The previous example illustrated some of the convergence difficulties that may be encountered when solving problems involving a nonlinear material response using implicit methods. We will now focus on solving a problem involving plasticity using explicit dynamics. As will become evident shortly, convergence difficulties are not an issue in this case since iteration is not required for explicit methods.
In this example you will assess the response of a stiffened square plate subjected to a blast loading in Abaqus/Explicit. The plate is firmly clamped on all four sides and has three equally spaced stiffeners welded to it. The plate is constructed of 25 mm thick steel and is 2 m square. The stiffeners are made from 12.5 mm thick plate and have a depth of 100 mm. Figure 10–18 shows the plate geometry and material properties in more detail. Since the plate thickness is significantly smaller than any other global dimensions, shell elements can be used to model the plate.
The purpose of this example is to determine the response of the plate and to see how it changes as the sophistication of the material model increases. Initially, we analyze the behavior with the standard elastic-plastic material model. Subsequently, we study the effects of including material damping and rate-dependent material properties.
This model uses the default rectangular coordinate system with the plate lying in the 1–3 plane. Since the plate thickness is significantly smaller than any other global dimensions, we can use shell elements of type S4R for the model.
The mesh in this model is based on the design shown in Figure 10–19, which is a relatively coarse mesh of 20 × 20 elements in the plate and 2 × 20 elements in each of the stiffeners. This mesh corresponds to the input file shown in “Blast loading on a stiffened plate,” Section A.9. It provides moderate accuracy while keeping the solution time to a minimum. Define the mesh so that the element normals for the plate all point in the positive 2-direction. Doing so ensures that the stiffeners lie on the SPOS face of the plate, which will be important when defining the element properties and shell offsets later.
The steps that follow assume that you have access to the full input file for this example. This input file, blast_base.inp, is provided in “Example: blast loading on a stiffened plate,” Section 10.5. Instructions on how to fetch and run the script are given in Appendix A, “Example Files.”
If you wish to create the entire model using Abaqus/CAE, please refer to “Example: blast loading on a stiffened plate,” Section 10.5 of Getting Started with Abaqus: Interactive Edition.
Figure 10–20 shows all the sets necessary to apply the element properties, loads, and boundary conditions.
This model includes all the nodes on the perimeter of the plate in a node set called EDGE. These nodes will have a completely fixed boundary condition. For output purposes, a node set called NOUT has been created containing the node at the center of the plate. Plate elements are included in an element set called PLATE, and the stiffener elements in an element set called STIFF. In addition, the four center elements on the central stiffener are included in an element set called STIFFMAX; this element set is for output purposes. These center elements will be subject to the maximum bending stress in the stiffeners.We now review the model data for this problem, including the model description, node and element definitions, element properties and shell offsets, material properties, boundary conditions, and amplitude definition for the blast load.
Model description
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 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)
Nodal coordinates and element connectivity
The mesh is shown in Figure 10–19 and the sets are shown in Figure 10–20.
Element properties and shell offset
Each element set in the model has the section properties shown below. To insure that each set of elements refers to a material definition, the appropriate MATERIAL parameter has been included on each *SHELL SECTION option:
*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 10–21 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 10–22.
If the thicknesses of the plate and stiffener is small in comparison to the overall dimensions of the structure, this overlapping material and the extra stiffness it would create has little effect on the analysis results. However, if the stiffener is short in comparison to its width or to the thickness of the base plate, the additional stiffness of the overlapping material could affect the response of the whole structure.Material properties
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 10–23.
*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. Please check your input data to see if they meet both criteria as explained in the "MATERIAL DATA DEFINITION" section of the Abaqus Analysis User's Guide. In general, regularization is more difficult if the smallest interval defined by the user is small compared to the range of the independent variable.Before continuing, set the regularization tolerance back to the default value (0.03) and remove the additional pair of data points.
Boundary conditions
The edges of the plate are fully constrained using the node set EDGE defined previously.
*BOUNDARY EDGE, ENCASTREAlternatively, you could specify the degrees of freedom by number.
*BOUNDARY EDGE, 1, 6
Amplitude definition for blast load
Since the plate will be subjected to a load that varies with time, you must define an appropriate amplitude curve to describe the variation. The amplitude curve shown in Figure 10–24 can be defined as follows:
*AMPLITUDE, NAME=BLAST 0.0, 0.0, 1.0E-3, 7.0E5, 10E-3, 7.0E5, 20E-3, 0.0 50E-3, 0.0The pressure increases rapidly from zero at the start of the analysis to its maximum of 7.0 × 105 Pa 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.
The history data begin with the *STEP option, which is followed immediately by a title for the step. After the title, this step is defined as a *DYNAMIC, EXPLICIT procedure with a time period of 50 ms.
*STEP Apply blast loading ** Explicit analysis with a time duration of 50 ms *DYNAMIC, EXPLICIT , 50E-03
Applying the blast load
The *DLOAD option is used 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 10–25. Since the magnitude of the load has been defined in the BLAST amplitude definition, we need to apply only a unit pressure under *DLOAD. This pressure is applied 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 full option is shown below:
*DLOAD, AMPLITUDE=BLAST PLATE, P, 1.0
Output requests
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. In this example we monitor the out-of-plane displacement at the center node by adding the following command to the input file:
*MONITOR, NODE=<center node number>, DOF=2For the input file shown in “Blast loading on a stiffened plate,” Section A.9, the node number at the center of the plate is 411.
Set the number of intervals during the step at which field data are written to the output database file (ODB) to 25. This ensures that the selected data outputs are written every 2 ms since the total time for the step is 50 ms. 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 visually. This model requests field output for the stresses, plastic strains, and nodal displacements.
*OUTPUT, FIELD, NUMBER INTERVAL=25 *ELEMENT OUTPUT S,PE *NODE OUTPUT U
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 STEPSave your input in a file called blast_base.inp since these results will serve as a base state from which to compare subsequent analyses. Run the analysis using the following command:
abaqus job=blast_base
We now examine the output information contained in the status (.sta) file.
Status file
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 = ( 1.000000E+00, 3.488372E-03, 1.000000E+00)
Moments of Inertia :
About Center of Mass About Origin
I(XX) 2.849002E+02 1.123410E+03
I(YY) 5.519482E+02 2.228948E+03
I(ZZ) 2.712609E+02 1.109771E+03
I(XY) -8.881784E-16 -2.925000E+00
I(YZ) -8.881784E-16 -2.925000E+00
I(ZX) -2.273737E-13 -8.385000E+02
-------------------------------------------------------------------------------
STABLE TIME INCREMENT INFORMATION
-------------------------------------------------------------------------------
The stable time increment estimate for each element is based on
linearization about the initial state.
Initial time increment = 8.18646E-06
Statistics for all elements:
Mean = 1.30938E-05
Standard deviation = 2.69043E-06
Most critical elements :
Element number Rank Time increment Increment ratio
----------------------------------------------------------
1022 1 8.186462E-06 1.000000E+00
1024 2 8.186462E-06 1.000000E+00
1027 3 8.186462E-06 1.000000E+00
1029 4 8.186462E-06 1.000000E+00
1033 5 8.186462E-06 1.000000E+00
1038 6 8.186462E-06 1.000000E+00
2022 7 8.186462E-06 1.000000E+00
2024 8 8.186462E-06 1.000000E+00
2027 9 8.186462E-06 1.000000E+00
2029 10 8.186462E-06 1.000000E+00
During the analysis the status file can be viewed to monitor the progress of the analysis. Shown below is the beginning of the solution progress portion of the status file. Many more increments have been carried out than you would expect from an Abaqus/Standard analysis and that the output database file is being written at intervals of 2 ms.-------------------------------------------------------------------------------
SOLUTION PROGRESS
-------------------------------------------------------------------------------
STEP 1 ORIGIN 0.0000
Total memory used for step 1 is approximately 1.7 megabytes.
Global time estimation algorithm will be used.
Scaling factor: 1.0000
Variable mass scaling factor at zero increment: 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 8.186E-06 1024 0.000E+00 0.000E+00
ODB Field Frame Number 0 of 25 requested intervals at increment zero.
ODB Field Frame Number 0 of 5 requested intervals at increment zero.
244 2.005E-03 2.005E-03 00:00:00 8.182E-06 2035 4.499E+03 4.224E-03
ODB Field Frame Number 1 of 25 requested intervals at 2.005236E-03
488 4.001E-03 4.001E-03 00:00:01 8.181E-06 2018 1.105E+04 2.506E-02
ODB Field Frame Number 2 of 25 requested intervals at 4.001393E-03
733 6.005E-03 6.005E-03 00:00:01 8.138E-06 2030 5.879E+03 4.555E-02
ODB Field Frame Number 3 of 25 requested intervals at 6.004539E-03
978 8.003E-03 8.003E-03 00:00:02 8.133E-06 2030 1.727E+02 4.976E-02
ODB Field Frame Number 4 of 25 requested intervals at 8.002752E-03
1224 1.000E-02 1.000E-02 00:00:02 8.139E-06 2030 2.299E+03 4.461E-02
ODB Field Frame Number 5 of 25 requested intervals at 1.000000E-02
Output for the node referenced on the *MONITOR option is also included in this file.Run Abaqus/Viewer by entering the following command at the operating system prompt:
abaqus viewer odb=blast_base
Changing the view
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 tools in the View Manipulation toolbar. Specify the view and 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.
Verifying shell section assignment
You can also visualize the section assignment and the shell thickness while postprocessing the results. For example, regions with common section assignments can be color coded to verify that the properties were assigned correctly (select Sections from the Color Code toolbar to color the mesh according to section assignment). To render the shell thickness, select View
ODB Display Options from the main menu bar. In the ODB Display Options dialog box, toggle on Render shell thickness and click Apply. If the model looks correct, as shown in Figure 10–26, toggle off this option and click OK before proceeding with the rest of the postprocessing instructions. Otherwise, correct the section assignment and rerun the job.
Animation of results
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. Then, create a time-history animation of the deformed shape. Use the Animation Options dialog box 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 10–27.
The animation images can be saved to a file for playback at a later time.To save the animation:
From the main menu bar, select AnimateSave As.
The Save Image Animation dialog box appears.
In the Settings field, enter the file name blast_base.
The format of the animation can be specified as AVI, QuickTime, VRML, or Compressed VRML.
Choose the QuickTime format, and click OK.
The animation is saved as blast_base.mov in your current directory. Once saved, your animation can be played external to Abaqus/Viewer using industry-standard animation software.
History output
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 10–28 (with displacements in millimeters).
To generate a history plot of the central node displacement:
In the Results Tree, double-click the history output data named Spatial displacement: U2 at the node in the center of the plate (set NOUT).
Save the current X–Y data: in the Results Tree, click mouse button 3 on the data name and select Save As from the menu that appears. Name the data DISP.
The units of the displacements in this plot are meters. Modify the data to create a plot of displacement (in millimeters) versus time by creating a new data object.
In the Results Tree, expand the XYData container.
The DISP data are listed underneath.
In the Results Tree, double-click XYData; then select Operate on XY data in the Create XY Data dialog box. Click Continue.
In the Operate on XY Data dialog box, multiply DISP by 1000 to create the plot with the displacement values in millimeters instead of meters. The expression at the top of the dialog box should appear as:
"DISP" * 1000
Click Plot Expression to see the modified X–Y data. Save the data as U2_BASE.
Close the Operate on XY Data dialog box.
