Create a three-dimensional, deformable part with an extruded shell base feature to represent the plate. Use an approximate part size of 5.0, and name the part Plate. A suggested approach for creating the part geometry shown in Figure 10–28 is summarized in the following procedure:

Define the material and section properties for the plate and the stiffeners.

Create a material named Steel with a mass density of 7800 kg/m³, a Young's modulus of 210.0E9 Pa, and a Poisson's ratio of 0.3. At this stage we do not know whether there will be any plastic deformation, but we know the value of the yield stress and the details of the post-yield behavior for this steel. We will include this information in the material definition. The initial yield stress is 300 MPa, and the yield stress increases to 400 MPa at a plastic strain of 35%. To define the plastic material properties, enter the yield stress and plastic strain data shown in Figure 10–27. The plasticity stress-strain curve is shown in Figure 10–29.

During the analysis ABAQUS calculates values of yield stress from the current values of plastic strain. As discussed earlier, the process of lookup and interpolation is most efficient when the stress-strain data are at equally spaced values of plastic strain. To avoid having the user input regular data, ABAQUS/Explicit automatically regularizes the data. In this case the data are regularized by ABAQUS/Explicit by expanding the data to 15 equally spaced points with increments of 0.025.

To illustrate the error message that is produced when ABAQUS/Explicit cannot regularize the material data, you could set the regularization tolerance to 0.001 (in the Edit Material dialog box, select GeneralRegularization) and include one additional data pair, as shown in Table 10–2.

 ***ERROR: Failed to regularize material data. Please check
 your input data to see if they meet both criteria as 
 explained in the "MATERIAL DEFINITION" section of the
 ABAQUS Analysis User's Manual. In general, regularization is
 more difficult if the smallest interval defined by the user
 is small compared to the range of the independent variable.

Create two homogeneous shell section properties, each referring to the steel material definition but specifying different shell thicknesses. Name the first shell section property PlateSection, select Steel as the material, and specify 0.025 m as the value for the Shell thickness. Name the second shell section property StiffSection, select Steel as the material, and specify 0.0125 m as the value for the Shell thickness.

Assign the PlateSection definition to the regions of the plate and the StiffSection definition to the stiffeners (use [Shift]+Click to select multiple regions in the viewport).

In this model the stiffener and base plate are joined at their midsurfaces; thus, an area of material overlaps, as shown in Figure 10–30.

Create a dependent instance of the plate. Use the default rectangular coordinate system, with the plate lying in the 1–3 plane.

At this point, it is convenient to create the geometry sets that will be used to specify boundary conditions and output requests. Create one set named Edge for the plate edges and one set named Center at the center of the intersection of the plate and the middle stiffener, as shown in Figure 10–31. To create the set Center, you need to partition the edge of the original part in half using the Partition Edge: Enter Parameter tool.

Create a single dynamic, explicit step. Name the step Blast, and specify the following step description: Apply blast loading. Enter a value of 50E-3 s for the time period of the step.

In general, you should try to limit the number of frames written during the analysis to keep the size of the output database file reasonable. In this analysis saving information every 2 ms should provide sufficient detail to study the response of the structure. Edit the default output request F-Output-1, and set the number of intervals during the step at which preselected field data are saved to 25. This ensures that the selected data are written every 2 ms since the total time for the step is 50 ms.

A more detailed set of output for selected regions of the model can be saved as history output. Edit the default history output request H-Output-1 to write the whole model energies (selected by default) as well as displacement data for the center of the plate as history data to the output database file at 500 points during the analysis (i.e., every 1.0E–4 s of simulation time).

Create a history output request named Center-U2 for the step Blast. Select Center as the output domain, and select U2 as the translation output variable. Enter 500 as the number of intervals at which the output will be saved during the analysis.

Next, define the boundary conditions used in this analysis. Create a Symmetry/Antisymmetry/Encastre mechanical boundary condition in step Blast named Fix edges. Apply the boundary condition to the edges of the plate using the geometry set Edge, and specify ENCASTRE (U1 = U2 = U3 = UR1 = UR2 = UR3 = 0) to fully constrain the set.

