Start ABAQUS/CAE (if you are not already running it). You will have to create four parts: a deformable part representing the blank and three rigid parts representing the tools.

The blank is made from a high-strength steel (elastic modulus of 210.0 × 10⁹ Pa, = 0.3). Its inelastic stress-strain behavior is shown in Figure 12–18 and tabulated in Table 12–1. The material undergoes considerable work hardening as it deforms plastically. It is likely that plastic strains will be large in this analysis; therefore, hardening data are provided up to 50% plastic strain.

Create a material named Steel with these properties. Create a homogeneous solid section named BlankSection that refers to the material Steel. Assign the section to the blank.

The blank is going to undergo significant rotation as it deforms. Reporting the values of stress and strain in a coordinate system that rotates with the blank's motion will make it much easier to interpret the results. Therefore, a local material coordinate system that is aligned initially with the global coordinate system but moves with the elements as they deform should be created. To do this, create a rectangular datum coordinate system using the Create Datum CSYS: 3 Points tool. From the main menu bar of the Property module, select AssignMaterial Orientation. Select the blank as the region to which the local material orientation will be assigned, and pick the datum coordinate system in the viewport as the CSYS (select Axis–1 and accept 0.0 for the additional rotation options).

You will now create an assembly of part instances to define the analysis model. Begin by instancing the blank. Then, instance and position the rigid tools using the techniques described below.

The final assembly is shown in Figure 12–19.

At this point it is convenient to create the geometry sets that will be used to specify loads and boundary conditions and to restrict data output. Six sets should be created: one at each rigid body reference point, one at the symmetry plane of the blank, and one at each end of the blank midplane. The last two sets require that a vertex first exist at these locations; an edge partition can be performed to satisfy this requirement.

Begin by partitioning the vertical edges of the blank in half using the procedure described below.

There are two major sources of difficulty in ABAQUS/Standard contact analyses: rigid body motion of the components before contact conditions constrain them and sudden changes in contact conditions, which lead to severe discontinuity iterations as ABAQUS/Standard tries to establish the exact condition of all contact surfaces. Therefore, wherever possible, take precautions to avoid these situations.

Removing rigid body motion is not particularly difficult. Simply ensure that there are enough constraints to prevent all rigid body motions of all the components in the model. This may mean using boundary conditions initially to get the components into contact, instead of applying loads directly. Using this approach may require more steps than originally anticipated, but the solution of the problem should proceed more smoothly.

Unless a dynamic impact event is being simulated, always try to establish contact between components in a reasonably smooth manner, avoiding large overclosures and rapid changes in contact pressure. Again, this usually means adding additional steps to the analysis to move components into contact before fully loading them. This approach, although requiring more steps, will minimize convergence difficulties and, therefore, make the solution far more efficient. With these points in mind, we can now define the steps for this example.

The simulation will consist of five steps. Since the simulation involves material, geometric, and boundary nonlinearities, general steps must be used. In addition, the forming process is quasi-static; thus, we can ignore inertia effects throughout the simulation. A brief summary of each step (including the details of its purpose, definition, and associated output requests) is given below. However, the details concerning how the loads and boundary conditions are applied are discussed later.

You can request that ABAQUS monitor the value of a degree of freedom at one selected point. The value of the degree of freedom is shown in the Job Monitor and is written at every increment to the status (.sta) file and at specific increments during the course of an analysis to the message (.msg) file. In addition, a plot of the degree of freedom value over time appears in a new viewport that is generated automatically when you submit the analysis. You can use this information to monitor the progress of the solution.

In this model you will monitor the vertical displacement (degree of freedom 2) of the punch's reference node throughout each step. Before proceeding, make the first analysis step (Establish contact I) active by selecting it from the Step list located under the toolbar. The monitor definition applied for this step will be propagated automatically to all the subsequent steps.

Contact must be defined between the top of the blank and the punch, the top of the blank and the blank holder, and the bottom of the blank and the die. The rigid surface must be the master surface in each of these contact interactions. Each contact interaction must refer to a contact interaction property that governs the interaction behavior.

In this example we assume that the friction coefficient is zero between the blank and the punch. The friction coefficient between the blank and the other two tools is assumed to be 0.1. Therefore, two contact interaction properties must be defined: one with friction and one without.

