15665658 square-cup-deep-drawing-using-forming-limit-diagram

1,199 views

Published on

formability

Published in: Business, Technology
0 Comments
1 Like
Statistics
Notes
  • Be the first to comment

No Downloads
Views
Total views
1,199
On SlideShare
0
From Embeds
0
Number of Embeds
3
Actions
Shares
0
Downloads
53
Comments
0
Likes
1
Embeds 0
No embeds

No notes for slide

15665658 square-cup-deep-drawing-using-forming-limit-diagram

  1. 1. Chapter 55: Square Cup Deep Drawing using Forming Limit Diagram 55 Square Cup Deep Drawing using Forming Limit Diagram PART 1. Explicit Forming  Summary 1098  Introduction  Modeling Details  Results 1099 1101 1104 PART 2. Implicit Spring Back  Introduction 1108  Modeling Details  Results  Input File(s)  Reference 1110 1112 1112 1108
  2. 2. 1098 MD Demonstration Problems CHAPTER 55 Summary Title Chapter 55: Square Cup Deep Drawing using Forming Limit Diagram Features • Failure criterion based on the Forming Limit Diagram • Springback: Explicit -> Implicit switching Geometry Punch Clamp Sheet Die Material properties • Sheet Metal (aluminum sheet): Anisotropic Materials under Plane Stress Conditions Exx = 71.0 GPa,  = 0.33 Stress constant = 0.0 MPa, Hardening modulus = 576.79 MPa Strain offset = 0.01658, Exponent for power-law hardening = 0.3593 Lankford parameters: R0 = 0.71, R45 = 0.58, R90 = 0.70 • Punch, Die, and Clamp: Rigid Analysis characteristics Transient explicit dynamic analysis (SOL 700 explicit single precision) Nonlinear implicit static analysis (SOL 700 implicit double precision) Boundary conditions • Explicit: Fixed boundary condition of Die and Clamp • Implicit Springback: Fixed at the center point of the plate Element types 4-node shell elements FE results Stress Contour Plot, Forming Limit Diagram and more Explicit Forming Implicit Spring Back Element will fail at next step 80.00% FLD at Mid. Surface FLD with Safety margin Major True Strain (%) 60.00% 40.00% 20.00% 0.00% -30.00% -20.00% -10.00% 0.00% -20.00% Minor True Strain (%) 10.00% 20.00%
  3. 3. CHAPTER 55 1099 Square Cup Deep Drawing using Forming Limit Diagram PART 1. Explicit Forming Introduction This is a sheet metal forming example of a plate with anisotropic behavior that is drawn through a square hole by means of a punch. This particular example has experimental results from a verification problem of the 1993 NUMISHEET Conference held in Japan. The results are obtained at single punch depth (20 mm punch travel) for an aluminum alloy plate. The material is seen to be anisotropic in its planar directions; i.e., the material behavior is different for all directions in the plane of the sheet metal as well as in the out of plane direction. The data obtained from the NUMISHEET Conference is as follows: Aluminum Alloy Thickness = 0.81 mm Young’s modulus = 71 GPa Poisson’s ratio = 0.33 Density = 2700 kg/m3 Yield stress = 135.3 MPa Stress = 576.79 * (0.01658 + p)0.3593 MPa Lankford parameters: R0 = 0.71, R45 = 0.58, R90 = 0.70 Friction coefficient = 0.162 The size of the plate modeled was 0.15 x 0.15 (in meters). No strain-rate dependency effects were included in the material data, so the metal sheet was analyzed without these effects. The dimensions of the plate, die, punch, and clamp are all given in Figure 55-1. SOL 700 Entries Included SOL 700 TSTEPNL DYPARAM,LSDYNA,BINARY,D3PLOT CSPH PSPH EOSGRUN SPHDEF TIC MATD010 PSOLIDD MATD003
  4. 4. 1100 MD Demonstration Problems CHAPTER 55 Figure 55-1 Dimensions of Plate, Die, Punch, and Clamp (in Millimeters)
  5. 5. CHAPTER 55 1101 Square Cup Deep Drawing using Forming Limit Diagram Modeling Details Punch Clamp Sheet Die Z X Figure 55-2 Y SOL 700 Model (Exploded View) The SOL 700 model is shown in Figure 55-2. The main parts in the finite element model are: • • • • sheet metal punch die clamp Sheet Metal The SOL 700 material model for sheet metals is a highly sophisticated model and includes full anisotropic behavior, strain-rate effects, and customized output options that are dependent on material choice. Since not all of the materials can be derived from the simplified set given by the NUMISHEET organization, most participants in the conference used an isotropic material model. In reality, the process is definitely anisotropic and effects due to these differences can be seen in the transverse direction. For materials displaying in-plane anisotropic behavior, the effect would be even more noticeable. The parameters on the MAT190 (refer to the MD Nastran Quick Reference Guide) specify planar anisotropic behavior and are as follows (for the aluminum sheet): • MATD190 elastic material properties. • Isotropic behavior was assumed in the elastic range: Exx = 71.0 GPa = 0.33
