外文翻译---冲压工艺中几何及内圆角对模具应力产生的影响.docx

附录a 外文文献effects of geometry and fillet radius on die stresses in stamping processesabstract: this paper describes the use of the finite element method to analyze the failure of dies in stamping processes. for the die analyzed in the present problem, the cracks at different locations can be attributed to a couple of mechanisms. one of them is due to large principal stresses and the other one is due to large shear stresses. a three-dimensional model is used to simulate these problems first. the model is then simplified to an axisymmetric problem for analyzing the effects of geometry and fillet radius on die stresses. 2000 elsevier science s.a. all rights reserved.keywords: stamping; metal forming; finite element method; die failure1. introductionin metal forming processes, die failure analysis is one of the most important problems. before the beginning of this decade, most research focused on the development of the- oretical and numerical methods. upper bound techniques 1,2, contact-impact procedures 3 and the finite element method (fem) 4,5 are the main techniques for analyzing stamping problems. with the development of computer technology, the fem becomes the dominant technique 6-12.altan and co-workers 13,14 discussed the causes of failure in forging tooling and presented a fatigue analysis concept that can be applied during process and tool design to analyze the stresses in tools. in these two papers, they used the punching load as the boundary force to analyze the stress states that exist in the inserts during the forming process and determined the causes of the failures. based on these concepts, they also gave some suggestions to improve die design.in this paper, linear stress analysis of a three-dimensional (3d) die model is presented. the stress patterns are then analyzed to explain the causes of the crack initiation. some suggestions about optimization of the die to reduce the stress concentration are presented. in order to optimize the design of the die, the effects of geometry and fillet radius are discussed based on a simplified axisymmetric model.2. problem definitionthis study focuses on the linear elastic stress analysis of the die in a typical metal forming situation (fig. 1). the die (fig. 2) with a half-moon shaped ingot on the top surface is punched down towards the workpiece which is held inside the collar, and the pattern is made onto the workpiece. cracks were found in the die after repeated operation: (i) when the die punched the workpiece, there is crack initiation between the tip of the moon shaped pattern and one of the edges (crack i); and (ii) after repeated punching, there is also a crack at the fillet of the die (crack ii).the present work was carried out with the following objectives: (i) to establish the causes of the crack initiation; and (ii) to study the effects of geometry and fillet radius.3. simulation and analysis3.1. 3d simulationthe simulation is performed with the fem code abaqus 15. twomeshes are created for the die shown in fig. 3a and b. the 3d solid elements for the workpiece are c3d8 (8- node linear brick) elements. there are about 4000 nodes and 3343 elements in the coarse mesh model, and 7586 nodes and 6487 elements in the fine mesh model. the boundary condition involves fixing the bottomof the die, i.e., u2=0 for all the nodes on the die bottom. a pressure of 200 mpa is applied on the top surface of the half-moon pattern. youngs modulus is 200 gpa and poissons ratio is 0.3.in order to analyze