Define the following surfaces: BlankTop on the top edge of the blank; BlankBot on the bottom edge of the blank; DieSurf on the side of the die that faces the blank; HolderSurf on the side of the holder that faces the blank; and PunchSurf on the side of the punch that faces the blank.

Now define two contact interaction properties. (In the Model Tree, double-click the Interaction Properties container to create a contact property.) Name the first one NoFric; since frictionless contact is the default in ABAQUS, accept the default property settings for the tangential behavior (select MechanicalTangential Behavior in the Edit Contact Property dialog box). The second property should be named Fric. For this property use the Penalty friction formulation with a friction coefficient of 0.1.

Finally, define the interactions between the surfaces and refer to the appropriate contact interaction property for each definition. (In the Model Tree, double-click the Interactions container to define a contact interaction.) In all cases define the interactions in the Initial step and use the default finite-sliding formulation (Surface-to-surface contact (Standard)). The following interactions should be defined:

The Interaction Manager shows that each interaction has been created in the Initial step and propagated to all subsequent steps, as shown in Figure 12–20.

Recall that the first stage of the process is to hold the blank between the blank holder and the die. At the start of the first increment of the analysis contact may not be fully established between the various components, even though their surfaces are coincident initially. Problems can occur when contact is not fully established: components may undergo rigid body motion; or the contact status may oscillate between open and closed, which is known as chattering. Chattering is especially common in contact analyses with multiple components.

To avoid rigid body motions and chattering in this simulation, the endpoints of the midplane of the blank will be fixed in the vertical direction to prevent the blank from moving initially. These points are used because constraints should not be applied to regions that are also part of a contact surface. If a contact region is constrained by a boundary condition in the direction that contact occurs, there will be two constraints applied to a single degree of freedom. This can cause numerical problems, and ABAQUS/Standard may issue a zero pivot warning message in the message file.

One method of establishing contact is to apply a force to the blank holder. However, the blank holder may undergo rigid body motion in the vertical direction because contact between the blank holder and the blank may not be fully established. Therefore, it is better to move the blank holder by means of an applied displacement. This ensures firm contact between these two surfaces. In addition, move the die slightly upward to establish firm contact between it and the blank. The magnitude of the applied displacement should be large enough so that firm contact is established yet small enough so that plastic yielding does not occur.

Constrain the blank holder and die in degrees of freedom 1 and 6, where degree of freedom 6 is the rotation in the plane of the model. All of the boundary conditions for the rigid surfaces are applied to their respective rigid body reference nodes. Constrain the punch completely, and apply symmetric boundary constraints on the region of the blank lying on the symmetry plane (geometry set Center).

Table 12–2 summarizes the boundary conditions applied in this step:

Now that contact between the blank and the blank holder and die has been established, the blank is fully constrained in the 2-direction. Therefore, deactivate the boundary condition on the right side of the midplane of the blank (it is no longer necessary). To do this, open the Boundary Condition Manager and click the cell under Remove right constraint in the row for boundary condition MidRightBC. Click Deactivate on the right side of the dialog box.

In this step the boundary condition used to move the blank holder down should be removed and replaced with a concentrated force. There should be no problems replacing the applied displacement on the blank holder with a force because there is firm contact between the blank holder and the blank. In this simulation the required blank holder force is 440 kN. Generally, care should be taken to ensure that the newly applied force is of the same order as the reaction force generated from the boundary condition so that the contact condition does not change significantly.

Using the Boundary Condition Manager, edit the RefHolderBC boundary condition in Step 3 to remove the constraint on U2.

Create a mechanical concentrated force in this step named RefHolderForce. Apply the load to set RefHolder in step Holder force. Specify a magnitude of –440.E3 for CF2.

In this step the punch must be moved down in the 2-direction just enough to achieve contact with the blank. The vertical constraint on set MidLeft should be removed, and a small pressure should be applied to the top surface of the blank to pull it onto the surface of the punch.

Using the Boundary Condition Manager, deactivate the MidLeftBC boundary condition in Step 4 and change the RefPunchBC boundary condition to specify a value of –0.001 for U2.

It can be difficult to choose the proper magnitude of pressure to apply. In this analysis you should use a pressure magnitude (1000 Pa) that produces a force on the blank that is three orders of magnitude lower than the blank holder force. A positive pressure acts into the surface; however, in this simulation you want the pressure to act out of the surface, so use a negative pressure. This technique is used to prevent chattering of the BlankTop and Punch surfaces.

