Workshop 3Shape Optimization of a Plate with a Hole© Dassault Systèmes, 2012Topology and Shape Optimization in AbaqusIntroductionIn this workshop you will become familiar with the process of setting up, submitting, monitoring and postprocessing a shape optimization problem using Abaqus/CAE.A finite element model of a plate with a hole is provided (see Figure W3–1). You will import this model into Abaqus/CAE and then perform a shape optimization on it.Preliminaries1. Enter the working directory for this workshop:../atom/plate2. Start a new session of Abaqus/CAE using the following command:abaqus caewhere abaqus is the command used to run Abaqus.3. In the Start Session dialog box, underneath Create Model Database , click With Standard/Explicit Model .4. From the main menu bar, select File →Run Script .5. In the Run Script dialog box, select ws_atom_plate.py and click OK .6. A model named hole-plate-quarter will be created.Figure W3– 1 Quarter symmetry model of a plate with a hole.171Examining the finite element modelIn this finite element model we are interested in the static response of a plate with a hole tomultiple load cases. Taking advantage of symmetry, we construct only a quarter symmetrymodel. The model consists of the following:1.Parts: The model consists of a single part named PART–1.2.Mesh: The plate is meshed with CPS4 elements.3.Materials: Material properties of steel have been assigned to the plate.4.Steps: Two steps, one for each load case are specified. Nonlinear geometric effects areconsidered.5.Loads: Two loads of magnitude 200 and 100 are specified in the X- and Y-directions, inSteps 1 and 2, respectively. The loads are not propagated from one step to another; thus,they represent independent load cases.6.Boundary conditions: Symmetry boundary conditions are applied to appropriate edges.Before proceeding with the optimization analysis, examine the finite element model.To examine the finite element model:1. In the Model Tree, click to expand the model hole–plate–quarter as shown in FigureW3–2.2.Expand the following containers: Parts, Materials, Assembly, Steps, Loads and BCs.3.Right-click on each of the items in the containers and choose Edit from the menu thatappears.4.Click Cancel in order to avoid making changes to the analysis.Figure W3–2 Model Tree for quarter plate model.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 172© Dassault Systèmes, 2012 Topology and Shape Optimization in AbaqusCreating and submitting an analysis job Once you have examined the model, you will submit an analysis job to ensure that the model runs without error and produces meaningful results.To create and submit an analysis job:1. Switch to the Job module.2. From the main menu bar, select Job →Manager .3. From the buttons on the bottom of the Job Manager , click Create to create a job.4. In the Create Job dialog box that appears:a. Name the job hole –plate –quarter and select the model hole –plate –quarteras the source; click Continue .5. In the Edit Job dialog box that appears, click OK to accept all defaults.6. From the buttons on the right side of the Job Manager , click Submit to submit your job for analysis. The status field will show Running . When the job completes successfully, the Status field will change to Completed as shown in Figure W3–3.Figure W3–3 Job Manager.7. In the Job Manager , click Results to postprocess the analysis results.8. In the Visualization toolbox, plot the Mises stress distribution for each of the load cases as shown in Figure W3–4.Figure W3–4 Contour plots of Mises stress.9. Return to the Job module and dismiss the Job Manager.173Defining a shape optimizationIn shape optimization, typically the goal is to homogenize the stress on the surface of acomponent by adjusting the surface nodes. Thus, the minimization is achieved byhomogenization. Shape optimization is not limited to minimizing stresses; it may be extended to plastic strains, natural frequencies, etc.In this workshop you will homogenize the Mises stress on the periphery of a hole in a plate. You will consider two load cases simultaneously, ensuring that the plate is equally stressed in bothload cases and therefore equally likely to fail (or survive) either load case.The workflow for shape optimization is exactly the same as that for topology optimization.Creating an optimization task:1.Switch to the Optimization module (Figure W3–5).Figure W3–5 Switching to the Optimization module.2.From the main menu bar, select Task→Create.3.In the Create Optimization Task dialog box that appears: the optimization task optimize-shape.b.Select Shape optimization as the type and click Continue.c.You will be prompted to select an optimization region.d.Select the set DESIGN_NODES, as shown in Figure W3–6.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 174Figure W3–6 Selecting the optimization region.In shape optimization the design variables are the positions of the surface nodes; thus, the optimization region is always a set of nodes.Next, you will select and configure the optimization algorithm.In the Edit Optimization Task dialog box (Figure W3–7):1.In the Basic tabbed page, select Freeze boundary condition regions.2.Select Specify smoothing region, and select the whole model.3.Select Fix all as the Number of node layers adjoining the task region to remain free.4.In the Mesh Smoothing Quality tabbed page, set the Target mesh quality to Medium.5.Accept all defaults in the Advanced tabbed page.6.Click OK.