the principal stress concentration area in the region of crack i, different cases are studied. let the models shown in fig. 3a and b be case 1. a new 3d model (case 2) is used as shown in fig. 3c. the die is separated into three parts. the abaqus command *contact pair, tied is used to tie separate surfaces together for joining dissimilar meshes. the advantage of this model is its convenience in changing the mesh of the half-moon pattern and its position. first, the half-moon pattern is moved 6 mm towards the center (case 3) as shown in fig. 3d. second, the fillet radius of the half-moon pattern is changed from 0 to 0.5 mm (case4) as shown in fig. 3e.3.2. results and discussionfor the two meshes used in case 1. the maximum principal shear stress (s12) distribution at the region of fillet are shown in fig. 4a and b. the results show that the stress distribution patterns are the same for the two different meshes, and therefore, the convergence of the solutions is established.altan and co-workers 14 have presented the stress analysis of an axisymmetric upper die. in their work, when the material of the workpiece flows to fill the volume between the dies and collar, the contact surface of the die is stretched. at the area of the transition radius, the principal stresses change direction and reach high tensile values.according to their analysis, the fatigue failure is due to two factors: (i) when the stress exceeds the yield strength of the die material, a localized plastic zone generally forms during the first load cycle and undergoes plastic cycling during subsequent unloading and reloading, thus microscopic cracks initiate; and (ii) tensile principal stresses cause the microscopic cracks to grow and lead to the subsequent propagation of the cracks.the von mises stress distribution is shown in fig. 5a. very high stress occur in the half-moon and fillet regions. if the contact pressure keeps increasing, plastic zones will form first in these two regions.fig. 5b shows the maximum principal stress (sp3) distribution pattern. in order to show the area of crack i initiation, fig. 5c provides a zoomed view of the area. it is clear that a tensile principal stress (sp3) concentration of 25.5 mpa exists between the half-moon pattern and the free edge and is the cause of crack initiation.since crack i propagates nearly normal to the 1-2 plane, the direction of the stresses which cause the crack initiation must be parallel to that plane. fig. 5d shows the direction of the maximum principal tensile stress at node 145 and confirms crack i is normal to the 1-2 plane.after repeated punching, crack ii initiates in the fillet region, and gives rise to fatigue failure. the geometry in the local area is very similar to the case which altan and co-workers 14 have analyzed. however, there are no contacts tresses in that area for the present case, and fig. 5b shows that the maximum principal stresses are all compressive at the fillet. fig. 5e shows that there is high shear stress (s12) concentration at the fillet which is about 30 mpa. the shear stresses seem to be the stresses which lead to the initiation and propagation of cracks.the results of the four cases (cases 1-4) for the largest maximum principal stresses are listed in table 1.when the number of elements for the half-moon pattern is increased from 10 to 70, the largest principal stress at the position of crack i initiation is increased by (30.5-25.5)/ 30.5=16%(case 2). the principal stresses are very sensitive to the half-moon pattern.cases 