Rib Forging Workshop Nine REFERENCE: Training Manual Viscoplasticity (5-35)

Workshop Supplement September 30, 2001 Inventory # W9-2 Workshop Nine: Rib Forging Anand’s Model Purpose Run a large-strain, rib forging problem which uses Anand’s Model Goal Solve a 2D analysis using viscoplastic Anand’s Model Model Description 2D VISCO106 elements with rigid-deformable contact.

Workshop Supplement September 30, 2001 Inventory # W9-3 1.Read in the input file named “ANL_W09_Rib.inp” Use the GUI menu method: –Utility Menu > File > Read Input From… Select the file “ANL_W09_Rib.inp” Click on [OK] or Command Input method: –/INPUT,ANL_W09_Rib,inp Notes: This will read in an input file which will generate the geometry, loads, and boundary conditions for the current exercise. We will have a 2D part comprised of VISCO106 elements and a rigid- deformable contact surface. The current database will be erased, and the jobname will be changed to “Exercise_9”. The graphics and other settings will also be set to be consistent with these slides. Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-4 Before continuing with the exercise, you can also examine the mesh and the boundary conditions on the model to become more familiar with it. The workpiece has boundary conditions in the normal direction along its three sides. One side represents symmetry boundary condition. An imposed displacement of 2.25 units in the -y direction is applied on the pilot node, which controls the entire rigid surface. A friction coefficient of is used for the contact pair. Anand’s model is used for the workpiece to represent viscoplastic behavior. A uniform temperature is applied. A coarse mesh is used for this exercise, so that the solution runs in a reasonable amount of time. Rigid Target Surface Pilot Node Deformable Workpiece Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-5 2.Verify the element options for VISCO106 (4-node quad) Use the GUI menu method: –Main Menu > Preprocessor > Element Type > Add/Edit/Delete … Select “Type 1 VISCO106” Click on [Options] Verify element options, then click on [OK] Select [Close] or Command Input method: –/PREP7 –ETLIST Notes: Element type 1 will use VISCO106. Recall from the discussion in Ch. 2 that VISCO106 is a penalty- based Mixed U-P element. It is used specifically for Anand’s model. Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-6 3.Add constants for Anand’s Model Use the GUI menu method: –Main Menu > Preprocessor > Material Props > Material Models … Make sure that “Material Model Number 1” is highlighted. Select “Structural > Nonlinear > Inelastic > Rate Dependent >Visco-Plasticity > Anand’s Model” Enter the constants as shown in the dialog box on the right. Click on [OK] Select “Material > Exit” or Command Input method: –TB,ANAND,1 –TBDATA,1,4307.6,37962 –TBDATA,3,2770.2,7.0 –TBDATA,5, ,1.618e5 –TBDATA,7,2744.1, –TBDATA,9,1.3 Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-7 4.Specify Solution Options for the analysis. Use the GUI menu method: –Main Menu > Solution > -Analysis Type- Sol’n Control … Select “Large Displacement Static” under “Analysis Options” Enter “15” for “Time at end of loadstep” Toggle option to “Time Increment” instead of “Number of substeps” Enter “0.1” for “Time Step Size” Enter “0.001” for “Minimum time step” Enter “0.5” for “Maximum time step” Select “Write every substep” for “Frequency” or Command Input method: –/SOLU –NLGEOM,ON –TIME,15 –DELTIM,0.1,0.001,0.5 –OUTRES,ALL,ALL Notes: If you want greater accuracy, you can also select the “Nonlinear” tab and specify maximum equivalent plastic strain increment for each substep (CUTCON command). In this case, we will use the defaults for cutback control. The maximum time step specified also helps ensure that the path- dependent nature of the problem is captured. Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-8 5.Solve the viscoplastic problem Use the GUI menu method: –Main Menu > Solution > -Solve- Current LS After reviewing the status window, close it by selecting “File > Close” To start the analysis, click on [OK] or Command Input method: –SOLVE Notes: The /STATUS window shows that plastic material properties are included. Because this is a large strain, nonlinear problem, the solution will take several minutes to run. Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-9 EQUIL ITER 6 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= E-03 LINE SEARCH PARAMETER = SCALED MAX DOF INC = E-03 FORCE CONVERGENCE VALUE = CRITERION= EQUIL ITER 7 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= E-03 LINE SEARCH PARAMETER = SCALED MAX DOF INC = E-03 FORCE CONVERGENCE VALUE = CRITERION= EQUIL ITER 8 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= E-03 LINE SEARCH PARAMETER = SCALED MAX DOF INC = E-03 FORCE CONVERGENCE VALUE = CRITERION= EQUIL ITER 9 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= E-04 LINE SEARCH PARAMETER = SCALED MAX DOF INC = E-04 FORCE CONVERGENCE VALUE = CRITERION= <<< CONVERGED >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 9 *** LOAD STEP 1 SUBSTEP 33 COMPLETED. CUM ITER = 212 *** TIME = TIME INC = *** MAX PLASTIC STRAIN STEP = CRITERION = *** AUTO TIME STEP: NEXT TIME INC = DECREASED (FACTOR = ) After the solution is completed, review the contents of the Output Window. Note that viscoplastic strains are treated similar to rate-independent plastic strains, where the plastic strain increment is used as a criterion for bisecting. In this analysis, the maximum timestep of 0.5 prevented the strain increment from becoming too large, so the plastic strain increment criterion was always satisfied. For greater accuracy, the user can decrease the maximum timestep or specify a tighter plastic strain increment limit. The default limit, as shown below, is Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W Plot equivalent plastic strain results Use the GUI menu method: –Main Menu > General Postproc > -Read Results- Last Set This reads in the last substep –Main Menu > General Postproc > Plot Results > -Contour Plot- Element Solu … Select “Strain-plastic” from the left column and “vonMises EPPLEQV” from the right. Click on [OK] to plot plastic strains or Command Input method: –/POST1 –SET,LAST –PLESOL,EPPL,EQV Notes: Because we have a coarse mesh, the results are very approximate. However, this provides a good idea of the response of the system under the movement of the rigid surface. Time permitting, postprocess other results of interest such as plastic work (NL,PLWK) Workshop Nine: Rib Forging …Anand’s Model

Workshop Supplement September 30, 2001 Inventory # W9-11 Below is an animation of von Mises stress for a finer mesh. The element size and quality has been controlled to minimize element distortion during the analysis. The results have been reflected with the /EXPAND command (Utility Menu > PlotCtrls > Style > Symmetry Expansion > Periodic/Cyclic Symmetry) Workshop Nine: Rib Forging …Anand’s Model