CHAPTER 5 FINITE ELEMENT ANALYSIS AND AN ANALYTICAL APPROACH OF WARM DEEP DRAWING OF AISI 304 STAINLESS STEEL SHEET

Transcription

1 97 CHAPTER 5 FINITE ELEMENT ANALYSIS AND AN ANALYTICAL APPROACH OF WARM DEEP DRAWING OF AISI 304 STAINLESS STEEL SHEET 5.1 INTRODUCTION Nowadays, the finite element based simulation is very widely used by many researchers to analyze the sheet metal processes successfully. Accurate prediction of the effects of various process parameters on the detailed metal flow became possible only recently, when the finite element method was developed for the analyses (Shiro Kobayashi et al 1989).The finite element based simulations are carried out in order to investigate the maximum drawing loads, the thickness, radial and hoop strains all expressed in percentages, in warm deep drawing of circular cups from AISI 304 stainless steel sheets. The finite element results at room temperature and at different experimented warm temperatures are compared with those of the experimental values for validation. Many researchers tried the analytical method to find out the thickness distribution in the deep drawn cup, LDR value, height of the drawn cup and the drawing force in the conventional deep drawing process. Very few researchers used the analytical methods in warm deep drawing process and still much to be developed in this regard. To name the few researchers used analytical methods are: Korhonen (1982), Ramaekers et al (1994), Cho et al (2002), Cwiekala et al (2011), Bai et al (2011) in conventional deep

2 98 drawing ; Swadesh Kumar Singh and Ravi Kumar (2005), Azodi et al (2008) in hydro-mechanical deep drawing; Chandra and Kannan (1992) (i & ii), Jung-Ho Cheng (1996), Hwang et al (1997) in super plastic forming and Hong Seok Kim et al (2008) in warm deep drawing. From the literature survey, it is observed that most of the current research work in warm deep drawing are concentrated on the experimental and FE simulations alone and very little focus has been made on analytical methods. In this research work, an attempt is made to analytically find out some of the parameters like thickness distribution in the deep drawn cup, LDR value, drawing force in warm deep drawing process of AISI stainless steel sheet at different temperatures ranging from room temperature to 300 o C. The calculated values by analytical methods are compared with those of the experimental and FE simulations results for its accuracy of prediction. 5.2 FINITE ELEMENT ANALYSIS ON WARM DEEP DRAWING In metal forming technology, proper design and control requires, among other things, the determination of deformation mechanics involved in the processes. Without the knowledge of the influences of variables such as material properties, workpiece geometry, friction and contact conditions on the process mechanics, it would not be possible to design the dies and equipments adequately, or to predict or prevent the occurrence of defects in the components produced. Thus, process modeling for computer simulation has been a major concern in modern metal forming technology Commercially Available Software Packages for Finite Element Analysis on Warm Deep Drawing There are many commercially available software packages for finite element method such as NUMISHEET 93, DEFORM, AUTOFORM,

3 99 DD3IMP, LS-DYNA, MSC.MARC, PAM-STAMP, ANSYS and ABAQUS etc. 2-Dimensional (2D) and 3-dimensional (3D) simulation for finite element analysis is possible in these software packages. Recently, Mark Colgan and John Monaghan (2003) have combined experimental and finite element analysis using the program AUTOFORM and Padmanabhan et al (2007) have performed the finite element method combined with Taguchi technique using deep drawing 3 dimensional implicit codes (DD3IMP) to analyze the deep drawing operation ABAQUS Software Package The ABAQUS software is a product of Dassault systèmes simulia corporation, USA. ABAQUS/CAE is a complete ABAQUS environment that provides a simple, consistent interface for creating, submitting, monitoring and evaluating results from ABAQUS/Standard or ABAQUS/Explicit simulations. Different modules are available in ABAQUS/CAE such as defining the geometry, defining the material and generating the mesh etc., and each module defines a logical aspect of modeling process. Once all or required modules are defined, a model is built from which the ABAQUS/CAE generates an input file which is submitted to ABAQUS/Standard or ABAQUS/ Explicit for analysis. Analysis is performed and the information is sent to the ABAQUS/CAE so that the user can know the progress of the job and any error indicated can be rectified. Once the input is accepted successfully, the job is analyzed and the result database is generated. Finally the visualization module helps to read the output database and to view the results of the analysis. The meshing of parts of the model is very important in any analysis by finite element method. In ABAQUS, there are many types of elements that are available for meshing. To name a few, the widely used softwares are:

4 100 CAX4R- 4 node, reduced integration, axisymmetric quadrilateral element, SAX1- first order, axisymmetric shell element, S4R- first order, finite strain quadrilateral shell element, MAX1 first order, axisymmetric membrane element etc (ABAQUS user s manual 2009) Finite Element Analysis of Warm Deep Drawing of AISI 304 Stainless Steel Using ABAQUS Software Package The finite element method (FEM) based simulations of deep drawing using ABAQUS/CAE at room temperature, 100 o C, 200 o C, and 300 o C are carried out for a circular shaped cups which are drawn from AISI 304 stainless steel sheet. The results from the simulations are compared with the experimental values with respect to the maximum drawing load, strains like thickness strains, radial strains and hoop strains. In deep drawing, the metal is held between the die and the blank holder and the punch forces the material into the die to form a component with the desired size and shape. The ratio of drawing against stretching is controlled by the force on the blank holder and the friction conditions at the interfaces between blank-die and blank holder- blank. Higher blank holder force and friction at these interfaces limit the slip at the interface and increases the radial stretching of the blank. So, it is essential to control the slip at these interfaces in order to deep draw successfully. Rupture or necking occurs, if the slip is restrained too much, due to the severe stretching of the material, whereas, wrinkles will form, if the material flows very easily into the die and so proper interface conditions are very much important for the satisfactory results during deep drawing process simulation (ABAQUS user s manual 2009). The flow chart of methodology used for the FEM based simulation of deep drawing of circular cups is shown in Figure 5.1.

5 Figure 5.1 Flowchart for FEM simulation methodology 101

6 Finite element model and geometry All finite element models are created using ABAQUS/CAE pre processor which are analyzed in this study and investigations. The axisymmetric FEM model created for analysis is shown in the Figure 5.2 and the 3D model is shown in the Figure 5.3. PUNCH Ø Ø 20 R 5 BLANK HOLDER 1.0 BLANK R 6 Ø 42 Ø DIE All dimensions in mm Figure 5.2 Finite element model of circular cup deep drawing Figure 5.3 3D Model for FEM simulation of deep drawing process

7 103 For the analysis in ABAQUS/CAE, the punch, die, and the blank holder are modeled as analytically rigid surfaces whereas only the blank is defined as deformable body. The blank is meshed by the element CAX4R, a four node bilinear axisymmetric quadrilateral elements with reduced integration. These elements belong to the family of solid elements and are of the first order, which means that the strain is computed as an average over the element volume instead of the first order gauss point (Magnus Söderberg 2006). The feature of reduced integration used in the CAX4R element causes the integration order to be lower than full integration; in this case only one integration point in the centre of the element is used. With the use of reduced integration, the number of constraints which are introduced by the elements is reduced, and this prevents locking in the elements causing a stiff response. The drawback of this technique is that no energy is registered in the element integration point for certain modes of deformation and these modes are usually referred to as hourglass mode which is addressed in ABAQUS using hourglass control algorithm (Magnus Söderberg 2006). The blank is modeled using 20 elements of type CAX4R in order to match with the grid pattern used in the experimental analysis. These meshes are coarser for this analysis. However, since the primary interest in this problem is to study the membrane effects, the analysis will still provide a fair indication of stresses and strains occurring in the process. Thickness changes and membrane effects are modeled properly with CAX4R element however, the bending stiffness of the element is very low. The element does not exhibit locking due to incompressibility and the element is very cost- effective due to lesser computational time when compared to other elements (ABAQUS user s manual 2009).

8 Material properties The material used in the simulation of deep drawing process and the important properties of the material are shown in the Table 5.1. Table 5.1 Important material properties of AISI304 austenitic stainless steel used in FEM simulations S.No. Property Value 1 Density 7.8 g/cc 2 Young s modulus 210 GPa 3 Poisson ratio 0.3 The plastic stress-strain values used in this analysis are from the flow curves of stainless steel 304 obtained experimentally up to the temperatures of 200 o C by Eren Billur et al (2009). The stress values for the corresponding strain values for 300 o C are extrapolated by numerical method. The material model used in these analyses is isotropic Von Mises hardening model Contact and boundary conditions The contact between the blank and the tools is enforced by a kinematic contact condition, using pure master-slave surface pairs established in the first step of the solution. The surfaces of the analytically rigid bodies are defined as the master surfaces and the surfaces defined on the blank form the slave surfaces. The friction between the contact surfaces is implemented with a coulomb model. The boundary conditions are defined for each step of the simulation which defines the displacement of the blank, punch, die, and blank holder and the type of loading.

9 Loading conditions The entire finite element analysis is carried out in five steps. In the first step, the blank holder is moved onto the blank with the prescribed displacement to establish the contact. The second step involves the removal of the boundary condition and application of the blank holder force of 100 KN and this force is kept constant for step 2 and 3. The third step is the actual deep drawing process in which the punch pushes the blank with the defined punch force of 300 KN into the die through a total distance of 32 mm, that is, the height of the cup (30 mm) plus the initial clearance (2 mm) between the punch and the top surface of the blank. The important process parameters used during the deep drawing step is shown in the Table 5.2. In the fourth step, all the nodes of the model are fixed in their current position and the contact pairs are removed from the model and the last step is to withdraw the punch back to its original position. Table 5.2 Important process parameters used in FEM simulations S.No. Process parameter Value 1 Punch speed 60 m/min 2 Friction coefficient (ABAQUS user s manual 2009) (a) Blank-punch 0.25 (b) Blank-die 0.10 (c) Blank-blank holder Assumptions Made in the Simulations (i) The material is assumed to be isotropic which means that it has similar properties in all directions.

10 106 (ii) The material is assumed to satisfy the relationship between the true stress and true strain given by Hollomon (1945) which is mathematically expressed by the equation (5.1). = K n (5.1) (iii) The mechanical interaction between the contact surfaces is assumed to be the frictional contact. (iv) For shells and membranes, the thickness change is calculated from the assumption of incompressible deformation of the material. (v) It is assumed that no reverse loading occurs during simulation and so the Bauchinger effect is not modeled. 5.3 APPLICATION OF ANALYTICAL METHOD IN WARM DEEP DRAWING Flow Stresses and Strains in Warm Deep Drawing of Stainless Steel Sheet The flow stress and strain of the material is very important parameter in deciding the forming characteristics of the material especially in deep drawing operation. There are many constitutive material equations are available to relate the flow stress and the flow strain which is known as the flow curve equation and depending on the situation, the appropriate equation may be used for accurate results. The flow stress and strain values of AISI 304 stainless steel sheet material with 1.0 mm thickness for the analytical and FEM simulations in this research work are used from the experimental values obtained by hydraulic bulge test at various temperatures and strain rates by Eren Billur et al (2009).

11 107 In this work, it is assumed that the material obeys the Hollomon strain hardening equation (5.1) = K n The parameters K and n are determined by fitting the equation (5.1) using least square method and the flow stresses are calculated for the different strains and also for different temperatures up to 200 o C Thickness Distribution in the Warm Deep Drawn Cup The change in the thickness of the material, when it is deep drawn from the blank into a desired shape and dimensions, occurs due to plastic deformation and also due to the influence of temperature in warm deep drawing. The prediction of the amount and region of maximum reduction of thickness is the primary concern of the designer in order to design a part without the occurrence of fracture either during manufacturing or while in use in future. A new methodology is developed to calculate the thickness distribution in the warm deep drawn cup of AISI 304 stainless steel material and the steps involved are as follows: (i) For the elements/nodes on the blank which moves on the top surface of the die before reaching the die corner radius while deep drawing, the thickness at the die entry (t e ) is calculated by the equation (5.2) which is derived by Ramaekers et al (1994). = (5.2)

12 108 (ii) When the element bends over the die radius, the change in thickness is calculated using the equation (5.3) given by Marciniak et al (2002). (5.3) where, T 0 0 t 0 (5.4) T y y t 0 (5.5) (iii) When the element leaves the die radius, it unbends and gets straighten and the change in thickness is again calculated using the equation (5.3) (iv) When the element wrap around the punch corner radius also the equation (5.3) is used for calculating the thickness value. (v) Identify the elements which undergo the types of deformation as mentioned above and apply the appropriate equations to determine the final thickness of the element of the deep drawn cup. (vi) The same procedure is adopted for warm deep drawing also by using the corresponding material constants at that temperature. In the experimental study of the present work, the measurements are made at the positions of 0, 6, 12, 18, 24, 30, 36 and 42 mm from the center of the blank. For the analytical prediction also, the same nodes/ elements are considered in order to compare the calculated values with those of

13 109 experimental and FEM simulation results. The types of deformation that the nodes/elements undergo are stated below: (i) The node/element at 42 mm and 36 mm move along the top surface of the die and bend at the die corner radius. (ii) The node/ element at 30 mm and 24 mm move along the top surface of the die and bend as well as unbend to straighten at the die radius. (iii) The node/ element at 18 bend and unbend at the die radius and also bend at the punch corner radius. (iv) The node/ element at 12 mm, 6mm and center of the blank theoretically do not undergo any deformation and the thickness remains unchanged. It is assumed that the value of 0 = 0.01, since the pre strain, in most of the cases, is less than 0.01 (Ramaekers et al 1994). For AISI 304 stainless steel, R = 1 ; y = 262 MPa Initial thickness of the blank (t 0 ) = 1.0 mm The value of 0 is calculated using the values of 0, appropriate K and n from the equation (5.1) Analytical Method of Determination of LDR Values and Height of the Deep Drawn Circular Cup The LDR values at different temperatures are calculated using the equation (5.6) from the literature of Swadesh Kumar Singh and Ravikumar (2005).

14 110 = + 1 (5.6) The drawing efficiency ( ) for different temperatures are initially assumed and finally checked with the experimental drawing efficiency values by using the equation 5.7 from George E. Dieter (1987). Since the flow stress values are decreased when the temperature is increased, the assumed drawing efficiencies are 70% at room temperature (Kurt Lange 1985), 80% at 100 o C, 90% at 200 o C, and 95% at 300 o C. LDR e (5.7) The deep drawn height of the cup is determined by the equation (5.8) (Marciniak et al 2002). 1 (5.8) Analytical Method of Determining the Punch Force The punch force excluding the blank holding force, force required to overcome the friction, die cushion force and consideration of the factor of safety is calculated from the equation (5.9) given by Korhonen (1982). F p = (5.9) Since the flow stress, yield stress and ultimate tensile strength are decreased, when the temperature is increased, it is assumed that the ultimate tensile strength decreased by 15% when the temperature is increased from room temperature to 100 o C; further decreased by 10% of the stress value at

15 o C, when the temperature is increased from 100 o C to 200 o C; and finally, decreased by 10% of the stress value at 200 o C, when the temperature is increased from 200 o C to 300 o C. The punch force is calculated at different temperatures and compared with the punch force obtained in the experiments. 5.4 SUMMARY Finite element based simulations of deep drawing of stainless steel AISI304 circular cups are carried out using ABAQUS/CAE software at different temperatures from room temperature (30 o C) to 300 o C at an increment of 100 o C. The results of FEM simulations on drawing loads, the maximum thinning region location and thickness, radial and hoop strain measurements are compared with those of experimental results for validation. A new methodology for the determination of thickness distribution using analytical method in the warm deep drawn cup is proposed and the LDR values, height of the deep drawn cups and the punch force at different temperatures are calculated using the analytical methods which are used for conventional deep drawing process by determining the materials constants of the strain hardening equation at each temperature. The results of analytical methods are compared with those of experimental results for its accuracy of predictions.