2-4 show the effect of location of the half-moon and its fillet radius. if the half-moon pattern is moved 6 mm towards the center, the largest principal stress at the position of crack i is reduced by (25.3-30.5)/30.5=-17% (case 3). if the fillet radius of the half-moon pattern is changed to 0.5 mm, the principal stress is reduced (28.5-30.5)/ 30.5=-7% (case 4). therefore both these methods can reduce the stress concentration, the first being more effective.4. effects of geometry and fillet radius on die stress distribution4.1. 2d modelingin order to optimize the die, the effects of geometry and fillet radius on die stress distribution are discussed further. an axisymmetric model is used (fig. 6) for the analysis.initially, the radius r1 of the inner cylinder is set to 10 mm, the height h of the inner cylinder is set to 5 mm, and the height h of the outer cylinder is set to 25 mm. also, r2 is the radius of the outer cylinder, and the ratio r2/r1 is changed from 1.2 to 1.5, 2.0, 3.0 and 4.0. the radius r of the fillet ischanged from 2.0 to 0.5 mm, and h is changed from 5 to 2 and 0 mm. the pressure is given as 200 mpa at the top surface. the nodes at the bottom edge are fixed, and all others are free to translate (except those on the axis in the radial direction).4.2. results and discussiona total of 30 cases were studied. parameters that are varied include r2/r1 ratio, h, and fillet radius r. these 30 cases are shown in table 2. for all cases, r1 is fixed at 10 mm and h is fixed at 25 mm.4.2.1. effect of r2/r1the effect of varying the r2/r1 ratio is examined for cases with the value of h fixed at 5 mm. fig. 7a-c with the value of h fixed at 5 mm and varying ratio of r2/r1 shows that the maximum value of the principalstress (sp3) reduces with increasing r2/r1, and changes in position from a point on the surface to below the surface. this trend is reflected in fig. 8a.on the other hand, fig. 8b indicates that the maximum shear stress (s12) becomes larger with increasing ratio of r2/r1. the rate of this increase drops with increasing r2/r1. the shear stress patterns for some cases are shown in fig. 7f-h.4.2.2. effect of height hthe effect of height h of the inner portion is examined for three cases with h=0, 2 and 5 mm with r fixed at 2 mm. from fig. 8a, it can be seen that the maximum principal stress (sp3) increases marginally with increasing h up to r2/r1 of 2, after which the trend is reversed. however, for large h, the effect becomes less important. on the other hand, the maximum shear stress is higher with increasing h for the same r2/r1 ratio. stress patterns are shown in fig. 7a, d-f, i and j.4.2.3. effect of fillet radius rthe effect of fillet radius r is examined for two cases with r=0.5 and 2 mm. the results are shown in fig. 8c and d. it can be seen that for r2/r1 larger than 2, the maximum principal stress (sp3) is relatively insensitive to changes in the fillet radius. for r2/r1 ratio less than 2, a larger fillet radius results in a larger principal stress. however, the changes in the principal stress are less drastic compared with the changes in the maximum shear stress (s12) shown in fig. 8d.from fig. 8d, it can be seen that themaximum shear stress nearly doubles when the fillet radius is reduced from 2 to 0.5 mm for the same r2/r1 ratio. stress patterns are shown in fig. 7a, f, k and l.fig. 8. showing: (a) sp3 for r2/r1=1.2-4.0, h=0-5 mm, r=2 mm; (b) s12 for r2/r1=1.2-4.0, h=0-5 mm, r=2 mm; (c) sp3 for r2/r1=1.2-4.0, h=5 mm r=0.5 and 2 mm; (d) s12 for