ME Optimization of a Truss

Transcription

1 ME Optimization of a Truss Analysis Problem Statement: The following problem will be analyzed using Abaqus and optimized using HEEDS m 300 kn 300 kn 22 m 35 m Figure 1 Full truss geometry and loading. All joints are pins (can rotate freely); all members have circular cross-sectional areas, and are made of steel (E = 200 GPa, ν=0.3, ρ = 7,860 kg/m 3 ). Symmetry will be enforced during the optimization, though the entire structure will be modeled. This will be performed by assigning symmetric members the same design variable. Optimization Problem Statement: minimize: subject to: by varying: total mass of truss structure maximum axial stress 150 MPa maximum vertical displacement 0.05 m cross-sectional area of the twelve members 1

2 Analysis Procedure: 1. Create a directory called Truss_Opt in C:\Temp. This directory (C:\Temp\Truss_Opt) will be the working directory for this project. 2. Open Abaqus/CAE. 3. In the Part Module, draw the geometry as shown in Figure 1 using the sketcher for a 2D, Deformable, Wire Part. 4. In the Property Module, create a material called Steel with properties: E = 200 GPa, ν=0.3, ρ = 7,860 kg/m 3. a. Density is available in the General menu in the material definition. b. The elastic modulus and Poisson s ratio is available in the Mechanical menu. 5. In the Property Module, create seven different sections, named Section-1, Section-2, etc. All seven sections should be Beam-Truss sections. a. There will be a separate section for each set of members, because the crosssectional area of each set of members is to be an independent design variable. b. Use a baseline cross-sectional area of m 2 for all sections. This corresponds to circular bars with radius m. Figure 2 Section manager after creating all section definitions. 2

3 6. In the Property Module, assign each section to the corresponding member, based on the numbering shown in Figure 2. This will impose symmetry on the optimization. a. Assign Section-1 to members 1 and 12 b. Assign Section-2 to members 2 and 11 c. Assign Section-3 to members 3 and 10 d. Assign Section-4 to member 4 e. Assign Section-5 to members 5 and 8 f. Assign Section-6 to members 6 and 9 g. Assign Section-7 to member 7 7. In the Assembly Module, instance the part as an independent part instance. 8. In the Step Module, create a Static Linear Perturbation step after the Initial step. 9. Edit the Field Output Requests to include EVOL, which is the volume of each element. 10. In the Load Module, apply the loading shown in Figure 1 (concentrated load in the 2- direction with magnitude of ). 11. In the Load Module, apply boundary conditions as shown in Figure 1. a. Left-hand side of member 1 is pinned (U1 and U2 constrained) and the right-hand side of member 12 constrained vertically only (U2 constrained). 12. In the Mesh Module, use a mesh seed of 20 on the assembly. a. This is larger than the length of any one member, so it will put nodes only at joints. 13. In the Mesh Module, assign the entire truss the element T2D2, a linear 2D truss element available in the Standard library. 14. Mesh the assembly. 15. In the Job Module, create a job named: Truss 16. Submit the job. 17. Save your CAE database view the results. 3

4 Optimization Procedure: The HEEDS Abaqus Portal will be utilized for this optimization. This is a direct interface between the Abaqus output database (which is a binary file) and HEEDS, which allows quick and simple definition of responses based on Abaqus outputs. 1. Open the HEEDS v5.3 Modeler 2. Save your HEEDS project in the same directory as your analysis files, with the name Truss_optimization 3. In the Processes tab, add the following to the analysis (see Figure 3). a. The execution file does not need to be browsed, just type: abaqus b. The command line options are: interactive job=truss c. In the input files, add Truss.inp d. In the output files, add Truss.odb Figure 3 Analysis options for truss optimization. 4. Move on to the variables tab and add seven design variables. Name them Section1, Section2, etc. These design variables will correspond to the areas of each respective section of the truss. 5. The range is the same for all variables: Min = 7.85e-5 m 2, Baseline = m 2, and Max = m 2. When finished, it should look like Figure 4. a. These values correspond to radii m, m, and 0.06 m, respectively. 4

5 Figure 4. Design variable definition. 6. