PATRAN+NASTRAN进行的拓扑优化教材

WORKSHOP PROBLEM 6 Topology and Shape Optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-1 Objectives n Create the FE-model n Carry out the topology optimization n Generate a new FE-model based on the topology results n Carry out the shape optimzation 6-2 MSC/CONSTRUCT Exercise Workbook Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-3 Model Description: The goal of this exercise is to find a light weight structure for given constraints and a single force. Here both optimization options of MSC/CONSTRUCT should be applied subsequently. First of all the topology of the plate should be optimized similar to workshop example 2. This leads to a faceted shape which has to be smoothed for the subsequent shape optimization. Figure 6.1 below shows the geometry and boundary conditions of the two-dimensional plate. Figure 6.1 Geometry and boundary conditions of the plate Young’s Modulus: 2.1 *105 N/mm2 Poisson Ration: 0.3 Length: 480mm Width: 320mm Thickness: 20mm Loading: 600N 480 32 0 x y F 6-4 MSC/CONSTRUCT Exercise Workbook Suggested Exercise Steps: 1. n Generate the MSC/NASTRAN input file 2. n Create a parameter file and carry out the topology optimization 3. n Generate a new FE-model for the shape optimization n Create the Geometry n Create the FE-Model n Set the properties of the plate n Define the Material n Define the Element Properties n Assign the load and boundary conditions n Define the Design Nodes n Generate the Input File 4. n Create the parameter file and carry out the shape optimization 5. n Postprocessing Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-5 Exercise Procedure: 1. Generate a MSC/NASTRAN input deck for the topolo- gy optimization For this exercise use the MSC/NASTRAN input deck from workshop example No. 2; topo_var.bdf. This input file should contain the necassary commands for the optimization. In this input file modify the force definition in the following way and save the file plate_topo.bdf. FORCE 1 200 0 200. 0. 1. 0. FORCE 1 225 0 200. 0. 1. 0. FORCE 1 250 0 200. 0. 1. 0. 2. Carry out the topology optimization For the optimization use the parameter file simple.par from the same workshop example. Modify the relative volume in the objective function to 0,5. Adjust the name of the input file to plate_topo.bdf and carry out the optimization. 3. Generate a new FE-model based on the results of the topology optimzation Based on the final material distribution of the topology optimization a smoothed geometry has to be generated first. This geometry has to be meshed. Then the boundary conditions can be applied. 6-6 MSC/CONSTRUCT Exercise Workbook 3.1 Plot the optimized material distribution Additional you need the Trans_Gr_17.: Figure 6.2 Material distribution 3.2 Create a new geometry In order to simplify the generation of the new geometry two little holes in the model will be ignored. Groups/Post Selected Groups to Post: Hard_Gr_0017 Apply Selected Groups to Post: Trans_Gr_0017 Apply Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-7 From the faceted geometry of the Figure 6.2 one has to generate curves and surfaces which subsequently can be meshed. Within MSC/PATRAN there are basically 2 ways for the mesh generation. u defining a polygon line and use the paver u defining surfaces explicitly and use the isomesher The first method is much simpler compared to the second one but might lead to a poor element quality. As the element quality is crucial for the results of the optimization the second method is chosen here. 3.2.1 At fist display the nodes and elements In the windows "LIST A" in lista’ contents databox the element number are listed. Tools/List/Create Model: FEM Object: Node Method: Association Association: Element Element: select all elements Apply Add to Group Group Name: Hard_Group_17 Apply Cancel 6-8 MSC/CONSTRUCT Exercise Workbook In the Dislplay / Finite Elements you can change the node size. Figure 6.3 Basis model with the finite elements and associated nodes 3.2.2 Create the geometry (curves and surfaces) u Geometry Action: Create Object: Curve Method: Point Option: 2 Point Starting Point List: Node 1 Ending Point List: Node 7 Apply Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-9 Repeat this option with the following numbers. Starting Point List Ending Point List 7 15 15 95 95 122 122 175 175 225 225 275 401 407 407 415 415 345 345 322 322 275 322 223 223 122 51 210 351 210 Change the method to Fillet and create form curve 15 and 16 a circular curve with the Fillet radius =40. Generate arcs. Change the Method to 2DArc3Point. Starting Point List Middle Point List Ending Point List 269 321 169 269 268 291 291 290 213 169 168 141 213 140 141 Action: Create Object: Curve Method: Fillet Fillet Radius: 40 Starting Point List: select Curve 15 and node 210 (with mouse) Ending Point List: select Curve 16 and node 210 (with mouse) Apply 6-10 MSC/CONSTRUCT Exercise Workbook Delete all existing nodes and elements. Posted for this all elements and nodes and delete these in Finite Elements - Delete. You can’t use this for the new geometry. Figure 6.4 Curves Modify these curves in order to get surfaces which finally -after meshing- lead to finite elements of good quality. u Geometry Action: Edit Object: Curve