r2/r1=1.2-4.0, h=5 mm, r=0.5 and 2 mm.4.2.4. suggestion for optimum performancebased on the above analysis, some possible optimum solutions for the axisymmetric model can be achieved, as below.1. both the maximum principal stress (sp3) and maximum shear stress (s12) are larger with increasing h. thus, h should be relatively small.2. with changes in r, the values of sp3 and s12 show different trends. if the maximum principal stress is more likely the cause of die failure, r should be changed to a smaller value. conversely, if the maximum shear stress is the cause, r should be larger. generally speaking, the value of r should be between 1.5 and 2.0 for the dimensions used here.3. the effects of r2/r1 on sp3 and s12 are significant when r2/r1 is less than 2. however, the trends are different. if the maximum principal stress is the cause of die failure, r2/r1 should be changed to a larger value, otherwise r2/r1 should be smaller.5. conclusionsthe finite element code abaqus has been used for die stress analysis. a 3d model is used to analyze the different mechanisms of crack initiation. this method not only pre-dicts the causes of cracks, but also the direction of crack propagation.subsequently, a 2d model is used to study the effects of die geometry and fillet radius on the stress distribution. some guidelines on die design are given. at the early stage of die design, the fem can help to predict possible failure and to optimize die design so as to save cost and time. the results are valuable both in theoretical research and indus-trial application.冲压工艺中几何及内圆角对模具应力产生的影响摘要： 本文描述使用有限元法分析冲压工艺中产生的模具故障问题。在以下问题中，模具的不同位置出现裂纹，这些可以归为机械装置领域。裂纹出现的原因之一在于主应力，原因之二在于剪应力。本文使用3d模型来模拟这些问题。3d模拟图使本文分析的问题简化成轴型问题。关键词：冲压 金属成型 有限元法 模具故障1. 简介金属成型过程中，分析模具故障是重要问题之一。21世纪初，大多数研究专注于理论和数字化方法。上限分析，冲击接触程序以及有限元法，是分析冲压工艺的三种主要方法。随着电脑科技的发展，有限元法成为突出的分析技术。埃尔顿及其合作者讨论了锻造工具失败的原因，并且展示了可应用于工序和工具设计的疲劳分析理念。在其两页的文章中，他们使用冲剪载荷作为边界力来分析成型过程中所受的应力情况，并且确定故障出现的原因。在此理念下，他们也给模具设计提出了建议。在这篇文章里，用线性应力分析3d模拟图，因此，应力图用来解释裂纹产生的原因。本文也提出了一些减少应力集中以优化模具的建议。为了优化模具设计，“几何及内圆角对模具的影响”放在简化的轴形图上讨论。2 问题说明本项研究专注于典型金属成型过程中模具的线弹性应力分析。如图1所示。图2 中，上表面的半月形模块向下朝轴环内的工件运动，模块嵌入工件内。反复操作后，模具上出现裂纹1，当模具碰撞工件时，在半月形模块和一个边缘之间出现裂纹1；(2) 反复碰撞后，模具圆角上出现裂纹2。本篇文章的研究目标：（1）确定裂纹产生的原因，（2）研究几何及内圆角的作用。图1. 典型金属成型过程图2.冲模裂纹1和23. 模拟和分析3.1 3d模拟模拟图使用有限元。如图3中a和b所示的两个网格图。三维实体单元为工件c3d8，(8-代码是线性砖)的元素。粗糙网格图中约有4000个节点和3343个元素，精细网格图中约有7586个节点和6487个元素。研究的基本条件包括：固定模具底部，模具底部所有节点的u2=0，半月形模块顶部受200mpa，初期模数是200gpa，泊松比率是0.3。为了分析裂纹1区域内的主应力集中区要研究多个案例。图3中a和b两个模型所展示的为案例1，图3中c图新模型展示为案例2，模具分成三个部分。使用有限元分析命令及接触副连接分开的表面。此模型的优点在于易于改变半月形模块的网格及其位置。首先，如图3中d图所示为案例3，半月形模块朝中心移到6毫米，然后，半月形模块内圆角由0变为0.5毫米。3.2 结果和讨论对于案例1中所使用的两个网络格，如图4中a和b所示，最大主剪向力分布在圆角区内。此结果显示，两个不同网格图受力区分布一样。因此问题可以归结为一个。埃尔顿及其合作者展示了模具顶端的轴形受力分析，在他们的研究中，当工件材料向下填充模具和圈之间的空间时，模具的接触面拉长，在承转半径区域，主应力改变方向并且达到一个高的拉力。图3.（a）粗网格（b）细网格（c）冲模网格的另一部分（d）月牙形向中心移动（e）月牙形不同变化的模式 根据他们的分析，导致疲劳故障的原因有两个：第一，当应力超出模具材质的强度时，局部塑性区在第一次循环负载中渐渐产生，并且在接下来的重复负载中经历塑性区。因此，微小的裂纹产生。第二，主应力拉伸致使微小的裂纹产生并最终导致其扩大。图5中a图所示，冯米塞斯应力分布，在半月形模块和内圆区产生较高的应力。加入接触面压力保持增长，塑性区在这两个区域内首先出现。图5中b图展示最大主应力分布。为了展示裂纹1出现的区域，图5中c提供乐儿放大的受力图。很明显，在半月形模块和自由边之间存在25.5mpa的里，这也是导致裂纹出现的原因。当裂纹增加至1-2个格时，导致裂纹产生的应力必须与此平面平行。图5中b图显示最大主应力在节点145上的方向，此图也确认了裂纹1相当于1-2个点。图4.（a）网格物体在圆角处的最大主剪应力（b）细网格物体在圆角处的最大主剪应力图5.应变应力分布反复撞击后，裂纹2出现在圆角区，因此而导致疲劳故障增加。 此研究中的区域与埃尔顿机器合作者所研究的非常相似。然而，当前问题中，此区域没有接触应力。图5中b图所示，在圆角区域最大的主应力都是收缩的。图5中e图所示，在圆角区有大约30mpa的剪应力。此剪应力好像是导致裂纹产生和扩大的原因。 案例1至案例4的主力效果如表格1。当半月形模块的组成元素由10增至70时，裂纹中最大主应力增至（30.5-25.2）/30.5=10% (案例2)，由此可见，最大主应力于半月形模块息息相关。案例2至去哪里4，显示半月形模块的位置及其内圆角的变化。如果半月形模块向中心移动6毫米，裂纹1处产生的最大主应力减少（25.3-30.5）/30.5=-17% （案例3）。如果半月形模块内圆角变成0