Tutorial Week 7 Optimisation

Transcription

1 Introduction Tutorial Week 7 Optimisation This tutorial will introduce the optimisation study technique using the Response Surface Method in Workbench. You will learn to: Import a SolidWorks geometry into Workbench with a named variable Perform a parametric study to create a response surface Find the values required to produce an optimum result Criteria Objective 1: Minimise the maximum von Mises stress on the outer surface of the implant stem. Objective 2: Minimise the strain energy density of the implant. Design Variable 1 and Constraint: Vary the length of the implant stem (between 250 and 300 mm). Design Variable 2 and Constraint: Vary the radius of the implant neck (between 5 and 10 mm). Step 1: Create Geometry in Solidworks Open SolidWorks and create the geometry as shown below. You need to make the bone and the implant as separate parts. For the implant, we need to define the parameters while defining the dimensions so that Workbench can identify them as being parameters. When you are creating the stem section, set the length to be L=300 mm, but also give the dimension a name. The correct format for

2 this name is that it needs some identifier, followed by an underscore, followed by the parameter name. For example, we can call this variable ANSYS_Length (see figure). will automatically be added to the end of the name when you create it. Do the same thing for the neck. Make sure the identifier is the same as the one you defined for the length. For example, we can call this ANSYS_Neck.

3 After completing the two SolidWorks parts, save them, then create an assembly. Your geometry should look like this. Save the assembly file. Step 2: Import into Workbench Open Workbench and create a new Static Structural module. Enter your material properties for bone and implant into the Engineering Data. Open the Design Modeler by double clicking on Geometry. Import an external geometry, and select the SolidWorks assembly file you created. Scroll down in the Details View (bottom left), and change the Parameter Key from DS to ANSYS. What we are doing here is defining that identifier we used in SolidWorks to make a dimension a parameter. By default, the identifier is DS, so we could have called our parameters DS_Length and DS_Neck. What you choose for your identifier is up to you for future studies. Click Generate. Once finished, scroll down to the bottom of the Details View. You should see the parameters we defined in SolidWorks. We need to tell Workbench that we wish to use them in this Static Structural analysis. Click on the little boxes to the left of these parameters to show a blue P. Of course, if we decide not to have one of these in our parametric study, we can easily just not click this box. That variable will still have a name, but will not be changed in the study. Close the Design Modeler window.

4 Step 3: Finish Setting Up Static Structural Continue working through the Static Structural components the same way as you have done previously. Remember to assign the materials, check the contacts, create a mesh, define the boundary conditions, and choose the results you want to retrieve. Important! At this point, you should conduct the mesh convergence study to find an ideal mesh. It is a good idea to keep track of how long each mesh takes to solve so that you can determine which mesh is good to use for the optimisation study. After doing this, continue with the tutorial. As part of our optimisation study, we wish to minimise the maximum von Mises stress, and minimise the strain energy density. Insert a von Mises stress and select the outer surface of the stem as the geometry selection. Under the Details pane, scroll down until you see the Maximum value for the results. Click on the box here to set this as an output parameter. Remember, we want to minimise this maximum value. Repeat this process for the strain energy density. Close the Static Structural window. Step 4: Optimisation Study Back in the Project Schematic, add a Response Surface Optimisation under the Parameter Set.

5 Double click on Design of Experiments to open it in a new tab. Here you will see the two input parameters (ANSYS_Length and ANSYS_Neck) and the two output parameters (Equivalent Stress Maximum and Strain Energy Maximum). Click on P1 (the length of the stem). Here, you can define the design space for this variable. Set the Lower Bound to 250, and the Upper Bound to 300. These values are chosen based on the question. In the same way, define the design space for the neck (P2). Click on Design of Experiments (the top one with the lightning bolt). Change the Design of Experiments Type to Custom + Sampling. Set the total number of samples to 12. Double click on Design Points vs Parameter on the left to add this chart. Set P1 as the x-axis (bottom) and P2 as the y-axis (bottom). Then click Preview. Doing this will generate 12 points of various combinations of P1 and P2 that Workbench will test. You can change the number of points if you wish and preview the combinations. You can also change the Design of Experiments Type to get different arrangements. Once you are happy with the number and distribution of design points for the response surface, click on Update. Beware that this will start the solving process for each and every one of the design points, and so this may take a long time. During this time, any new solutions will be added automatically to the table. After all the results have been determined, close the Design of Experiments tab. Double click on Response Surface. Here you can define the Response Surface Type, which is the way the response surface is calculated. For this tutorial, we will leave it as Full 2 nd Order Polynomial. Click on Update. Some new components have been added to the Outline. Click on Response and then change the Mode from 2D to 3D. Select P1 as the x-axis, P2 as the y-axis, and P3 as the z-axis. You should see the resulting response surface for the von Mises stress. Set P4 for the z- axis to see the response surface for the strain energy density. At this point, you can change the Response Surface Type and view different response surfaces.

6 Return to the Project Schematic window. Open the Optimisation tab. Click on Optimisation. Change the Method Name to MOGA (Multiobjective Genetic Algorithm). Click on Objectives and Constraints. On the right, select P3 (stress) as the parameter, and set it to minimum. Repeat this for P4 (strain energy). Then click Update.

7 You do not need to define limits for the constraints of P1 and P2 here because they have already been restricted in the previous step. Click on Tradeoff. Change the x- axis to P3 and the y-axis to P4. Here you should see the pareto front showing the optimal combinations of stress and strain energy.