Since large strains involved in the process, nonlinear analysis was performed [15]. It was a dynamic problem in which the contact loads on the blank varied in each forming time step. The established sheet metal forming simulation model was submitted to the solver Ls-Dyna, to calculate the accurate nodal forces on each elements nodes during sheet metal forming simulation.
The results of sheet metal forming simulation were detailed in Fig. 4, which presented the load-displacement curves from the generated RCFORC file during SMF simulation. The abscissa represented the stamping stroke, while the ordinate indicated the corresponding resultant forces in X, Y, and Z directions of all contact nodes between the die components and blank. It was noteworthy that the resultant forces escalated rapidly and peaked at the end of press stroke (i.e. simulation end time). The obtained peak forming force in the Z direction was 5700 KN (as illustrated in Fig. 4), which was implemented as boundary conditions in the next procedure for structural analysis.
3.2. Linear static structural analysis
The sheet metal forming simulation of long beam was firstly conducted in order to evaluate the accurate contact forces at the end of stamping. As the drawing dies generally operated in the linear range of materials, linear static structural analysis was performed in this subsection to investigate the structural behaviors of die components. Besides the attained contact loads, another loading cases were considered in the die structural analysis, in which the lifting forces during transportation were also applied to the die analysis model.
To prevent unnecessary problems, some small geometry features (e.g. fillets included in die 3D geometric models) were removed prior to discretizing the geometry models into 3D meshes. To get a perception of the die components, different views of the original die were shown in the following figures, as illustrated in Fig. 5.
Due to the complexity of drawing die structure, 10-node 3D tetrahedral elements offering more precision with six additional nodes were chosen to discretize the die components. In this work, the punch and die shoe were modeled with approximately 430,000 tetrahedral elements. The punch also referred as the die post, which was constructed of Cr12MoV cast steel, and the die shoe was fabricated by HT300 cast iron. In linear static structural analysis, three material properties (i.e. elastic modulus, Poisson’s ratio, and density) were required to predict die structural behaviors under loading. The material properties for the punch and die shoe are presented in Table 3. Cast steel, which was a ductile material, exhibited similar performance when subjected to tension and compression conditions. While for the brittle material, cast iron, behaved much stronger in compression than in tension, with very little yielding occurred and the failure mode was fracture.
Table 3 Material properties for the die components.
Different load cases were considered in this study. The first load case was the forming load case, which represented the die components under peak load condition. The force boundary was attained from the sheet metal forming simulation, where the contact pressure and drawbead forces on the die were calculated. Such contact pressure vectors could be represented by X, Y, and Z nodal contact force components, which were directly transferred from rigid shell meshes to the deformable solid elements established for linear structural analysis, using an efficient load mapping algorithm. The die shoe was clamped or bolted to the bolster of the press, thus the model for this load case was constrained in the X, Y, and Z directions at the bottom surface nodes. The established linear structural model for the load case 1 is presented in Fig. 6. The obtained nodal forces were implemented on the corresponding elements nodes in X, Y, and Z directions. The length of the arrows reflected the magnitude of the load, and the direction of the arrows indicated the direction of load.
The analysis models were calculated in the linear solver Optistruct. To explore the structural behaviors of this long beam drawing die, the results of linear structural analysis were analyzed. In this study, the die shoe was constructed of HT300 cast iron, a brittle material that exhibited stronger performance in compression than tension. Thus, the die shoe was most susceptible to failure due to tensile stresses. Hence, the maximum tensile principal stress (i.e. P1 Stress) was applied as the main indicator to evaluate the behaviors of the die shoe, although all three principal stresses (P1, P2, P3 Stress) were calculated by the solver. Meanwhile, the die post made of Cr12MoV cast steel was judged by the von mises stress.
Results and analyses of the stresses in forming load case could be viewed in Figs. 7 and 8, For the punch, the maximum von mises stress reached 471 MPa, occurring at the sharp corner of the punch surface, as shown in Fig. 7. Sharp corners tended to concentrate stress, resulting in highly localized stress in these areas [17, 18]. For the die shoe, the stress eccentricity was observed in the reinforcement ribs, the von mises stress in the Y direction was obviously larger than that in the -Y direction, due to the asymmetrical shape of the target part. The von mises stress of the reinforcement ribs in Y direction reached 85 MPa, while only 26 MPa recorded in the -Y direction, as illustrated in Fig. 8.