  6. 6. 1102 MD Demonstration Problems CHAPTER 55 • Planar anisotropic yielding and isotropic hardening were assumed in the plastic range: A = Stress constant = 0.0 MPa B = Hardening modulus = 576.79 MPa C = Strain offset = 0.01658 n = Exponent for power-law hardening = 0.3593 • Lankford parameters: R0 = 0.71 R45 = 0.58 R90 = 0.70 Punch, Die, and Clamp These three components provide the constraints and driving displacement for the analysis and are modeled as rigid bodies. Contact is then specified with the metal sheet using the friction coefficient values provided. The three contact types are specified as following: • Contact between the punch and the sheet • Contact between the die and sheet • Contact between the clamp and sheet Finally, the punch is given a scaled downward velocity providing the driving displacement for the analysis. Input File SOL 700,NLTRAN stop=1 SOL 700 is an executive control entry and activates an explicit nonlinear transient analysis. Case control section is below: DLOAD = 1 IC = 1 SPC = 1 BCONTACT = 1 TSTEPNL = 1 The bulk entry section starts: BEGIN BULK $ TSTEPNL 1 $ DYPARAM LSDYNA 20 2.0E-3 BINARY D3PLOT 0.002
  7. 7. CHAPTER 55 1103 Square Cup Deep Drawing using Forming Limit Diagram TSTEPNL is a SOL 700 bulk data entry which describes the number of Time Steps (20) and Time Increment (2.00 ms) of the simulation. The end time is the product of the two entries. Notice here the Time Increment is only used for the first step. The actual number of Time Increments and the exact value of the Time Steps are determined by SOL 700 during the analysis. The time step is a function of the smallest element dimension during the simulation. LSDYNA,BINARY,D3PLOT option of DYPARAM entry controls the output time steps of d3plot binary file. The result plots at every 0.002 seconds are stored in d3plot binary file. Bulk data entries that define properties for shell elements PSHELL1 1 + .81 1 BLT Gauss MATD020 2 1 1.0 4 210.E9 7 + 0.3 The MATD020 entry defines the rigid material property. In the example, the clamp, die, and punch are modeled by the rigid materials. MATD190 1 2.7E-4 7.1E7 0.33 2.0 + 6.0 .71 .58 .70 + 2.0 77 + 1.0 0.0 + 0.0 1.0 TABLED1,77,,,,,,,,+ +,-100.0,196.67,0.0,30.,30.,45.,40.,47.,+ +,50.,45.,ENDT 576.79E3.3593 .01658 0 0.0 0.0 + + + + The MATD190 entry defines an anisotropic material developed by Barlat and Lian (1989) for modeling sheets under plane stress conditions and with Forming Limit Diagram failure criteria. This material allows the use of the Lankford parameters for the definition of the anisotropy. In the model, Gosh’s hardening rule is used: n Y  p  = k  0 + p  – p The forming limit diagram is defined in by TABLED1 as shown above. All fields are set for the coefficients of equations. See MD Nastran Quick Reference Guide for details. SPCD2,1,RIGID,MR2,3,0,100,1.0,,+ + TABLED1,100,,,,,,,,+ +,0.0,-1000.,0.02,-1000.,ENDT
  8. 8. 1104 MD Demonstration Problems CHAPTER 55 The SPCD2 entry defines imposed nodal motion on a node, a set of nodes or nodes of a rigid body. The rigid punch is moving downward at 1000 m/s from 0 to 0.02 seconds. FORCE 9999 MR3 -19.6E6 1. The FORCE entry defines a force on the grid point as well as rigids. Since the forces on the rigid body are not yet supported by the Nastran input processor, TODYNA and ENDDYNA entries are used in conjunction with the FORCE entry to by-pass the IFP (Input File Processor) and directly access SOL 700. BCTABLE 1 SLAVE 1 0 0.162 0. 0 3 0. 0 SS1WAY 0.162 0. 