Method: Break Option: Parametric Breaking point: 0.5 Curve List: Curve 22 20 18 27 28 16 17 15 Apply Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-11 Repeat this action at the Break point 0.67 for Curves 9 and 2 as well as at Break Point 0.4 for Curve 39 and 41. Delete the original curves. Figure 6.5 Modified curves Create surfaces on this shown curves like in Figure 6.6 u Geometry Action: Create Object: Surface Method: Curve Option: 2 Curves Starting Curve List: Curve 1 Ending Curve List:: Curve 37 Apply 6-12 MSC/CONSTRUCT Exercise Workbook Figure 6.6 Surfaces 3.2.3 Create the finite element model and mesh the surface. Repeat this with the number 3 for the Curves 7 and 6. u Finite Elements Action: Create Object: Mesh Seed Type: Uniform Number: 6 Curve List: Surface 1.1 18.3 Apply u Finite Elements Action: Create Object: Mesh Type: Surface Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-13 Equivalence and remove duplicated nodes. Figure 6.7 FE-Model 3.2.4 Define the material, the element properties and the boundary conditions according Figure 6.8. The additional boundary conditions in x should be only used for the optimization. Create for this a subcase which include the boundary conditions for the optimization. Global Edge Length: 18 Element Topology Quad4 SurfaceList Surface 1:18 Apply 6-14 MSC/CONSTRUCT Exercise Workbook Figure 6.8 Boundary conditions 3.2.5 Define the design nodes. 3.2.6 Generate an input file for the analysis. Groups/Create New Group Name:: Design_Nodes Group Contents: Add Entitty Selection Apply u Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: shape Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-15 An MSC/NASTRAN input file will be generated called shape.bdf. Exit your MSC/PATRAN session. 3.3 Create a parameter file shape.par Use the parameter file shape_simple.par from the workshop example 4, modify the Object Definition Section and save as shape.par. Create the MSC/CONSTRUCT group from the previous created MSC/PATRAN group ’Design_Nodes. Create the MSC/CONSTRUCT group in the Construct-Menu Translation Parameter... Data Output: XDB Only OK Direct Text Input u Bulk Data Section Bulk Data Section: PARAM, DBALL, SCRATCH OK Subcase Create Output Request Form Type: Basic Select Result Type: Grid Point Stresses Create OK Apply Apply Groups Type: NODES Patran Groups: Design_Nodes Create 6-16 MSC/CONSTRUCT Exercise Workbook Figure 6.9 Parameter file shape.par ! INPUT FILE FOR TOPOLOGY OPTIMIZATION ! MODEL :frozen ! AUTHOR :training ! DATE :09-Dec-97 14:49:18 ! LAST CHANGE : ! REMARKS : ! DESCRIPTION : ! - - - - -DATA INPUT SECTION! ! READ, topo_var.bdf ! - - - - OBJECT DEFINITION SECTION SELECT, NODE, S, NODE , 1 , 8 , 1 SELECT, NODE, A, NODE , 15 , 43 , 7 SELECT, NODE, A, NODE , 44 , 49 , 1 SELECT, NODE, A, NODE , 51 , 54 , 1 SELECT, NODE, A, NODE , 81 , 84 , 1 SELECT, NODE, A, NODE , 86 , 88 , 1 SELECT, NODE, A, NODE , 113 , 116 , 1 SELECT, NODE, A, NODE , 166 , 172 , 1 SELECT, NODE, A, NODE , 174 , 176 , 1 SELECT, NODE, A, NODE , 198 , 206 , 1 SELECT, NODE, A, NODE , 243 , 248 , 1 SELECT, NODE, A, NODE , 250 SELECT, NODE, A, NODE , 251 SELECT, NODE, A, NODE , 268 SELECT, NODE, A, NODE , 269 SELECT, NODE, A, NODE , 271 , 273 , 1 SELECT, NODE, A, NODE , 299 , 301 , 1 SELECT, NODE, A, NODE , 323 SELECT, NODE, A, NODE , 327 SELECT, NODE, A, NODE , 328 SELECT, NODE, A, NODE , 345 SELECT, NODE, A, NODE , 346 SELECT, NODE, A, NODE , 349 , 354 , 1 SELECT, NODE, A, NODE , 391 , 396 , 1 SELECT, NODE, A, NODE , 398 , 400 , 1 SELECT, NODE, A, NODE , 422 , 424 , 1 SELECT, NODE, A, NODE , 426 SELECT, NODE, A, NODE , 427 SELECT, NODE, A, NODE , 453 , 455 , 1 SELECT, NODE, A, NODE , 506 , 512 , 1 SELECT, NODE, A, NODE , 514 , 517 , 1 SELECT, NODE, A, NODE , 544 , 547 , 1 SELECT, NODE, A, NODE , 549 , 554 , 1 SELECT, NODE, A, NODE , 561 , 589 , 7 SELECT, NODE, A, NODE , 591 , 596 , 1 SELECT, NODE, A, NODE , 601 , 613 , 4 SELECT, NODE, A, NODE , 614 , 616 , 1 SELECT, NODE, A, NODE , 624 , 632 , 4 SELECT, NODE, A, NODE , 634 , 636 , 1 GROUP, NODE, DESIGN_NODES ! ! - - - - -OPTIMIZATION SECTION ! --------------------------------------------------------------------------- LOAD_CALC, LOAD_CALC_1, HYPO, MISES OBJ_FUNC, USER_OBJ_FUNC_1, STRESS, 0.10, FIX OPTIMIZE, SHAPE, DESIGN_NODES , USER_OBJ_FUNC_1, LOAD_CALC_1 STOP, ITER_MAX, 9 ! - - - - -OUTPUT SECTION ! --------------------------------------------------------------------------- INCLUDE, uf_shape_pat.mac SAVE EXIT Carry out the optimization and compare the results with Figure 6.10 Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-17 Figure 6.10 Stresses after the 10th iteration For a comparison with the paver mesh, the FE-mesh and the stresses after the 10th iteration will be shown in the following figures. In order to mesh with the paver create a chain curve of the outer and the inner curves like shown in figure 6.4. On this this two curves you can create a trimmed surface (these are options in the menu Geometry) and then mesh the surface with the paver. 6-18 MSC/CONSTRUCT Exercise Workbook Figure 6.11 FE-model meshed with the paver Figure 6.12 Stresses after the 10th iteration Workshop 6 Topology and Shape optimization of a Plate MSC/CONSTRUCT Exercise Workbook 6-19 6-20 MSC/CONSTRUCT Exercise Workbook