The results of displacement are shown in Figs. 9 and 10. The deformation experienced by the punch (including the direction and magnitude of the displacements) was also taken into account. The magnitude of the deformation experienced by the punch reached 0.209 mm, as shown in Fig. 9. The punch was mainly deformed mainly in the Y and Z directions. Specifically, the relative displacement in Y direction of the punch was 0.197 mm. The deformation in X direction was shown in Fig. 10, which was negligible, as only 0.044 mm was recorded in positive direction and -0.040 mm in negative direction. Besides, it was worth noting that the deformation in X direction was symmetrical about the Y axis. This was because the shape of the target part in the X direction was almost symmetrical, and the contact forming forces in the X direction loaded on both sides of the punch were almost equal which could cancel each other out.
The second load case was a transportation case, which was an operation for transportation and cleaning. In production, transportation of stamping dies was set as a four point lifting operation and lifting lugs were applied to attach all die components to facilitate transport. Since the dies were generally lifted with a very small and negligible acceleration, the lifting load case was also considered as a static condition. In the lifting load case, the nodes in the lifting lugs were constrained in all degrees of freedom except for the X-axis rotation. Only the die shoe instead of the entire beam drawing die was selected to conduct structural analysis for lifting load case, since the die shoe structure suffering the greatest force during the lifting operation. The structure supported to be lifted in four lifting lugs. The established mechanical model of the lifting load case was shown in Fig. 11, where P1, P2 were the equivalent pressure transferred by the weight of other die components (g=9.8 m/s2).
Results for the lifting load case were presented in Figs. 12 and 13. For the original die shoe structure, the maximum tensile principal stress (i.e. P1 Stress) of 11.8 MPa was achieved in the case of lifting load, and the maximum displacement was around 0.022 mm.
3.3. Topology optimization of stamping die component
The topology optimization method exhibits great potential in terms of mass reduction [16, 19]. In this subsection, the topology optimization process of the long beam drawing die component was conducted, and then the structures were redesigned based on the initial topology optimization results. Most importantly, the linear structural analysis of the redesigned structure was performed for strength verification by imposing the same level of forming load and a lifting load. To analyze the results of redesigned die structure, the displacements and von mises stress in the structure were investigated and compared with ones from the original structure.
The boundary conditions (derived from SMF simulation), materials properties (defined the same as those in linear structure analysis as mention before) were required prior to define the design space, which was set as design variables of the die topology optimization model. The outer materials contacting with the blank for forming and assembling with other components were determined as non-design space, which would be excluded from density manipulation for optimization solver. The rest of the volume was assigned as available design space which would be optimized, as shown in Fig.14. The non-design space with blue color in the figure remained unchanged during optimization, and the green space was assigned as design space.
In the establishment of topology optimization problem for the long beam drawing die, the design variables, constraints, together with optimization objective were determined. Setting a volume fraction of 0.30, the volume of the optimized design area was required to be at most 30% of the initial design space volume. The objective function was defined to find the minimum compliance (i.e. the maximum stiffness) for given a certain available amount of material volume.
Results from the topology optimization are shown in Fig. 15, which met the objective function and constraints to minimize the compliance and use a volume fraction of 0.30. The outer red frame in the figures indicated that the density of this material was 1.0 and the material could not be removed.
It was worth noting that the obtained initial optimized structure was a conceptual design, which could not be fabricated with current manufacturing techniques. Thus, further efforts should be made to reconstruct the structure based on the initial optimized results. In addition, when executing the die structure reconstruction, both current manufacturing techniques and design principles for die structure in industrial practice should also be taken into account. The reconstructed structure is shown in Fig. 16. As mentioned earlier in the proposed methodology, to verify the structural strength, the redesigned structure was meshed and then subjected to the same load cases. The same steps (as illustrated in Fig. 1) were conducted with the original die structure and analyses were made in both cases ( i.e. forming load case and lifting load case). In order to study the efficiency of weight reduction, results (i.e. stresses, displacement as well as the weight of the new structure) would be compared with the original structure. Results of the linear structural analysis are shown in Figs. 17 to 20.
To evaluate the effectiveness of this methodology, a table was summarized as presented in Table 4, where the numerical values of displacements, stresses and weight in the original and reconstructed die were illustrated. In comparison of the results, it was found that the reconstructed structures had a reduced mass of 18%, with 4.2% decrease of maximum von mises stress for the punch. For the reconstructed structure, the maximum tensile principal stress was 12.7 MPa, fulfilling the constraints settings upon it when lifting the structure in four supported lugs.
Table 4 Comparison between original and reconstructed die structure.