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus175© Dassault Systèmes, 2012 Topology and Shape Optimization in AbaqusFigure W3–7 Optimization task editor.You have now configured the shape optimization algorithm. Next, you will define design responses.Creating design responses:1. From the main menu bar, select Design Response →Create .2. In the Create Design Response dialog box that appears:a. Name the design response Mises –Stress –step1.b. Accept Single-term as the type, and click Continue .c. You will be prompted to select the design response region type.d. In the prompt area, select Whole Model as the design response region.3. In the Edit Design Response dialog box that appears (Figure W3–8):a. In the Variable tabbed page, select Stress and Mises hypothesis .b. Note that the field Operator on values in region is set to Maximum value bydefault.c. Switch to the Steps tabbed page, select Specify and click to add a step.d. Select Step-1 from the Step and Load Case drop-down list.e. Click OKto create the design response.176© Dassault Systèmes, 2012 Topology and Shape Optimization in AbaqusFigure W3–8 Design response for the strain energy.4. Similarly, define a design response for Step –2.a. Name the design response Mises –Stress –step2.5. Similarly, define a design response for the volume (see Figure W3–9).a. Name the design response Volume .Figure W3–9 Design response for the volume.177© Dassault Systèmes, 2012 Topology and Shape Optimization in AbaqusNext, you will create an objective function. Creating an objective function:1. From the main menu bar, select Objective Function→Create .2. In the Create Objective Function dialog box that appears:a. Name the objective function optimize-shape and click Continue .3. In the Edit Objective Function dialog box that appears (Figure W3–10):a. Click to add all design responses eligible to participate in an objectivefunction.b. Leave the Reference Target field at the Default setting.c. Change the Target to Minimize the maximum design response values .d. Click OK .Figure W3–10 Objective function optimize-shape .Next, you will create a volume constraint.The purpose of creating volume constraints in a shape optimization is to ensure that the overall volume of the component remains the same. In most cases it is undesirable to simply addmaterial to reduce stress. Rather, material is redistributed to minimize stress. Volume constraints ensure that either no material is added or very little material is added as a result of the shape optimization.Creating a constraint:1. From the main menu bar, select Constraint →Creat e .2. In the Create Constraint dialog box that appears:a. Name the constraint volume-constraint and click Continue .3. In the Edit Optimization Constraint dialog that appears (Figure W3–11):a. Click the drop-down menu for the Design Response , and select Volume .b. Toggle on A fraction of the initial value and enter 1.c. Click OKto create the optimization constraint for volume.178Figure W3–11 Optimization constraint on volume.The setup of the optimization task is now complete. Next, you will create and submit an optimization process.Creating an optimization process:1.Switch to the Job module.2.From the main menu bar, select Optimization→Create.3.In the Edit Optimization Process dialog box that appears (Figure W3–12): the optimization process optimize-shape.b.In the Description field of the dialog box, enter shape optimization.c.Note the Maximum cycles field is set to 10 by default for shape optimization.d.Click OK.Figure W3–12 Edit optimization process.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus179Submitting an optimization process:1.From the main menu bar, select Optimization→Manager.2.From the buttons on the right side of the Optimization Process Manager, click Validateto validate the optimization process.a.When the validation process completes successfully, the Status field will changeto Check Completed.3.Click Submit in the Optimization Process Manager.4.Once the Status changes to Running,click Monitor if you wish to monitor the progressof the optimization process.Postprocessing shape optimization resultsYou may postprocess the solution when the optimization process is complete.Opening the Abaqus output database file:1.Click Results in the Optimization Process Manager.Note that the Abaqus output database file is stored in the folder named ATOM_POST. Allsolution folders generated by ATOM have the structure shown in Figure W3–13.The .odb file stored in the folder ATOM_POST contains the optimization results. Note thatthe history data available for optimization are also available inoptimization_report.csv. You may access this file after the optimization is completebut not during it. Abaqus will stop writing to the file if it is opened during the run. Thefolders SAVE.dat, SAVE.inp, etc. are archives of the Abaqus runs that were performed bythe optimizer. The file atom.out contains the output log from the optimizer.Figure W3–13 File structure from an optimization run.