Spring-back Simulation of Sheet Metal Forming for the HT-7U Vacuum Vessel

Transcription

1 Spring-back Simulation of Sheet Metal Forming for the HT-7U Vacuum Vessel Yuntao Song *, Damao Yao, Songtao Wu, Peide Weng Institute of Plasma Physics, Chinese Academy of Sciences, (ASIPP) P.O. Box 116, Hefei, Anhui, * Tel: , Fax: Abstract The HT-7U vacuum vessel is an all-metal welded double wall toroidal structure, which has characteristics of ultra-high vacuum and thin shell. Cross-section of the vessel is noncircular, but D shaped. Now some of the forming tools will be fabricated according to its outline dimensions. In order to design a optimal shapes for the forming tools and avoid an undesirable local deformation at the head of sheet, authors utilized the software package ANSYS/LS- DYNA and DYNAFORM to simulate the process of the deep drawing in sheet metal forming and develop a parameter optimization system for the design of the die and punch. During the numerical simulation the updated LaGrange formulation and elastic-plastic constitutive equation were adopted to solve the problem of large strain and large deformation in sheet forming process. According to the simulation analysis results the optimum shape of the die and punch surface was finally determined. Keywords: Sheet metal forming, Spring-back simulation, Finite Element Method 1.Introduction The HT-7U vacuum vessel is one of the key parts for HT-7U superconducting tokamak device. It can provide an ultra-high vacuum and cleanly location for the operation of plasma. The vessel has a double-wall toroidal structure interconnected with two toroidal stiffening ribs. The channels formed between the ribs and walls are filled with boride water as a nuclear shielding. Base pressure for the design is 1.3x10-5 Pa. The whole HT-7U vacuum vessel consists of 16 sectors. During final assembly, they are all field welded together to form toroid. The vessel outermost radius is.7m and height is.58m. Fig.1 has shown its configuration with ports arrangement [1][]. The thickness of each shell is only 8mm. Compared with its circumflexion radius the shell thickness is very smaller. So it has a characteristic of ultra-high vacuum and thin shell. The crosssection of vessel is noncircular, but D shape, which has six different dimensions along its circumference including one beeline. Each piece of arc shell also has two curvatures in the space of three dimensions with circumference radius itself r i and the sweep axis radius R. Their structures are shown in Fig..Now all kind of the R&D programs is in progress. The primary forming tools of HT-7U vacuum vessel are being designed. In this work Fig.1. Schematic view of the HT-7U Vacuum Vessel some of crucial and complex problems must be considered, such as localized buckling, undesirable local deformation at the head of panel and excessive spring back on the end of panel because of the plastic deformation and residual stresses. According the traditional techniques method the process of forming tools design and construction required a tryout in which the die and the punch are reworked to compensated for spring-back after a sheet metal stamping operation. It is very difficult to predict and control accurately the spring-back deformation for this kind of large hyperbolical shell - 1 -

