entry box or clicking the arrows. Since two elements were used through the slab thickness, there are 5 planes of nodes and thus five planes with saved stresses numbered 3 - 7. Changing the plane to 5, which is the mid-thickness of the slab, and clicking the View Stresses button brings up the following colormap of Figure 8; note that with this particular thermal gradient and axle loading, the maximum stress at the mid-thickness is actually larger than that on top of the slab (0.694 MPa). In addition to viewing stress colormaps, you can retrieve precise values for stresses and displacements at any point in the slab or base.

Figure 8: Maximum Principal Stresses at Mid-Thickness of Slab

Model Accuracy and Mesh Refinement. At this point, a critical question is the accuracy of the results. The best way to verify the model accuracy is through a mesh refinement, which is covered in two meshing examples. The current analysis poses some interesting issues, however, arising from the binlinear thermal gradient and to some extent the slab-base shear transfer due to the 1 MPa/mm shear stiffness at the slab-base interface. To investigate this issue in the present model, a series of meshes with increasing refinement have been constructed for the model as presented, and for the same model with a linear thermal gradient (-5^o C at the top of slab, 5^o C at the bottom of slab). The maximum principal stresses at the top and mid-thickness of the slab are presented below in Table 1. It is important to note that 30X30 elements in plan are required to demonstrate convergence with the binlinear thermal gradient, while 12x12 elements gives a reasonable result and 24x24 elements gives an excellent result with the linear thermal gradient.

Table 1: Slab Principal Stresses in MPa (Top/Mid-Thickness)

EverFE Home