The plate will be subjected to a load that varies with time: the pressure increases rapidly from zero at the start of the analysis to its maximum of 7.0 × 10⁵ N in 1 ms, at which point it remains constant for 9 ms before dropping back to zero in another 10 ms. It then remains at zero for the remainder of the analysis. See Figure 10–32 for details.

Define a tabular amplitude curve named Blast. Enter the amplitude data given in Table 10–3, and specify a smoothing parameter of 0.0.

Next, define the pressure loading. Since the magnitude of the load will be defined by the amplitude definition, you need to apply only a unit pressure to the plate. Apply the pressure so that it pushes against the top of the plate (where the stiffeners are on the bottom of the plate). Such a pressure load will place the outer fibers of the stiffeners in tension.

The plate load and boundary conditions are shown in Figure 10–33.

Seed the part with a global element size of 0.1. In addition, select SeedEdge By Number and specify that two elements be created along the height of the stiffeners. Mesh the plate and stiffeners using quadrilateral shell elements (S4R) from the Explicit element library. The resulting mesh is shown in Figure 10–34. This relatively coarse mesh provides moderate accuracy while keeping the solution time to a minimum.

Create a job named BlastLoad. Specify the following job description: Blast load on a flat plate with stiffeners: S4R elements (20x20 mesh) Normal stiffeners (20x2).

Save your model in a model database file, and submit the job for analysis. Monitor the solution progress; correct any modeling errors that are detected, and investigate the cause of any warning messages.

By default, ABAQUS plots the fast representation of the model. Plot the undeformed shape with the filled render style.

The default view is isometric, which does not provide a particularly clear view of the plate. To improve the viewpoint, rotate the view using the options in the View menu or the view tools in the toolbar. Select the viewpoint method for rotating the view. Enter the X-, Y-, and Z-coordinates of the viewpoint vector as 1,0.5,1 and the coordinates of the up vector as 0,1,0.

As noted in earlier examples, animating your results will provide a general understanding of the dynamic response of the plate under the blast loading. First, plot the deformed model shape and change the Deformed Shape Plot Options to display a Filled render style. Then, create a time-history animation of the deformed shape. Use the Animation Options button in the prompt area to change the mode to Play once.

You will see from the animation that as the blast loading is applied, the plate begins to deflect. Over the duration of the load the plate begins to vibrate and continues to vibrate after the blast load has dropped to zero. The maximum displacement occurs at approximately 8 ms, and a displaced plot of that state is shown in Figure 10–35.

Since it is not easy to see the deformation of the plate from the deformed plot, it is desirable to view the deflection response of the central node in the form of a graph. The displacement of the node in the center of the plate is of particular interest since the largest deflection occurs at this node.

Display the displacement history of the central node, as shown in Figure 10–36 (with displacements in millimeters).

We can see that once the load has been removed and the plate vibrates freely, the kinetic energy increases as the strain energy decreases. When the plate is at its maximum deflection and, therefore, has its maximum strain energy, it is almost entirely at rest, causing the kinetic energy to be at a minimum.

Note that the plastic strain energy rises to a plateau and then rises again. From the plot of kinetic energy we can see that the second rise in plastic strain energy occurs when the plate has rebounded from its maximum displacement and is moving back in the opposite direction. We are, therefore, seeing plastic deformation on the rebound after the blast pulse.

Even though there is no indication that hourglassing is a problem in this analysis, study the artificial strain energy to make sure. As discussed in Chapter 4, “Using Continuum Elements,” artificial strain energy or “hourglass stiffness” is the energy used to control hourglass deformation, and the output variable ALLAE is the accumulated artificial strain energy. This discussion on hourglass control applies equally to shell elements. Since energy is dissipated as plastic deformation as the plate deforms, the total internal energy is much greater than the elastic strain energy alone. Therefore, it is most meaningful in this analysis to compare the artificial strain energy to an energy quantity that includes the dissipated energy as well as the elastic strain energy. Such a variable is the total internal energy, ALLIE, which is a summation of all internal energy quantities. The artificial strain energy is approximately 1% of the total internal energy, indicating that hourglassing is not a problem.