2 along the two-curvature radius. This method also Fig.. Single shell for the 1/16 vacuum Vessel has no cost-efficient and waste lots of time moreover. So it become a very important research project how to simulate the spring-back deformation for the shell of HT-7U vacuum vessel. In recent years, with the rapid advancement of computer technologies the numerical simulation of sheet metal forming focused on the finite element analysis. In order to find the optimal shapes for the technical surface on the die and punch some kinds of software ANSYS/LS-DYNA and DYNAFORM were used in the numerical simulation. The paper has presented the dynamic simulation for sheet metal forming process. According to the simulation analysis results the optimum shape of the die and punch surface was finally determined..principal theory for numerical simulation In the metal forming operation, the highly nonlinear deformations processes tend to generate a large amount of elastic strain energy in the metal material besides of the some plastic deformation area. The elastic energy, which stored in the metal sheet during the forming, is subsequently released after the forming pressure is removed. This release of energy is the driving force for spring-back of sheet metal forming. Hence, the spring-back deformation for the sheet metal forming are mainly lie on the amount of elastic energy stored in the part while it is being plastically deformed. There are numerous factors that influence elastic energy stored in metal sheet, such as the shape of the die, the properties of the material, the boundary conditions and the interfacial loads. All of these factors must be taken into account in the springback simulation. In order to get an accurate simulation results an elastic-plastic finite element code based on Mindlin shell theory was employed to analysis. The equilibrium equations are derived from the principle of virtual work and elastoplastic constitutive relation [3] [4]. The updated LaGrange formulation was adopted in the solver of the incremental deformation for metal sheet forming. The virtual work formulation for the dynamic elastic-plastic finite element code is as bellow: U& Τ δ ( f ρu&& vu& dω = Ω ) σ δddω Ω s T δu& T TdS Where Ω and S T are the volume of the configuration and the area of the surface under at time t, respectively, and f, ρ u& &, and v u& are the volume force, inertia force and the damp force, respectively, on the configuration of time t. The D is the strain tensor and σ is the Kirchhoff Stress tensor. Ρ, ν and u are the density of material, damp coefficient and displacement, respectively. T is the pressure acting on the body surface[5]. During forming process the deformation history and boundary are very complex. The element used in the simulation should be able to characterize the three-dimensional deformation in the sheet-metal forming processes. The authors employed a type of 4-node degenerated shell element for the simulation. And the material of metal sheet under roller often has a distinct characteristic of anisotropy. So in the model Hill s yield function is used. For the thin shell element it can be regarded as a planar stress state, that is the σ 33 =0. Then the yield function can be obtained f ( σ ij ) = σ σ ij ) = Fσ + Gσ 11 + H ( σ 11 σ ) + Nσ 1 Where F, G, H, L, M, N are the anisotropy parameters and σ ij is the yield stress. [6] [7] During the sheet metal forming process, the contact and friction between the metal sheet and the die including the impacted flange usually change. It is necessary to satisfy this kind of compulsive boundary condition caused by the contact in the - -

3 calculation. A kinetic-restriction method is adopted in this paper, which can accord with additive contact boundary condition. On the computation of the increment between the step n and the step n+1 under the punch making a small travel, firstly no consider the contacting and got the deformation according to the result of step n+1,then search the nodes begin contact and calculate the contact force. In each iteration the same sequence of operations is repeated until the convergence is obtained. The friction between the die and the metal sheet obey the Coulomb law: τ F = µσ N Where the τ F is the shear friction force, σ N is the normal contact force; μ is the coefficient of friction. 3. Design of the forming tools Before the numerical simulation, a primary forming tool was designed. Owing to the welding procedure for vacuum vessel the inner shell and outer shell was divided into six segments in conformity to their different dimensions. So the largest and typical segment was chosen to illuminate the shell forming process. The dimensional sketches are shown in Fig.3. Each one of the forming tool s dimensions is selected under a conservative evaluation according to the theory formulation for the cooling forming. It is only to provide a preparatory dimension for the next simulation on which R and r i is 119mm and 345mm respectively. The upper punch and the down die are all selected the casting. Fig.3. Design of the forming tools Fig.4. Finite element model for the simulation 4. Numerical simulation for spring-back Based on the structure and its geometry dimension, the forming tools including the punch and die has the axial symmetry characteristic. Considering the computer capacity a 1/ part was chosen to performing its spring-back simulation. The axonometric view of a 3 D finite element model is shown in Fig.4, which included the upper punch, down die and the metal sheet. The dimension of R, r i and r 0 are all parameter variables. Thickness of the metal sheet is defined 8 mm. Two kinds of 4-node shell element were selected as the model finite unit. One is the shell163, and the other is shell181. It has 341 nodes, 5018 elements and 1848 equations in all. Shell163 is an element with both bending and membrane capabilities. Both in-plane and normal loads are permitted. It has 1 degrees of freedom at each node: translations, accelerations, and velocities in the nodal x, y, and z directions and rotations about the nodal x, y, and z- axes. The element is used in explicit dynamic analyses only. Shell181 is suitable for analyzing thin to moderately-thick shell structures. It is a four-node element with six degrees of freedom at each node: translations in the x, y, and z directions, and rotations about the x, y, and z-axes. Shell181 is well-suited for linear, large rotation, and/or large strain nonlinear applications. In the process of the spring-back simulation an explicit-to-implicit sequential solution method was used, in which firstly simulated the dynamic forming process explicitly in ANSYS/LS-DYNA, - 3 -

