Products: ABAQUS/Standard ABAQUS/Explicit
This example illustrates the forming of a three-dimensional shape by a deep drawing process. The most efficient way to analyze this type of problem is to analyze the forming step with ABAQUS/Explicit and to import the results in ABAQUS/Standard to analyze the springback that occurs after the blank is removed from the tool with a static procedure. Since the forming process is essentially a quasi-static problem, the computations with ABAQUS/Explicit are performed over a sufficiently long time period to render inertial effects negligible. For verification purposes the complete analysis is also carried out with ABAQUS/Standard. However, this is computationally more expensive and will be prohibitively expensive for simulation of the forming of realistic, complex components.
The blank is initially square, 200 mm by 200 mm, and is 0.82 mm thick. The rigid die is a flat surface with a square hole 102.5 mm by 102.5 mm, rounded at the edges with a radius of 10 mm. The rigid square punch measures 100 mm by 100 mm and is rounded at the edges with the same 10 mm radius. The blank holder can be considered a flat plate, since the blank never comes close to its edges. The geometry of these parts is illustrated in Figure 1.5.2–1 and Figure 1.5.2–2. The rigid surfaces are offset from the blank by half the thickness of the blank to account for the shell thickness. While ABAQUS/Explicit automatically takes the shell thickness into account during the contact calculation, in ABAQUS/Standard the thickness is accounted for using “softened” contact (the pressure penetration curve defined with the *SURFACE BEHAVIOR option is shifted by half the blank thickness). A mass of 0.6396 kg is attached to the blank holder, and a concentrated load of 2.287 × 104 N is applied to the reference node of the blank holder. The blank holder is then allowed to move only in the vertical direction to accommodate changes in the blank thickness (this is only relevant in the ABAQUS/Explicit analysis since the thickness change is not taken into account in the ABAQUS/Standard contact calculations). The coefficient of friction between the sheet and the punch is taken to be 0.25, and that between the sheet and the die is 0.125. It is assumed that there is no friction between the blank and the blank holder.
The blank is made of aluminum-killed steel, which is assumed to satisfy the Ramberg-Osgood relation between true stress and logarithmic strain,
) of 513 MPa and a work-hardening exponent (
) of 0.223. Isotropic elasticity is assumed, with a Young's modulus of 211 GPa and a Poisson's ratio of 0.3. An initial yield stress of 91.3 MPa is obtained from these data. The stress-strain behavior is defined by piecewise linear segments matching the Ramberg-Osgood curve up to a total (logarithmic) strain level of 107%, with Mises yield, isotropic hardening, and no rate dependence.Given the symmetry of the problem, it is sufficient to model only a one-eighth sector of the box. However, we have employed a one-quarter model to make it easier to visualize. We use 4-node, three-dimensional rigid surface elements (type R3D4) to model the die, the punch, and the blank holder. The blank is modeled with 4-node, bilinear finite-strain shell elements (type S4R).
This problem was used by Nagtegaal and Taylor (1991) to compare implicit and explicit finite element techniques for the analysis of sheet metal forming problems. The computer time involved in running the simulation using explicit time integration with a given mesh is directly proportional to the time period of the event, since the stable time increment size is a function of the mesh size (length) and the material stiffness. Thus, it is usually desirable to run the simulation at an artificially high speed compared to the physical process. If the speed in the simulation is increased too much, the solution does not correspond to the low-speed physical problem; i.e., inertial effects begin to dominate. In a typical forming process the punch may move at speeds on the order of 1 m/sec, which is extremely slow compared to typical wave speeds in the materials to be formed. (The wave speed in steel is approximately 5000 m/sec.) In general, inertia forces will not play a dominant role for forming rates that are considerably higher than the nominal 1 m/sec rates found in the physical problem. The explicit solutions obtained with punch speeds of 10, 30, and 100 m/sec are compared with the static solution obtained with ABAQUS/Standard. The results at 10 m/sec are virtually indistinguishable from the static results. Minor differences can be observed at the intermediate speed of 30 m/sec. The results at 100 m/sec are considerably different from the static results. In the results presented here, the drawing process is simulated by moving the reference node for the punch downward through a total distance of 36 mm in 0.0036 seconds. Comparison of analyses of various metal forming problems using explicit dynamic and static procedures is discussed in the paper by Nagtegaal and Taylor.
Although this example does not contain rate-dependent material properties, it is common in sheet metal forming applications for this to be a consideration. If the material is rate-dependent, the velocities cannot be artificially increased without affecting the material response. Instead, the analyst can use the technique of mass scaling to adjust the effective punch velocity without altering the material properties. “Rolling of thick plates,” Section 1.3.6, contains an explanation and an example of the mass scaling technique.
The results from the forming simulation obtained using ABAQUS/Explicit are made available to ABAQUS/Standard by using the *IMPORT option with the parameter UPDATE=YES. The springback that occurs and the residual stress state are then determined by performing a static analysis in ABAQUS/Standard. During this step an artificial stress state that equilibrates the imported stress state is applied automatically by ABAQUS/Standard and gradually removed during the step. The displacement obtained at the end of the step is the springback, and the stresses give the residual stress state. Only the deformed sheet with its material state at the end of the ABAQUS/Explicit analysis is imported into ABAQUS/Standard. Boundary conditions are imposed in the ABAQUS/Standard analysis to prevent rigid body motion and for symmetry. The node at the center of the box is fixed in the z-direction.
The springback of the formed sheet is also analyzed in ABAQUS/Standard by setting UPDATE=NO on the *IMPORT option. In this case the displacements are the total values relative to the original reference configuration. This makes it easy to compare the results with the analysis in which both the forming and springback are analyzed with ABAQUS/Standard.