One thing we can notice from the deformed shape is that the central stiffener is subject to almost pure in-plane bending. Using only two first-order, reduced-integration elements through the depth of the stiffener is not sufficient to model in-plane bending behavior. While the solution from this coarse mesh appears to be adequate since there is little hourglassing, for completeness we will study how the solution changes when we refine the mesh of the stiffener. Remember that caution must be taken when refining the mesh, since mesh refinement will increase the solution time by increasing the number of elements and decreasing the element size.

Edit the mesh, and respecify the mesh density. Specify four elements through the height of each stiffener, and remesh the part instance. Create a new job named BlastLoadRefined. Submit this job for analysis, and investigate the results when the job has completed running.

This increase in the number of elements increases the solution time by approximately 20%. In addition, the stable time increment decreases by approximately a factor of two as a result of the reduction of the smallest element dimension in the stiffeners. Since the total increase in solution time is a combination of the two effects, the solution time of the refined mesh increases by approximately a factor of 1.2 × 2, or 2.4, over that of the original mesh.

Figure 10–38 shows the histories of artificial energy for both the original mesh and the mesh with the refined stiffeners.

In this section you will use the contour plotting capability of the Visualization module to display the von Mises stress and equivalent plastic strain distributions in the plate. Use the model with the refined stiffener mesh to create the plots; from the main menu bar, select FileOpen and choose the file BlastLoadRefined.odb.

Undamped structures continue to vibrate with constant amplitude. Over the 50 ms of this simulation, the frequency of the oscillation can be seen to be approximately 214 Hz. A constant amplitude vibration is not the response that would be expected in practice since the vibrations in this type of structure would tend to die out over time and effectively disappear after 5–10 oscillations. The energy loss typically occurs by a variety of mechanisms including frictional effects at the supports and damping by the air.

Consequently, we need to consider the presence of damping in the analysis to model this energy loss. The energy dissipated by viscous effects, ALLVD, is nonzero in the analysis, indicating that there is already some damping present. By default, a bulk viscosity damping (discussed in Chapter 9, “Nonlinear Explicit Dynamics”) is always present and is introduced to improve the modeling of high-speed events.

In this shell model only linear damping is present. With the default value the oscillations would eventually die away, but it would take a long time because the bulk viscosity damping is very small. Material damping should be used to introduce a more realistic structural response. Thus, modify the material definition.

The time period for the oscillation of the plate is approximately 10 ms, so we need to increase the analysis period to allow enough time for the vibration to be damped out. Edit the step definition, and increase the time period of step Blast to 150E-3 s.

The results of the damped analysis clearly show the effect of mass proportional damping. Figure 10–42 shows the displacement history of the central node for both the damped and undamped analyses. (We have extended the analysis time to 150 ms for the undamped model to compare the data more effectively.) The peak response is also reduced due to damping. By the end of the damped analysis the oscillation has decayed to a nearly static condition.

Some materials, such as mild steel, show an increase in the yield stress with increasing strain rate. In this example the loading rate is high, so strain-rate dependence is likely to be important.

Add rate dependence to your material definition.

Change the time period of step Blast back to the original value of 50 ms. Create a job named BlastLoadRateDep, and submit the job for analysis. When the analysis is complete, open the output database file BlastLoadRateDep.odb, and postprocess the results.

When rate dependence is included, the yield stress effectively increases as the strain rate increases. Therefore, because the elastic modulus is higher than the plastic modulus, we expect a stiffer response in the analysis with rate dependence. Both the displacement history of the central portion of the plate shown in Figure 10–43 and the history of plastic strain energy shown in Figure 10–44 confirm that the response is indeed stiffer when rate dependence is included. The results are, of course, sensitive to the material data. In this case the values of and are typical of a mild steel, but more precise data would be required for detailed design analyses.