4 Fig.7. Spring-back deformation before cutting Fig.5. σ-ε relation curve of 316L stainless steel and then modeled the spring-back deformations implicitly by removing statically the forming pressure in ANSYS. This method can relieve the calculations tolerances in a great extent and get an accurate simulation results for the sheet metal forming operations. DYNAFORM was used to proceeding the preprocessor and postprocessor.[8] Due to decrease the eddy current and the electromagnetic force while the plasma disruption, a kind of nonmagnetic stainless steel 316L are chosen for the HT-7U vacuum vessel structure material. The σ-ε relation curve of the steel used in the analysis is shown in the Fig.5 and other mainly parameters are Young s modulus, E=196GPa, Poisson s ratio μ=0.3,yield stress S y =7Mpa, respectively. Considering the impacted flange around the brim on the die, the sheet metal is forbidden to move along the vertical direction. The friction coefficient between the metal sheet and the die are defined as 0.15 acquiescently. Lastly, the inverted draw and toggle draw was selected and then made the normal surface of punch and die to plumb with the metal sheet. An auto Fig.6. Spring-back deformation without cutting Fig.8. Changes of the sheet metal thickness position operation for the forming tool was applied when the normal direction are consistent for all the elements of punch, die and the metal sheet. The maximum spring-back deformation for the sheet metal is 7.9mm before the cutting and 5.6mm after cutting. Fig.6 andfig.7 has shown the simulation results. The maximum plastic strain is only 0.031mm and the maximum stress on the sheet metal is 341MPa. Fig.8.has also given the detailed changes distribution of sheet metal thickness. 5. Summary The spring-back simulation of sheet metal forming for the HT-7U vacuum vessel has been performed using an elastic-plastic nonlinear finite element code. From the simulation process it has shown that is vital to the design of the forming tools used in the sheet stamping operation. This work is a an iteration process in which some spring-back simulation was calculated and then feedback to guide the design of the forming tools by providing a new shape dimensions to compensate the springback deformation. The design of the forming tools is repeated until reaching the desired spring-back amount, which matches exactly the sought-after geometry. According to the final simulation - 4 -

5 analysis results the optimum shape of the die and punch surface was finally determined. Now all kinds of these forming tools are fabricating in Shanghai & the Manufacture Center of ASIPP. 5. Acknowledgment All of the work presented here is the work of the HT-7U Vacuum vessel & PFC Team in ASIPP. The ANSYS, INC. Shanghai Office and the Research & Manufacture Center of ASIPP also support this work. The authors would like to express their sincere appreciation to all of members who participated and supported this study. References [1] D.m Yao et al. HT-7U vacuum vessel design, nd Symposium of Fusion Technology, September 9-13, 00, Helsinki, Finland [] S.T. Wu, The Modifications and Requirements of the HT-7U Tokamak Device Design, ASIPP Report, Sept [3] Xu weili,lin zhongxin,liu Guang, Li shuhui, State and trends of Auto-Body panel stamping simulation, Chinese Journal of Mechanical Engineering Vol.36,No.7,Jul.(000) [4] Shengqing Wang, The sheet forming simulation technology and its development in Japan, Journal of Plasticity Engineering, Vol.3, No., Jun. (1996) [5] Kong Yongming, Ma Ze-en,Liu Laiying, An simulation technology of sheet-metal forming with trial-and-error contact algorithm, J. Mater. Process. Technol.10 (00)1-5 [6] Dayong Li,Ping Hu,Ying Cao, Jincheng Wang, Section analysis of industrial sheet-metal stamping processes, J.Mater.Process.Technol.10(00)37-44 [7] Ye Wang,Qiyu Shen,Yuguo Wang, Yongqing Zhang, Research on applying one-step simulation to blank design in sheet metal forming, J. Mater. Process.Technol.10 (00) [8] Livermore Software Technology Corporation, LS-DYNA User s Manual, Jun.1997 [9] ANSYS/LS-DYNA3D Theoretical Manual for Release 5.4,ANSYS, inc.,