0 + + The BCBODY entry defines a flexible or rigid contact body in 2-D or 3-D. Although SOL 700 only supports flexible contact in BCTABLE, the rigid contact can be applied using the rigid material of contact bodies. In this example, all contact body pairs are given 0.162 static and kinetic friction coefficients. The surface-to-surface, one way contact method is used for all contact definitions. BCBODY .. $ BSURF .. 1 1 DEFORM 1 1 THRU 1600 The BCBODY entry defines a flexible or rigid contact body in 2-D and 3-D. The BSURF entry defines a contact surface or body by element IDs. All elements with the specified IDs define a contact body. $ GRID .. GRID $ CQUAD4 .. CQUAD4 1 -75. 75. 0.0 4528 -8.33333-37.0067-75.405 1 1 1 2 43 42 4468 63 4527 4273 4274 4528 Results To verify the result of MD Nastran, the major and minor principal strains at 0.015seconds are compared with those of Numisheet and Dytran results in Figure 55-3 and Figure 55-4. Left plots of each figure were represented by
  9. 9. CHAPTER 55 1105 Square Cup Deep Drawing using Forming Limit Diagram Makinouchi et al. (1993). The data in the plots were obtained from several companies which did the same test. MD Nastran gave a solution well within the spread of experimental values. Major Principal Strain 2.50E-01 2.00E-01 Strain 1.50E-01 1.00E-01 5.00E-02 0.00E+00 0 20 40 60 80 100 120 Distance from Center Along Line OB Figure 55-3 Comparison of Major Principal Strain Along Line OB (Numisheet and Dytran Results vs. MD Nastran SOL 700) Minor Principal Strain 0.00E+00 0 20 40 60 80 -5.00E-02 Strain -1.00E-01 -1.50E-01 -2.00E-01 -2.50E-01 Distance from Center Along Line OB Figure 55-4 Comparison of Minor Principal Strain Along Line OB (Numisheet and Dytran Results vs. MD Nastran SOL 700) 100 120
  10. 10. 1106 MD Demonstration Problems CHAPTER 55 80.00% Element will fail at next step FLD at Mid. Surface FLD with Safety margin Major True Strain (%) 60.00% 40.00% 20.00% -30.00% -20.00% -10.00% 0.00% 0.00% 10.00% 20.00% -20.00% Minor True Strain (%) Figure 55-5 Forming Limit Diagram Along Line OB at 0.019 Seconds
  11. 11. CHAPTER 55 1107 Square Cup Deep Drawing using Forming Limit Diagram t = 0.000 seconds t = 0.004 seconds t = 0.008 seconds t = 0.012 seconds t = 0.016 seconds Figure 55-6 t = 0.020 seconds Maximum Principal Strain Contour Plots at Mid Surface at Various Times Note that the FLD diagram correctly predicts the failure of elements at t = 0.019 as shown in the stress fringe plots.
  12. 12. 1108 MD Demonstration Problems CHAPTER 55 PART 2. Implicit Spring Back Introduction Springback refers to an event in which there is elastic strain recovery after the punch is removed. This deformation can alter the final desired shape significantly. In an explicit dynamic analysis, it can take some time before the workpiece comes to a rest, so the springback simulation is performed using the implicit solver to speed up this part of the analysis. Using explicit-implicit switching available in SOL 700, the residual deformations after sheet metal forming are computed and used as a pre-condition for springback analysis. Because, in this example, there was a failure at around 0.019 seconds in the sheet metal as shown in Part 1, the explicit simulation was terminated at 0.018 seconds. The initial condition, including the final stresses and deformation and the element connectivity of the explicit run are transferred to the implicit run. The analysis scheme is described below. SOL 700 Explicit (Use SEQROUT Entry) Generate jid.dytr.nastin SOL 700 Implicit (Include jid.dytr.nastin) (Use SPRBCK Entry) Figure 55-7 Analysis Scheme SOL 700 Entries Included SOL 700 MATD036 SEQROUT SPRBCK Modeling Details The model of explicit run is the same as Part 1. In the implicit run, only the sheet metal is used. Input File Explicit Input File BEGIN BULK $ TSTEPNL 1 10 1.8E-3