Further details of the import capability are discussed in “Transferring results between ABAQUS/Explicit and ABAQUS/Standard,” Section 7.7.2 of the ABAQUS Analysis User's Manual.
ABAQUS/Explicit provides two algorithms for modeling contact and interaction problems. The general contact algorithm, which is specified using the *CONTACT option, allows very simple definitions of contact with very few restrictions on the types of surfaces involved (see “Defining general contact interactions,” Section 21.3.1 of the ABAQUS Analysis User's Manual). The contact pair algorithm, which is specified using the *CONTACT PAIR option, has more restrictions on the types of surfaces involved and often requires more careful definition of contact (see “Defining contact pairs in ABAQUS/Explicit,” Section 21.4.1 of the ABAQUS Analysis User's Manual).
The general contact algorithm is used in the primary input file for this example; input files using the contact pair algorithm are also provided. Contact definitions are not entirely automatic with the general contact algorithm but are greatly simplified. The ALL ELEMENT BASED parameter on the *CONTACT INCLUSIONS option is used to specify contact automatically for the entire model; this is the simplest way to define the contact domain. This option specifies self-contact for an unnamed, all-inclusive, element-based surface (defined automatically by ABAQUS/Explicit) that contains all exterior element faces, shell perimeter edges, and feature edges in the model. This surface spans all of the bodies in the problem, so self-contact for this surface includes contact between the bodies. By default, the general contact algorithm uses the original shell thickness for the contact calculations throughout the analysis. In sheet forming analyses such as this problem, thinning of the sheet can significantly affect the contact model where the shell surface is pinched between other surfaces. In this analysis the *SURFACE PROPERTY ASSIGNMENT option is used to specify that the current thickness should be considered for the blank.
Double-sided surfaces are not available in ABAQUS/Standard, so two single-sided surfaces are used to model the blank when the forming step is modeled in ABAQUS/Standard: one surface to model the top of the blank and one to model the bottom of the blank. When a shell in ABAQUS/Standard is pinched between two surfaces, at least one of the constraints must use “softened” contact to prevent conflicting constraints. In the analysis in which the forming and the springback steps are carried out with ABAQUS/Standard, softened contact is used for all contact constraints. The contact stiffness is chosen sufficiently high so that the results are not affected significantly. Different contact stiffnesses are used for the contact with the blank holder, the die, and the punch. To describe the rounding of the punch accurately, a higher contact stiffness is needed for the contact with the punch. In ABAQUS/Standard the blank and the blank holder are initially brought into contact by applying a prescribed displacement to the blank holder in the first step. In this way rigid body motions are prevented. In the second step the blank holder force is applied to the blank holder.
Figure 1.5.2–3 and Figure 1.5.2–4 show contours of shell thickness in the blank after forming for the ABAQUS/Explicit and ABAQUS/Standard analyses, respectively. Figure 1.5.2–5 and Figure 1.5.2–6 show contours of equivalent plastic strain in the blank in the final deformed shape for the ABAQUS/Explicit and ABAQUS/Standard analyses, respectively. The predicted results are similar. The differences are caused by differences in the contact calculations. In ABAQUS/Explicit the change in shell thickness is accounted for during the contact calculations, while in ABAQUS/Standard the thickness is accounted for indirectly using softened contact and changes in the shell thickness are not considered during the contact calculations.
Closer inspection of the results reveals that the corners of the box are formed by stretching, whereas the sides are formed by drawing action. This effect leads to the formation of shear bands that run diagonally across the sides of the box, resulting in a nonhomogeneous wall thickness. Note also the uneven draw of the material from the originally straight sides of the blank. Applying a more localized restraint near the midedges of the box (for example, by applying drawbeads) and relaxing the restraint near the corners of the box is expected to increase the quality of the formed product.
Figure 1.5.2–7 shows the reaction force on the punch, and Figure 1.5.2–8 shows the thinning of an element at the corner of the box. The shell thicknesses predicted by ABAQUS/Explicit and ABAQUS/Standard differ by 4%.
The springback analysis runs in 6 increments in ABAQUS/Standard. Most of the springback occurs in the z-direction, and the springback is not significant. The corner of the outside edge of the formed box drops approximately 0.35 mm, while the vertical side of the box rises by approximately 0.26 mm. Figure 1.5.2–9 shows a contour plot of the displacements in the z-direction obtained from the springback analysis.
The analysis with UPDATE=NO on the *IMPORT option yields similar results. However, in this case the displacements are interpreted as total values relative to the original configuration.
Forming analysis with ABAQUS/Explicit using the general contact capability.
Forming analysis with ABAQUS/Explicit using kinematic contact pairs.
ABAQUS/Standard springback analysis with the UPDATE=YES parameter on the *IMPORT option.
ABAQUS/Standard springback analysis with the UPDATE=NO parameter on the *IMPORT option.
Forming and springback analyses done in ABAQUS/Standard.
Original mesh using penalty contact pairs in ABAQUS/Explicit.
Forming analysis of a fine mesh case using the general contact capability (included for the sole purpose of testing the performance of the ABAQUS/Explicit code).
Forming analysis of a fine mesh case using kinematic contact pairs (included for the sole purpose of testing the performance of the ABAQUS/Explicit code).
Springback analysis of a fine mesh case (included for the sole purpose of testing the performance of the ABAQUS/Standard code).
Nagtegaal, J. C., and L. M. Taylor, “Comparison of Implicit and Explicit Finite Element Methods for Analysis of Sheet Forming Problems,” VDI Berichte No. 894, 1991.
