The *HEADING option is used to include a title and model description in the input file. The heading is useful for future reference purposes and may contain information on model revisions and the evolution of complex models. It can be several lines long, but only the first line will be printed as a title on the output pages. Below is the *HEADING definition that might be used for this analysis.

*HEADING
Blast load on a flat plate with stiffeners
S4R elements (20x20 mesh)
Normal stiffeners (20x2)
SI units (kg, m, s, N)

Use your preprocessor to generate the mesh shown in Figure 5–8 and the sets shown in Figure 5–9.

Give each element set the section properties shown below. Include the appropriate MATERIAL parameter on each *SHELL SECTION option so that each set of elements refers to a material definition.

*SHELL SECTION, MATERIAL=STEEL, ELSET=PLATE, OFFSET=SPOS
0.025,
*SHELL SECTION, MATERIAL=STEEL, ELSET=STIFF
0.0125,

The material named STEEL will be defined in the next section. Setting OFFSET to SPOS offsets the midsurface of the plate one half of the shell thickness away from the nodes. The effect is to make the PLATE nodes lie on the SPOS shell face instead of on the shell midsurface. The purpose of the shell offset in this case is to allow the stiffeners to butt up against the plate without overlapping any material with the plate. Figure 5–10 shows the cross-section of the joint between the stiffener and panel using the OFFSET parameter.

If the stiffener and base plate elements are joined at common nodes at their midsurfaces, an area of material overlaps, as shown in Figure 5–11.

Assume that both the plate and stiffeners are made of steel (Young's modulus of 210.0 GPa and 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 details of the post-yield behavior for this steel. We will add this information on the *PLASTIC option 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%. The plasticity data are shown below, and the plasticity stress-strain curve is shown in Figure 5–12.

*MATERIAL, NAME=STEEL
*ELASTIC
210.0E9, .3
*PLASTIC
300.0E6, 0.000
350.0E6, 0.025
375.0E6, 0.100
394.0E6, 0.200
400.0E6, 0.350
*DENSITY
7800.0,

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 data are regular—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 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, try setting the regularization tolerance, RTOL, to 0.001 and include one additional data pair, as shown below:

***ERROR: Failed to regularize material data. Try 
regularizing the independent variable intervals.

Fully constrain the edges of the plate using the node set EDGE defined previously.

*BOUNDARY
EDGE, ENCASTRE

*BOUNDARY
EDGE, 1, 6

Since the plate will be subjected to a load that varies with time, you must define an appropriate amplitude curve to describe the variation. Define the amplitude curve shown in Figure 5–13 as follows:

*AMPLITUDE, NAME=BLAST
0.0, 0.0, 1.0E-3, 7.0E5, 10E-3, 7.0E5, 20E-3, 0.0
50E-3, 0.0

Use the *DLOAD option to apply the blast load to the plate. It is important to ensure that the pressure load is being applied in the correct direction. Positive pressure is defined as acting in the direction of the positive shell normal. For shell elements the positive normal direction is obtained using the right-hand rule about the nodes of the element, as shown in Figure 5–14. Since the magnitude of the load has been defined in the BLAST amplitude definition, you need to apply only a unit pressure under *DLOAD. 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. Use the following option in your input file:

*DLOAD, AMPLITUDE=BLAST
PLATE, P, 1.0

To check on the progress of the solution, use the *MONITOR option to monitor the deflection at the center node of the plate during the analysis. Monitor the out-of-plane displacement at the center node by adding the following command to your input file:

*MONITOR, NODE=<center node number>, DOF=1

*OUTPUT, FIELD, NUMBER INTERVAL=25, VARIABLE=PRESELECT

A more detailed set of output can be saved for selected parts of the model by using the *OUTPUT, HISTORY option. Set the TIME INTERVAL parameter to 1.0E–4 seconds to write the required data at 500 points during the analysis. Write von Mises stress (MISES), equivalent plastic strain (PEEQ), and volumetric strain rate (ERV) for the elements in element set STIFFMAX. Since the nodes that will undergo the maximum displacements are at the center of the plate, use node set NOUT to output displacement and velocity history data for the center of the plate. In addition, save the following energy variables: kinetic energy (ALLKE), recoverable strain energy (ALLSE), work done (ALLWK), energy lost in plastic dissipation (ALLPD), total internal energy (ALLIE), energy lost in viscous dissipation (ALLVD), artificial energy (ALLAE), and the energy balance (ETOTAL).

*OUTPUT, HISTORY, TIME INTERVAL=1.0E-4
*ELEMENT OUTPUT, ELSET=STIFFMAX
PEEQ, MISES
*NODE OUTPUT, NSET=NOUT
U, V
*ENERGY OUTPUT
ALLKE, ALLSE, ALLWK, ALLPD, ALLIE, ALLVD, ALLAE, ETOTAL
*END STEP

abaqus job=blast_base

Information concerning model information, such as total mass and center of mass, and the initial stable time increment can be found at the top of the status file. The 10 most critical elements (i.e., those resulting in the smallest time increments) in rank order are also shown here. If your model contains a few elements that are much smaller than the rest of the elements in the model, the small elements will be the most critical elements and will control the stable time increment. The stable time increment information in the status file can indicate elements that are adversely affecting the stable time increment, allowing you to change the mesh to improve the situation, if necessary. It is ideal to have a mesh of roughly uniformly sized elements. In this example the mesh is uniform; thus, the 10 most critical elements share the same minimum time increment. The beginning of the status file is shown below.

