Since the blank is initially a flat disk, model it with axisymmetric shell elements (SAX1) as a straight line starting at the symmetry axis. The only question, to which there is no definitive answer, is how many elements you should use. Examine the forming processes, and consider the deformations the blank will experience during the analysis. The mesh should be adequate to capture all of the features of the rigid forms accurately.

When using a uniform mesh—as we are in this example—the element size must be small enough to capture the smallest feature of the rigid forms, which is the 0.002 m radius of the punch in forming stage 2. The general rule that we will use is that there should be 10 elements to model that radius, making the maximum element size 0.00125 m. If we use 50 elements in the blank, which is a disk with a radius of 0.045 m, the element length is 0.0009 m, which is adequate. Both dies and punches are composed of straight segments connected by fairly gradual radii. Since there are no sharp bends, there is no need for a terribly fine mesh; no area of the blank is subjected to severe crimping. Assume that 50 elements in the blank is adequate.

Model the rigid dies and punches with analytical rigid surfaces in forming stage 1 and axisymmetric rigid elements (RAX2) in forming stage 2. An analytical rigid surface provides a smooth representation of the surface as opposed to the piecewise linear representation offered by rigid elements. In this example, it would be straightforward to model the rigid parts in the second forming stage with analytical rigid surfaces. However, most three-dimensional dies and punches require the generality of a rigid surface meshed with rigid elements. In forming stage 2, you must mesh the rigid surfaces finely enough so that they are accurate representations of the actual rigid tools. Mesh each straight segment with a single element, and mesh each radius with 30 rigid elements.

The rigid surfaces should be as close as possible to the blank without any overclosure at the start of the forming step. Remember that ABAQUS/Explicit includes the thickness of shell elements when determining contact; therefore, the midplane of the blank must be at least one-half of the shell thickness away from the rigid tools above and below it. Prior to the first step ABAQUS/Explicit will attempt to resolve overclosures in a strain-free manner, and the resulting nodal location changes may distort the elements. In this example initial overclosures could change the initial shape of the blank if the overclosures are great enough.

Give each element set appropriate section properties. Create shell section properties for the blank so that it refers to a material called STEEL (to be defined later), uses five-point Gauss integration, and has a thickness of 0.5 mm.

*SHELL SECTION, ELSET=BLANK, MATERIAL=STEEL,
SECTION INTEGRATION=GAUSS
.0005, 5

The blank is modeled using only the elastic material model since a *FREQUENCY analysis is a linear perturbation step and, thus, ignores nonlinear material properties. Use the following data to define the elastic and mass properties of the steel:

*MATERIAL, NAME=STEEL
*ELASTIC
210.0E9, 0.3
*DENSITY
7800.,

Apply symmetry boundary conditions to node set BSYM, and fix node set BEND in the axial, or 2-, direction.

*BOUNDARY
BSYM, 1
BSYM, 6
BEND, 2

The history definition defines the *FREQUENCY procedure type to extract the first eigenmode. Request *RESTART output and the nodal displacements of the blank as field output to the output database file, and suppress other output.

*STEP
*FREQUENCY
1,
*RESTART, WRITE
*OUTPUT, FIELD
*NODE OUTPUT, NSET=BLANK
U,
*EL PRINT, FREQUENCY=0
*NODE PRINT, FREQUENCY=0
*END STEP

Save your frequency analysis input in a file named draw_freq_std.inp, and run the analysis using the following command:

abaqus job=draw_freq_std

When the analysis has completed, use ABAQUS/Viewer to plot the shape of mode 1. Start ABAQUS/Viewer by typing

abaqus viewer odb=draw_freq_std

The frequency analysis shows that the blank has a fundamental frequency of 304 Hz, corresponding to a period of 0.0033 s. Figure 7–12 shows the displaced shape of the first mode. We now know that the lower bound on the step time for the first forming stage is 0.0033 s.

The following would be a suitable description for the simulation:

*HEADING
Deep drawing of a can bottom -- stage 1, attempt 1
SI units (kg, m, s, N)

Give each element set appropriate section properties. Create shell section properties for the blank so that it refers to a material called STEEL (to be defined later), uses five-point Gauss integration, and has a thickness of 0.5 mm. Five section points through the shell thickness should provide accurate results for a body that will incur significant plasticity.

*SHELL SECTION, ELSET=BLANK, MATERIAL=STEEL,
SECTION INTEGRATION=GAUSS
.0005, 5

The blank, which is the only deformable body in this simulation, is modeled using an elastic-plastic material model. Use the following data to define the elastic and mass properties of the steel:

*MATERIAL, NAME=STEEL
*ELASTIC
210.0E9, 0.3
*DENSITY
7800.,

*PLASTIC
0.912E8, 0.0
0.131E9, 0.159E-02
0.171E9, 0.649E-02
0.211E9, 0.177E-01
0.251E9, 0.395E-01
0.291E9, 0.776E-01
0.331E9, 0.139
0.391E9, 0.295

Figure 7–13 shows that the plasticity curve for this example is quite smooth.

Use the *SURFACE option to define the analytical surfaces of the rigid tools.

*SURFACE, TYPE=SEGMENTS, NAME=PUNCH1
START,0.032,0.03025
LINE,0.032,0.00625
CIRCL,0.026,0.00025,0.026,0.00625
LINE,0.,0.00025
*SURFACE, TYPE=SEGMENTS, NAME=DIE1
START,0.0326,-0.02825
LINE,0.0326,-0.00425
CIRCL,0.0366,-0.00025,0.0366,-0.00425
LINE,0.050,-0.00025

To bind an analytical surface to a rigid body, assign the name of the analytical surface to the ANALYTICAL SURFACE parameter on the *RIGID BODY option. Use the REF NODE parameter to specify the rigid body reference node that will control the motion of the rigid body.

*RIGID BODY, ANALYTICAL SURFCE=PUNCH1,
REF NODE=<reference node number>
*RIGID BODY, ANALYTICAL SURFACE=DIE1,
REF NODE=<reference node number>

Define the surfaces on the top and bottom of the blank. The surfaces on the top and bottom of the blank must face PUNCH1 and DIE1, respectively.

*SURFACE, NAME=BLANK_TOP
BLANK, <SPOS or SNEG>
*SURFACE, NAME=BLANK_BOT
BLANK, <SPOS or SNEG>

The initial fixed boundary conditions can be part of the model definition or history definition. Since the model is axisymmetric, you must constrain each of the bodies—the blank, punch 1, and die 1—from motion in the radial, or 1-, direction and from in-plane rotation (degree of freedom 6). In addition, constrain die 1 from motion in the axial, or 2-, direction.

*BOUNDARY
REFP1, 1
REFP1, 6
REFD1, 1, 6
BSYM, 1 
BSYM, 6

In “Determining an appropriate step time,” Section 7.5.4, we performed a frequency analysis, which showed that the blank has a fundamental frequency of 304 Hz, corresponding to a time period of 0.0033 s. This time period provides a lower bound on the step time for the first forming stage. Choosing the step time to be 10 times the time period of the fundamental natural frequency, or 0.033 s, should ensure a quality quasi-static solution. This time period corresponds to a constant punch velocity of 0.45 m/s, which is typical for metal forming.

Even if the punch actually moves at a nearly constant velocity, it is desirable to use a different amplitude curve that allows the blank to accelerate more smoothly. When considering what type of loading amplitude to use, remember that smoothness is important in all aspects of a quasi-static analysis. The preferred approach is to move the punch as smoothly as possible the desired distance in the desired amount of time. We will analyze the first forming stage using both approaches—a constant punch velocity of 0.45 m/s and a smoothly ramped punch velocity using a SMOOTH STEP amplitude—and will compare the results.

Before you run the forming analysis, you may wish to know how many increments the analysis will take and, consequently, how much computer time the analysis requires. You can run a datacheck analysis to obtain the approximate value for the initial stable time increment, or you can estimate it using the relations in “Mass scaling,” Section 7.3. Knowing the stable time increment, which in this case does not change much from increment to increment, you can determine how many increments are required to complete the forming stage. Once the analysis begins, you can get an idea of how much CPU time is required per increment and, consequently, how much CPU time the step requires.

Using the relations stated in “Mass scaling,” Section 7.3, the stable time increment for this analysis is approximately 1 × 10^–7 s. Therefore, the forming stage requires approximately 330,000 increments for a step time of 0.033 s.

To help determine how closely the analysis approximates the quasi-static assumption, the various energy histories are useful. Especially useful is comparing the kinetic energy to the internal strain energy. Another useful history plot is that of the velocities at typical nodes. Earlier you created the node set, NHIST, containing nodes at which you will obtain velocity histories. Such output gives you an idea of the severity of any velocity spikes in the solution. Write these energy and velocity histories as history data to the output database file. Write the section forces, shell thicknesses, and nodal displacements to the output database as field data for postprocessing with ABAQUS/Viewer. You should also have ABAQUS save the state information so that you can restart the analysis. For your first attempt request state information at 20 intervals. Once you are more confident with the first forming stage, you can decrease this value. Define the reference node for the rigid surface PUNCH1 as the monitor node.

Before looking at the results that are ultimately of interest, such as stresses and deformed shapes, we need to determine whether or not the solution is close enough to being quasi-static to be acceptable. One good approach is to compare the kinetic energy history to the internal energy history. In a metal forming analysis most of the internal energy is due to plastic deformation. Since punch 1 has no mass, the blank is the only body with mass; and the kinetic energy is solely due to the motion of the blank. To indicate an acceptable quasi-static solution, the kinetic energy of the blank should be no greater than a few percent of the internal energy. For greater accuracy, especially when springback stresses are of interest, the kinetic energy should be lower. This approach is very useful because it is general for all types of metal forming processes and does not require any intuitive understanding of the stresses in the model; many forming processes may be too complex to permit an intuitive feel for the results.

While a good primary indication of the caliber of a quasi-static analysis, the ratio of kinetic energy to internal energy alone is not adequate to confirm the quality. You should also evaluate the two energies independently to determine whether they are reasonable. This part of the evaluation takes on increased importance when accurate springback stress results are needed because an accurate springback stress solution is highly dependent on accurate plasticity results. Even if the kinetic energy is fairly small, if it is highly oscillatory, the model could be experiencing significant plasticity. Generally, we expect smooth loading to produce smooth results; if the loading is smooth but the energy results are oscillatory, the results may be inadequate. Since an energy ratio is incapable of showing such behavior, you should also study the kinetic energy history itself to see whether it is smooth or noisy.

If the kinetic energy does not indicate quasi-static behavior, it can be useful to look at velocity histories at some nodes to get an understanding of the model's behavior in various regions. Such velocity histories can indicate which regions of the model are oscillating and causing the high kinetic energies.

In ABAQUS/Viewer, select FileOpen from the main menu bar; or use the tool from the toolbar to open the output database draw_stage1_attempt1.odb. Plot the kinetic energy and the internal energy.

Similarly, create a history plot of the model internal energy, ALLIE (see Figure 7–15).

Figure 7–14 shows the kinetic energy history, which is very noisy through the first half of the step before becoming smooth. That the kinetic energy history has no clear relation to the forming of the blank is an indication of the inadequacy of this analysis. In this analysis the punch velocity remains constant, while the kinetic energy—which is due to the blank entirely since the punch has no mass—is far from constant.

Figure 7–15 shows the internal energy history. Without anything further to which to compare the internal energy, it appears reasonable, although it is not clear why the slope changes at 8 ms.

Comparing Figure 7–14 and Figure 7–15 shows that the kinetic energy is a small fraction (less than 1%) of the internal energy through all but the very beginning of the analysis. The criterion that kinetic energy must be small relative to internal energy has been satisfied, even for this severe loading case.

Since the kinetic energy history is very noisy, it is useful to look at the velocity history of a node in the model to gain an understanding of the blank's motion. Plot the vertical velocity (V2) history of the first node in node set NHIST, which is a node in the central region of the blank (Figure 7–16).

The velocity of the node oscillates between values as great as ±10 m/s, while the punch velocity remains constant. Such noisy behavior has a strong effect on the results in this case, since the material includes plasticity. These results indicate that we must change the simulation in some way to obtain a smoother response.

The kinetic energy history shown in Figure 7–17 is still quite noisy, although somewhat different from that of attempt 1. The noise dies out by 20 ms, and the kinetic energy drops to zero. Near the end of the analysis it again becomes noisy.

The internal energy for attempt 2, shown in Figure 7–18, is similar to that of attempt 1. The internal energy history has a few unexplained bumps, rather than the expected smooth increase. Again, the ratio of kinetic energy to internal energy is quite small and appears to be acceptable.

For many forming analyses a smooth loading velocity, such as that used in attempt 2, is adequate to produce a quasi-static forming step. However, this particular forming process is somewhat less well-behaved than many because of the lack of a blank holder. Figure 7–19 shows the velocity history of the second node in node set NHIST, which contains the node at the free end of the blank.

The kinetic energy history shown in Figure 7–20 is much smoother and corresponds to the punch velocity much better than the previous attempts, though there is still some high frequency oscillation.

The internal energy history, shown in Figure 7–21, shows a smooth increase from zero up to the final value. Most of the internal energy is dissipated by plasticity. Again, the kinetic energy is small relative to the internal energy. These results appear to be acceptable.

Now that we are satisfied that the quasi-static solution for the first forming stage is adequate, study some of the other results of interest. Figure 7–23 shows a contour plot of SF1, which is the force summation through the entire thickness of the element in the radial direction, or the local 1-direction. The axisymmetric model has been swept 90° for visualization purposes.

The plot shows that SF1 is nearly constant at a value of approximately 3.274 × 10⁴ in the flat region near the symmetry line. We would expect SF1 to be fairly high and positive in this region because of the uniform stretching. Since the blank is formed in a smooth manner, we would expect SF1 to vary smoothly, as it does. It also is reasonable that SF1 drops to a lower value toward the free end of the blank.

Figure 7–24 shows a contour plot of the shell thickness, STH. At the start of the analysis the blank had a uniform shell thickness of 0.5 mm.

“Loading rates,” Section 7.2, and “Metal forming problems,” Section 7.2.3, discuss how to determine acceptable scaling of the loading rate or mass to accelerate the time scale of a quasi-static analysis. The goal is to model the process in the shortest time period in which inertial forces remain insignificant. There are bounds on how much the solution time can be increased while still obtaining a meaningful quasi-static solution.

As discussed in “Loading rates,” Section 7.2, we can use the same methods to determine an appropriate mass scaling factor as we would use to determine an appropriate load-rate scaling factor. The difference between the two methods is that a load-rate scaling factor of f has the same effect as a mass scaling factor of . Originally, we assumed that a step time of 10 times the period of the fundamental frequency of the blank would be adequate to produce quasi-static results. By studying the model energies and other results, we were satisfied that these results were acceptable. This technique produced a punch velocity of approximately 0.5 m/s, which is typical of actual punch velocities. Now we will accelerate the solution time using mass scaling and compare the results against our unscaled solution to determine whether the scaled results are acceptable. We assume that scaling can only diminish, not improve, the quality of the results. The objective is to use scaling to decrease the computer time and still produce acceptable results.

Our goal is to determine what scaling values still produce acceptable results and at what point the scaled results become unacceptable. To see the effects of both acceptable and unacceptable scaling factors, we investigate a range of scaling factors on the stable time increment size from to 30; specifically, we choose , 10, and 30. These speedup factors translate into mass scaling factors of 10, 100, and 900, respectively.

To apply mass scaling of 10, add the following option to the history definition,

*FIXED MASS SCALING, FACTOR=10

First we will look at the effect of mass scaling on the section forces and the displaced shape. We will then see whether the energy histories provide a general indication of the analysis quality.

One of the results of interest in this analysis is the radial section force, SF1. Since we have already seen the contour plot of SF1 at the completion of the unscaled analysis in Figure 7–23, we can compare the results from each of the scaled analyses with the unscaled analysis results. These contour plots display the results in the form of bands on the displaced mesh. Therefore, these SF1 contour plots also provide the displaced shape of the mesh. Figure 7–26 shows SF1 for a speedup of (mass scaling of 10), Figure 7–27 shows SF1 for a speedup of 10 (mass scaling of 100), and Figure 7–28 shows SF1 for a speedup of 30 (mass scaling of 900). These plots indicate that a speedup of produces results that are very similar to the unscaled results. For a speedup of 10 the results are similar, but the section force at the symmetry axis drops noticeably. For a speedup of 30 the section force results are quite different, indicating that this level of speedup is clearly too high.

Now that we have seen how mass scaling has affected some of the section force results, we will see whether the energy histories provide the same indication of analysis quality. Figure 7–29 shows the histories of kinetic energy and internal energy for all of the scaled analyses. The internal energy is almost identical for all three cases, whereas the kinetic energy increases from nearly zero for a speedup of to a maximum of approximately 7.0 for a speedup of 30.

As the mass scaling increases, the solution time decreases. The quality of the results also decreases because dynamic effects become more prominent, but there is usually some level of scaling that improves the solution time without sacrificing the results. Clearly, a speedup of 30 is too great to produce quasi-static results for this analysis.

A smaller speedup, such as , does not alter the results significantly. These results would be adequate for most applications, including springback analyses. With a scaling factor of 10 the quality of the results begins to diminish, while the general magnitudes and trends of the results remain intact. Correspondingly, the ratio of kinetic energy to internal energy increases noticeably. The results for this case would be adequate for many applications but not for accurate springback analysis.

The first option following *HEADING is the *IMPORT option, which reads the element definitions and the state from the corresponding ABAQUS/Explicit analysis. Your import input file should begin with the following:

*HEADING
Deep drawing of a can bottom -- first springback
ABAQUS/Standard springback following
draw_stage1_attempt3_sqrt10.inp
SI units (kg, m, s, N)
*IMPORT, STEP=1, INTERVAL=10, STATE=YES, UPDATE=NO
BLANK,
*IMPORT ELSET
BLANK,
*IMPORT NSET
BSYM, NHIST

Setting the STATE parameter equal to YES causes the state of the model—stresses, strains, etc.—to be imported. Setting the UPDATE parameter equal to NO causes the strains and displacements to be imported as well instead of being reset to zero. The data line following the *IMPORT option supplies the name of the element set containing the elements that are to be imported. The data line following the *IMPORT ELSET option lists element set names to be imported; the *IMPORT NSET option likewise identifies node set names to be imported.

You must redefine the boundary conditions, which are not imported. Impose the same symmetry boundary conditions as were imposed in the ABAQUS/Explicit input file.

*BOUNDARY
BSYM, 1
BSYM, 6

For output, write the final state of the model to the restart file.

*RESTART, WRITE, FREQUENCY=999

The history definition is quite straightforward since no loads are applied. Use the following history definition:

*STEP, NLGEOM
*STATIC
.1, 1.
*BOUNDARY, FIXED
BSYM, 2, 2
*OUTPUT, FIELD, FREQUENCY=10
*ELEMENT OUTPUT, ELSET=BLANK
STH, SF
*NODE OUTPUT
U,
*END STEP

The NLGEOM parameter is used on the *STEP option since the ABAQUS/Explicit analysis used it (this is the default setting in ABAQUS/Explicit). In general, it is safer to include the NLGEOM parameter because we do not always know whether or not geometric nonlinearities will affect the results. To remove rigid body motion, it is necessary to fix the blank in the 2-direction. Fix the blank at just a single point, such as node set BSYM, so that you impose no unnecessary constraints. It is important to use the FIXED parameter on the *BOUNDARY option so that BSYM is fixed at its final position at the end of forming stage 1. If you were to omit the FIXED parameter, BSYM would return to its original location prior to deformation. Either fixing BSYM at its final position from the previous stage or moving it back to its undeformed location will produce the same springback results; however, fixing BSYM at its final position retains the necessary continuity in the blank location through the stages of this simulation.

Save your input in a file named draw_spring1_std.inp, and run the analysis using the following command:

abaqus job=draw_spring1_std oldjob=draw_stage1_attempt3_sqrt10

Figure 7–30 shows a contour plot of SF1 at the end of the springback analysis in ABAQUS/Standard. These results are necessarily dependent on the accuracy of the forming stage preceding it. In fact, springback results are highly sensitive to errors in the forming stage, more sensitive than the results of the forming stage itself.

Import the model from the final increment of the springback analysis. Set the STATE parameter equal to YES so that the stress and strain state of the model is imported. Set the UPDATE parameter equal to NO so that the displacements are continuous. Begin your restart input file with the following *HEADING and *IMPORT option blocks:

*HEADING
Deep drawing of a can bottom -- stage 2
ABAQUS/Explicit annealing and forming stage 2 following
draw_spring1_std.inp
SI units (kg, m, s, N)
*IMPORT, STATE=YES, UPDATE=NO
BLANK,

Since you are importing only the blank from the ABAQUS/Standard analysis, you must define the rigid tooling needed for forming stage 2 and the necessary node and element sets as shown in Figure 7–11.

*RIGID BODY, ELSET=PUNCH2, REF NODE=<reference node number>
*RIGID BODY, ELSET=DIE2, REF NODE=<reference node number>
*RIGID BODY, ELSET=DOMER, REF NODE=<reference node number>

Define the surfaces on the blank and the rigid tools.

*SURFACE, NAME=BLANK_TOP
BLANK, <SPOS or SNEG>
*SURFACE, NAME=BLANK_BOT
BLANK, <SPOS or SNEG>
*SURFACE, NAME=PUNCH2
PUNCH2, <SPOS or SNEG>
*SURFACE, NAME=DIE2
DIE2, <SPOS or SNEG>
*SURFACE, NAME=DOMER
DOMER, <SPOS or SNEG>

You must also define the spring and dashpot on which die 2 sits. These are defined as a SPRINGA and a DASHPOTA element, each with one end attached to the reference node for die 2 (node set REFD2) and one end attached to ground (node set SPEND).

*ELEMENT, TYPE=SPRINGA, ELSET=SPRING
<element number>,<node # of REFD2>,<node # of SPEND>
*SPRING, ELSET=SPRING
2,
6.3E6,
*ELEMENT, TYPE=DASHPOTA, ELSET=DASHPOT
<element number>,<node # of REFD2>,<node # of SPEND>
*DASHPOT, ELSET=DASHPOT
2,
1.E4,

Define the 10 kg mass associated with die 2.

*ELEMENT, TYPE=MASS, ELSET=MASS
<element number>,<node # of REFD2>
*MASS, ELSET=MASS
10.,

You must define any desired sets for postprocessing.

*NSET, NSET=REF
REFP2, REFD2, REFDOMER, SPEND

*AMPLITUDE, NAME=RIGID, DEFINITION=SMOOTH STEP
0., 0., 1.E-6, 1.

*AMPLITUDE, NAME=FORM2, DEFINITION=SMOOTH STEP
0., 0., .033, 1.

Since an *ANNEAL step cannot be the first step in an ABAQUS/Explicit import analysis, begin the history by moving the rigid tooling into position. Moving the tooling into position is quite straightforward; the difficulty in this case is positioning the tools properly, given the unknown shape of the blank following springback. At the end of the first forming stage the position of the blank is known: the blank has been drawn to a depth of 0.015 m, and it is clamped between two rigid tools whose positions are known. However, during springback the blank is no longer constrained by the rigid tools, and it deforms freely to minimize its internal strain energy. The changes in shape during springback make it necessary to view the displaced shape following springback in ABAQUS/Viewer before positioning the rigid tools for the second forming stage.

After the first step it is imperative that there be no overclosure of contact pairs because, if such overclosure exists, it is resolved in a single increment. Resolving the overclosure results in a large velocity being imposed on an overclosed node, possibly distorting the associated elements and drastically increasing the kinetic energy. On the other hand, computer time is wasted if the rigid bodies are far away from the blank at the start of the step because the analysis runs while no deformation occurs in the blank.

Use ToolsQuery from the main menu bar in ABAQUS/Viewer to determine the coordinates of some nodes on the blank at the end of springback. The goal is to position the rigid bodies for the second forming stage as close as possible to the deformed blank without any overclosure. Even the slightest overclosure will cause analysis problems. Remember that you must consider the thickness of the shell when positioning the rigid bodies, since ABAQUS/Explicit considers the current shell thickness when performing contact calculations. The forming process is designed so that the curved parts of punch 2 and die 2 form concentric arcs with the blank in between. Punch 2 has a radius of 0.006 m, and it contacts the inner radius of the blank, which also has a radius of approximately 0.006 m after springback. Die 2 has a radius of 0.0065 m, and it contacts the outer radius of the blank, which—given its thickness of approximately 0.0005—also has a radius of approximately 0.0065 m. Include the *DIAGNOSTICS option with the CONTACT INITIAL OVERCLOSURE=DETAIL and DEFORMATION SPEED CHECK=DETAIL parameters to provide detailed information about possible initial overclosures and resulting excessive deformation speeds.

Use the amplitude definition named “RIGID” with the displacement boundary condition to move the rigid bodies into position. It is important that the velocity is zero at the end of the positioning step since the final velocity in the positioning step is the initial velocity in the second forming stage. Use the following step to position the rigid bodies for forming stage 2:

*STEP
*DYNAMIC, EXPLICIT
, 1.E-6
*RESTART, WRITE, NUMBER INTERVAL=1
*BOUNDARY, TYPE=VELOCITY
BSYM, 1, 2, 0.
BSYM, 6, 6, 0.
REFDOMER, 1, 1, 0.
REFDOMER, 6, 6, 0.
REFD2, 1, 1, 0.
REFD2, 6, 6, 0.
SPEND, 1, 1, 0.
REFP2, 1, 1, 0.
REFP2, 6, 6, 0.
*BOUNDARY, AMPLITUDE=RIGID
REFDOMER, 2, 2, <user-determined value>
REFD2, 2, 2, <user-determined value>
SPEND, 2, 2, <user-determined value>
REFP2, 2, 2, <user-determined value>
*DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=DETAIL,
DEFORMATION SPEED CHECK=DETAIL
*OUTPUT, HISTORY, TIME INTERVAL=1.E-5
*NODE OUTPUT, NSET=NHIST
U, V
*NODE OUTPUT, NSET=REF
U, RF
*ENERGY OUTPUT
ALLKE, ALLIE, ALLWK, ALLVD, ALLAE, ALLPD, ETOTAL
*OUTPUT, FIELD, NUMBER INTERVAL=4
*ELEMENT OUTPUT, ELSET=BLANK
STH, SF, S
*NODE OUTPUT
U,
*END STEP

Physically, annealing is the process of heating a metal part to a high temperature to allow the microstructure to recrystallize, removing dislocations caused by cold working of the material. The *ANNEAL procedure removes stresses and plastic strains from all deformable elements in the model without changing the shell thickness or deformed shape. The material properties are assumed to be the same before and after annealing. The *ANNEAL step is quite simple because there are no loadings or output requests permitted. The entire *ANNEAL step is as follows:

*STEP
*ANNEAL
*END STEP

In the second forming stage the deformed blank is clamped between punch 2 and die 2, which sits on a spring and dashpot. As punch 2 is moved 0.010 m in the negative 2-direction, the blank is forced to move in the negative 2-direction, pressing against the stationary domer in the flat region of the blank. At the end of the second forming stage the blank takes on a dome shape in the previously flat region, while retaining the vertically drawn region from the first forming stage. Since the analysis is similar to the first forming stage, assume that the step time, damping, and mass scaling are the same as for the first forming stage. The loading rate in this stage of the forming simulation is actually slower than that in the first stage because the distance swept by the second punch is shorter while the step time remains the same.

Add the following to your input file for forming stage 2:

*STEP
*DYNAMIC, EXPLICIT
, .033
*FIXED MASS SCALING, FACTOR=10
*DIAGNOSTICS, CONTACT INITIAL OVERCLOSURE=DETAIL, 
DEFORMATION SPEED CHECK=DETAIL
*CONTACT PAIR, INTERACTION=INTER
PUNCH2, BLANK_TOP
DIE2, BLANK_BOT
DOMER, BLANK_BOT
*SURFACE INTERACTION, NAME=INTER
*FRICTION
.1,
*BOUNDARY, TYPE=DISPLACEMENT, AMPLITUDE=FORM2, OP=NEW
REFP2, 2, 2, -0.010
*BOUNDARY, TYPE=VELOCITY, OP=NEW
REFP2, 1, 1, 0.
REFP2, 6, 6, 0.
REFD2, 1, 1, 0.
REFD2, 6, 6, 0.
SPEND, 1, 2, 0.
REFDOMER, 1, 6, 0.
BSYM, 1, 1, 0.
BSYM, 6, 6, 0.
*MONITOR, NODE=<node # for REFD2>, DOF=2
*RESTART, WRITE, NUMBER INTERVAL=10
*END STEP

Save your input data in a file called draw_stage2.inp. Run the analysis using the following command:

abaqus job=draw_stage2 oldjob=draw_spring1_std

Again you must evaluate the quality of the results as you did following the first forming stage to make certain that there are no severe dynamic effects to damage the analysis. We will not discuss the details of checking the results again because the procedures are the same as were used to check the results from the first forming stage. Some of the things to check are the histories of the kinetic energy, ALLKE, and the velocity of the reference node for die 2.

Die 2 moves as it is pushed by the blank, which is pushed by punch 2. Since the bodies may not be exactly in contact at the start of the step, some impact may occur as the bodies interact. When the blank impacts die 2, even with a small velocity, die 2 will oscillate somewhat since it sits on a spring and dashpot. Although it is best to avoid these oscillations as much as possible, they have little effect on the solution because the predominant forming is occurring in the dome region. The deformed model following the second forming stage is shown in Figure 7–31.