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 180Contour plotting the shape change:1.From the main menu bar, select Result→Step/Frame.a.From the Step/Frame dialog box, select the ATOM OPTIMIZATION step.b.Select Frame10 (or the highest iteration available to you) from the list ofavailable frames.c.Click OK to close the Step/Frame dialog box.d.In the Visualization toolbox, click and set the Deformation Scale Factor to1.e.In the Field Output toolbar:i. Set the Primary variable to DISP_OPT _VAL.ii.Set the Deformed variable to DISP_OPT.f.In the Visualization toolbox, click and hold .g.Select the last icon to plot contours on both the deformed and undeformedshapes.The contour plot of the deformed shape overlaid on the undeformed shape after 10iterations appears as shown in Figure W3–14. The figure shows the displacementsapplied by the optimizer (shape change) as a scalar. Growth is visualized in red whileshrinkage is visualized in blue. This plot provides an understanding of where themodel is shrinking and where it is growing. Recall that the volume was constrained toremain constant; thus, the growth and shrinkage balance each other. The plot alsoshows that the mesh in the interior moves as a result of the smoothing that wasapplied.Figure W3–14 Contour plot of DISP_OPT_VAL at 10 cycles.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus181Figure W3–15 shows the results after 150 iterations. As seen in the two figures, the difference in the peak values of DISP_OPT_VAL between the two jobs is not large. This implies that theshape optimization only made minor corrections to the shape between iterations 10 and 150.Figure W3–15 Contour plot of DISP_OPT_VAL at 150 cycles.While creating the objective function we had chosen to minimize the maximum design response values. The formulation finds the maximum objective function term and seeks to minimize itduring each design iteration. Given that the optimizer employs a large number of iterations, it is expected that the objective function terms will be more or less equal in magnitude at end of theoptimization. In this example, the stress due to the load in steps 1 and 2 is more or less equalafter the shape optimization. Thus, the plate is not more likely to fail in one load case versus the other.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 182Plot the Mises stress and compare the peak stress from each of the load cases.Plotting the Mises stress:1.From the main menu bar, select Result→Step/Frame.a.From the Step/Frame dialog box, select step Step-1_Optimization.b.Select Frame10 from the list of available frames.c.Click OK to close the Step/Frame dialog box.d.In the Visualization toolbox, click and set the Deformation Scale Factor to300.e.In the Field Output toolbar:i. Set the Primary variable to S (Int Pt) and select Mises as the component.ii.Set the Deformed variable to U.f.In the Visualization toolbox, click to plot contours on both the deformed andundeformed shapes.g.Repeat steps a-f for Step-2_Optimization.The results are shown in Figure W3–16 (a and b). Note the significant differencebetween the peak values of Mises stress after 10 iterations. This is a strong indicationthat the MIN_MAX formulation needs more iterations to achieve its goal.Figure W3–16 (c and d) shows the results from a solution that was allowed to run for150 iterations. The difference in the peak stresses is now significantly reduced.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus183a.Mises stress Step-1 at 10 cycles.b. Mises stress Step-2 at 10 cycles.c.Mises stress Step-1 at 150 cycles.d. Mises stress Step-2 at 150 cycles.Figure W3–16 Contour plots of Mises stress.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 184Plot the history output for variables OBJ_FUNCTION_DRESP: MISES-STRESS-STEP1 andOBJ_FUNCTION_DRESP:MISES-STRESS-STEP2. Compare the magnitudes, as shown inFigure W3–17.To plot history output:1.From the main menu bar, select Result→History Output.2.From the History Output dialog box that appears, select the ATOM OptimizationHistory variables.3.Click Plot to plot the selected variables.4.Click Dismiss to dismiss the dialog box.The red arrow in Figure W3–17 indicates the results obtained in 10 iterations. Clearly 10iterations were not sufficient for the optimization process to converge.Figure W3–17 History plots.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus185Finally, it is important to clarify that the MIN_MAX formulation may result in the increase insome objective function terms as it operates on others, even though a minimization wasspecified. In Figure W3–17 we see that during the first 60 iterations the peak Mises stress forStep-1 reduces while the peak Mises stress for Step-2 increases. The increase in peak Misesstress for Step-2 is nothing more than an unavoidable side effect of the shape change that wasdriven by Step-1 (the Mises stress in Step-1 was greater during the first 60 iterations). Atapproximately the 60th iteration, Step-2 begins to dominate the shape change and the Mises stress for Step-2 begins to reduce. Fortunately, the subsequent shape changes do not adversely affectthe Mises stress in Step-1.Note: A script that creates the model described in these instructions is availablefor your convenience. Run this script if you encounter difficulties following theinstructions outlined here or if you wish to check your work. The script is named ws_atom_plate_answer.pyand is available using the Abaqus fetch utility.© Dassault Systèmes, 2012 Topology and Shape Optimization in Abaqus 186。