 -------------------------------------------------------------------------------
  MODEL INFORMATION (IN GLOBAL X-Y COORDINATES)
 -------------------------------------------------------------------------------
  
    Total mass in model = 838.50
    Center of mass of model = ( 3.488360E-03, 9.999977E-01, 9.999990E-01)
  
     Moments of Inertia :
                  About Center of Mass              About Origin
       I(XX)          5.557794E+02                  2.232779E+03
       I(YY)          2.750539E+02                  1.113565E+03
       I(ZZ)          2.849024E+02                  1.123411E+03
       I(XY)          9.059906E-06                  2.925000E+00
       I(YZ)          4.272461E-04                  8.385000E+02
       I(ZX)          3.337860E-06                  2.924998E+00
  
 -------------------------------------------------------------------------------
  STABLE TIME INCREMENT INFORMATION
 -------------------------------------------------------------------------------
  
  
   The stable time increment estimate for each element is based on 
   linearization about the initial state.
  
  
    Initial time increment = 6.99621E-06
  
    Statistics for all elements:
       Mean = 1.01237E-05
       Standard deviation = 1.71465E-06
  
    Most critical elements :
     Element number   Rank    Time increment   Increment ratio
    ----------------------------------------------------------
         1033          1       6.996214E-06      1.000000E+00
         1038          2       6.996214E-06      1.000000E+00
         2033          3       6.996214E-06      1.000000E+00
         2038          4       6.996214E-06      1.000000E+00
         3033          5       6.996214E-06      1.000000E+00
         3038          6       6.996214E-06      1.000000E+00
         1013          7       6.996215E-06      9.999999E-01
         1018          8       6.996215E-06      9.999999E-01
         2013          9       6.996215E-06      9.999999E-01
         2018         10       6.996215E-06      9.999999E-01

 --------------------------------------------------------------------------------
  SOLUTION PROGRESS
 --------------------------------------------------------------------------------
  
  STEP 1  ORIGIN 0.00000E+00
  
   Total memory used for step 1 is approximately 755.2 kilowords
   Global time estimation algorithm will be used.
   Scaling factor :  1.0000
  
             STEP      TOTAL       CPU     STABLE      CRITICAL  KINETIC
  INCREMENT  TIME      TIME        TIME   INCREMENT    ELEMENT   ENERGY    MONITOR
         0  0.000E+00 0.000E+00   00:00:00 6.996E-06    1033   0.000E+00 0.000E+00
 Results number  0 at increment zero.
 ODB Field Frame Number    0 of   25 requested intervals at increment zero.
       235  2.000E-03 2.000E-03   00:00:12 8.573E-06    2026   4.468E+03 4.192E-03
 ODB Field Frame Number    1 of   25 requested intervals at  2.000078E-03
       469  4.006E-03 4.006E-03   00:00:25 8.572E-06    2018   1.119E+04 2.519E-02
 ODB Field Frame Number    2 of   25 requested intervals at  4.005884E-03
       702  6.003E-03 6.003E-03   00:00:38 8.572E-06    2031   6.167E+03 4.584E-02
 ODB Field Frame Number    3 of   25 requested intervals at  6.003135E-03
       935  8.000E-03 8.000E-03   00:00:50 8.556E-06    2031   1.766E+02 5.033E-02
 ODB Field Frame Number    4 of   25 requested intervals at  8.000187E-03
      1170  1.001E-02 1.001E-02   00:01:03 8.545E-06    2030   2.308E+03 4.535E-02
 ODB Field Frame Number    5 of   25 requested intervals at  1.000848E-02

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.

The default viewport annotations display the triad, title block, and state block in the viewport. You can suppress their display by changing the viewport annotations.

To fit the undeformed model shape in the viewport, select ViewAuto-fit.

Animating your results will provide a general understanding of the dynamic response of the plate under the blast loading. You will first plot the deformed model shape and then create a time-history animation of the deformed shape.

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 5–15.

The animation images can be saved to a file for playback at a later time.

Since it is not particularly easy to see the deformation of the plate from the deformed plot, it may be better to view the deflection response of the central node (node set NOUT) 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.

The other quantities saved as history output in the output database are the total energies of the model. The energy histories can help identify possible shortcomings in the model as well as highlight significant physical effects.

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, “Finite Elements and Rigid Bodies,” artificial strain energy is the energy used to control hourglass deformation, and the output variable ALLAE is the accumulated artificial strain energy. 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.

An input file for a model with a refined stiffener mesh is included in “Blast loading on a stiffened plate,” Section A.5 (blast_refined.inp); four elements through the depth are used to model the stiffener instead of two. 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 5–18 shows the histories of artificial energy for both the original mesh and the mesh with the refined stiffeners. As anticipated, the artificial energy is lower in the refined mesh. The important question, however, is whether or not the results changed significantly from the original to the refined mesh. Figure 5–19 shows that the displacement of the plate's central node is almost identical in both cases, indicating that the original mesh is capturing the overall response adequately. One advantage of the refined mesh, however, is that it better captures the variation of stress and plastic strain through the stiffeners.

Use the contour plotting capability of ABAQUS/Viewer 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 blast_refined.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, indicating that there is already some damping present in the analysis. By default, a bulk viscosity damping (discussed in Chapter 3, “Overview of 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. Modify the material data block to include damping, setting the mass proportional damping to 50.0.

*DAMPING, ALPHA=50.0, BETA=0.0

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. Therefore, increase the analysis period to 150 ms.

The results of the damped analysis clearly show the effect of mass proportional damping. Figure 5–22 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. The *RATE DEPENDENT option is used with the *PLASTIC option to introduce strain-rate dependence.

Add the following to the material option block:

*RATE DEPENDENT
40.0, 5.0

When the *RATE DEPENDENT option 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 5–23 and the history of plastic strain shown in Figure 5–24 confirm that the response is indeed stiffer when rate dependence is included.