Click the Axis Options 
tool in the toolbox. In the Axis Options dialog box, change the X-axis title to Time (s) and the Y-axis title to Displacement (mm). Click OK to close the dialog box. The resulting plot is shown in Figure 10–28.
The plot shows that the displacement reaches a maximum of 50.2 mm at 7.7 ms and then oscillates after the blast load is removed.
To generate history plots of the model energies:
Save the history results for the ALLAE, ALLIE, ALLKE, ALLPD, and ALLSE output variables as X–Y data. A default name is given to each curve; rename each according to its output variable name: ALLAE, ALLKE, etc.
In the Results Tree, expand the XYData container.
The ALLAE, ALLIE, ALLKE, ALLPD, and ALLSE X–Y data objects are listed underneath.
Select ALLAE, ALLIE, ALLKE, ALLPD, and ALLSE using [Ctrl]+Click; click mouse button 3, and select Plot from the menu that appears to plot the energy curves.
To more clearly distinguish between the different curves in the plot, open the Curve Options dialog box and change their line styles.
For the curve ALLSE, select a dashed line style.
For the curve ALLPD, select a dotted line style.
For the curve ALLAE, select a chain dashed line style.
For the curve ALLIE, select the second thinnest line type.
To change the position of the legend, open the Chart Legend Options dialog box and switch to the Area tabbed page.
In the Position region of this page, toggle on Inset and click Dismiss. Drag the legend in the viewport so that it fits within the grid, as shown in Figure 10–29.
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.
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 2% 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. Use caution when you refine 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.9 (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 10–30 shows the histories of artificial energy for both the original mesh and the mesh with the refined stiffeners. The artificial energy is slightly lower in the refined mesh. As a result, we would not expect the results to change significantly from the original to the refined mesh.
Figure 10–31 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.Contour plots
In this section you will 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.
To generate contour plots of the von Mises stress and equivalent plastic strain:
From the list of variable types on the left side of the Field Output toolbar, select Primary.
From the list of output variables in the center of the toolbar, select S. The stress invariants and components are available in the next list to the right. Select the Mises stress invariant.
From the main menu bar, select ResultSection Points.
In the Section Points dialog box that appears, select Top and bottom as the active locations and click OK.
Select PlotContoursOn Deformed Shape, or use the 
tool from the toolbox.
Abaqus plots the contours of the von Mises stress on both the top and bottom faces of each shell element. To see this more clearly, rotate the model in the viewport.
The view that you set earlier for the animation exercise should be changed so that the stress distribution is clearer.
Change the view back to the default isometric view using the 
tool in the Views toolbar.
Tip:
If the Views toolbar is not visible, select ViewToolbarsViews from the main menu bar.
Figure 10–32 shows a contour plot of the von Mises stress at the end of the analysis.
Similarly, contour the equivalent plastic strain. Select Primary from the list of variable types on the left side of the Field Output toolbar and select PEEQ from the list of output variables next to it.
Figure 10–33 shows a contour plot of the equivalent plastic strain at the end of the analysis.
The objective of this analysis is to study the deformation of the plate and the stress in various parts of the structure when it is subjected to a blast load. To judge the accuracy of the analysis, you will need to consider the assumptions and approximations made and identify some of the limitations of the model.
Damping
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 100 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. Modify the material data block to include damping, setting the mass proportional damping to 50.0.
*DAMPING, ALPHA=50.0, BETA=0.0BETA is the parameter that controls stiffness proportional damping, and at this stage we will leave it set to zero.
The duration of the oscillation of the plate is approximately 30 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 10–34 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.
Rate dependence
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 under the *PLASTIC option:
*RATE DEPENDENT 40.0, 5.0
With this definition of rate-dependent behavior, the ratio of the dynamic yield stress to the static yield stress (
) is given for an equivalent plastic strain rate (
), according to the equation 
, where 
and 
are material constants (40 and 5 in this case).
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 10–35 and the history of plastic strain shown in Figure 10–36 confirm that the response is indeed stiffer when rate dependence is included.