Create a mechanical pressure load named Small pressure. Apply the load to the surface BlankTop in step Establish contact II. Specify a magnitude of -1000.0.

In this step remove the pressure load applied to surface BlankTop, and move the punch down to complete the forming operation. When a pressure load is removed in a static analysis, the magnitude is ramped down to zero over the duration of the step. Therefore, the pressure will continue to pull on the surface BlankTop and hold it tightly against the punch, maintaining contact between the surfaces, particularly in the early part of the step. This helps prevent chattering between the punch and the blank at the beginning of the forming process. As long as the force created by the pressure is small compared to the force required to move the punch, it will have little effect on the solution. Using the Load Manager, deactivate the Small pressure load in this step. Using the Boundary Condition Manager, edit the RefPunchBC boundary condition to specify a value of –0.031 for U2. This represents the total displacement of the punch, accounting for the initial offset of 0.001 m.

For reference, the contents of the Boundary Condition Manager appear in Figure 12–21.

Before continuing, change the name of your model to Standard.

You should consider the type of element you will use before you design your mesh. When choosing an element type, you must consider several aspects of your model such as the model's geometry, the type of deformation that will be seen, the loads being applied, etc. The following points are important to consider in this simulation:

Create a job named Channel. Give the job the following description: Analysis of the forming of a channel. Save your model to 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.

Once the analysis is underway, an X–Y plot of the values of the degree of freedom that you selected to monitor (the punch's vertical displacement) appears in a separate viewport. From the main menu bar, select ViewportJob Monitor: Channel to follow the progression of the punch's displacement in the 2-direction over time as the analysis runs.

To illustrate how to interpret the contact diagnostic information in ABAQUS/CAE, consider the iterations in the sixth increment of the fourth step. As shown in Figure 12–23, this is one of the first increments in which severe discontinuity iterations are required. ABAQUS/Standard requires one iteration to establish the correct contact conditions in the model; i.e., whether or not the punch was contacting the blank. The second iteration does not produce any changes in the model's contact condition, so ABAQUS/Standard checks the force equilibrium. One additional iteration is required to converge on static equilibrium. Thus, once ABAQUS/Standard determines the correct contact state, it can easily find the equilibrium solution.

To further investigate the behavior of the model in this increment, look at the visual diagnostic information available in ABAQUS/CAE. The diagnostic information written to the output database file provides detailed information about the changes in the model's contact conditions. For example, the node number and location in the model of every slave node whose contact status changes in a severe discontinuity iteration, as well as the contact interaction to which it belongs, can be obtained using the visual diagnostics tool.

Enter the Visualization module, and open the file Channel.odb to look at the contact diagnostics information. In the first severe discontinuity iteration of the fourth step, 46 nodes on the blank experience contact overclosure, indicating that their contact status should be changed. This can be seen in the Contact tabbed page of the Job Diagnostics dialog box (see Figure 12–25). To see where the nodes are located on the model, toggle on Highlight selections in viewport.

ABAQUS/Standard removes the contact constraints from these nodes and performs another iteration; this time ABAQUS/Standard detects no changes in the contact state and, therefore, carries out the normal equilibrium convergence checks. The solution in this iteration does not satisfy the force residual tolerance check, so another iteration is performed. This time, the force residual tolerance check is satisfied and the displacement correction is acceptable relative to the largest displacement increment, as shown in Figure 12–26. Thus, the second equilibrium iteration produces a converged solution for this increment.

The basic result of this simulation is the deformation of the blank and the plastic strain caused by the forming process. We can plot the deformed model shape and the plastic strain, as described below.

The maximum plastic strain is 21.4%. Compare this with the failure strain of the material to determine if the material will tear during the forming process.

It is important to check that the force required to push the punch into the blank is much larger than the force created by the pressure applied to the surface of the blank. The force on the blank from the applied pressure is approximately 100 N (1000 Pa × 0.1 m × 1.0 m) at the start of Step 5. The solid line in Figure 12–29 shows the variation of the reaction force RF2 at the punch's rigid body reference node.

The punch force, shown in Figure 12–29, rapidly increases to about 160 kN during Step 5, which runs from a total time of 4.0 to 5.0. The punch force clearly is much larger than the force (100 N) created by the pressure load.

ABAQUS/CAE includes a number of features designed specifically for postprocessing contact analyses. Within the Visualization module, the Display Group feature can be used to collect surfaces into display groups, similar to element and node sets.