  13. 13. CHAPTER 55 1109 Square Cup Deep Drawing using Forming Limit Diagram As mentioned above, the end time of simulation is assigned to 0.018 seconds. SEQROUT 10 BCPROP 10 1 The SEQROUT entry generates the jid.dytr.nastin file at the end of simulation. The nastin file includes the final deformations and stresses of the assigned part. The nastin file can be used for a subsequent explicit or implicit SOL 700 run. In the example, only the result for Part 10 which includes the sheet metal is written out to the nastin file. Implicit Input File BEGIN BULK $ TSTEPNL 1 10 1.8E-3 As mentioned above, the end time of simulation is assigned to 0.018 seconds. Because all information of nodes and element connectivity is in jid.dytr.nastin file, Grid and CQUAD entries are removed in the implicit input. Only one point boundary condition at the center and SPRBCK entry are added in the input file. Since MATD190 is not available in the implicit analysis, MATD036 is used instead of MATD190. MATD036 and MATD190 are identical material models except that FLD is supported only in MATD190. MATD036 1 + 6.0 + 2.0 + + 2.7E-4 .71 7.1E7 .58 0.33 .70 2.0 1.0 0.0 0.0 1.0 576.79E3.3593 .01658 0 + 0.0 0.0 + + + MATD036 is only different in the failure criteria using FLD. Others are the same as MATD190 in the explicit simulations of Part 1 and 2. SPRBCK + + + 1 2 1 0.005 200 1 100 0.0 1.0E-2 1 1.00E-3 0.10 + + + SPRBCK activates the implicit spring back analysis. Nonlinear with BFGS updates solver type is used in the example. See MD Nastran Quick Reference Guide for other fields. SPC1 1 123456 841 Only one point at the center of the sheet metal is fixed to prevent singular condition in the implicit simulation.
  14. 14. 1110 MD Demonstration Problems CHAPTER 55 Results The springback simulation from explicit to implicit runs works fine. The results of explicit and implicit analyses are shown in Figures 55-8 to 55-10. Figure 55-8 shows the displacement contours at the start of analysis and at the end of analysis. Note that the initial deformation of the plate grids in the implicit analysis is set to zero because the final deformation of explicit analysis is applied to the initial location of grid points in the springback implicit analysis. In Figure 55-9 the initial stress condition of springback implicit analysis is perfectly coincident with the final stage of explicit analysis. The initial stress of implicit analysis causes the additional deformation in the springback implicit analysis. : Explicit Simulation t = 0.000 seconds t = 0.018 seconds (end of explicit run) Because the final results are applied as the initial condition for implicit simulation, the initial deformation of implicit simulation is set to 0. Implicit Simulation Initial condition of implicit run Figure 55-8 Final result of implicit run Vertical (Z-direction) Displacement Contour Plot
  15. 15. CHAPTER 55 1111 Square Cup Deep Drawing using Forming Limit Diagram Explicit Simulation t = 0.000 seconds t = 0.018 seconds (end of explicit run) Because the final results are applied as the initial condition of implicit simulation, the initial stress of implicit simulation is the same as the final stress of the explicit simulation. Implicit Simulation Initial condition of implicit run Figure 55-9 Final residual stress of implicit run von Mises Stress Contour Plot The location of each grid point along the diagonal line of the plate at the end of the explicit and the springback analysis is plotted in Figure 55-10; the maximum difference between these curves is around 0.756 mm. The centers of the implicit and explicit sheet are positioned to have the same position as a reference, hence the largest differences tend to appear at the ends of the sheet.
  16. 16. 1112 MD Demonstration Problems CHAPTER 55 at the end of explicit run 5 -100 -80 -60 -40 -20 0 20 40 60 80 0 100 -5 -10 -15 Deformation to vertical direction at the end of implicit run -20 Distance from center Figure 55-10 Comparison of Vertical Displacements (z-direction) After Explicit and Springback Simulations Along Diagonal Line of Plate Input File(s) File Description nug_55a.dat MD Nastran input file of explicit square cup deep drawing analysis using Forming Limit Diagram. nug_55b.dat MD Nastran explicit input file for springback analysis. nug_55c.dat MD Nastran implicit input file for springback analysis nug_55d.dat MD Nastran stress and deformation information of explicit analysis for input to implicit analysis Reference Makinouchi, A., Nakamachi, E., Onate, E., and Wagoner, R. H., “Numerical Simulation of 3-D Sheet Metal Forming Processes, Verification of Simulation with Experiment,” NUMISHEET 1993 2nd International Conference.

×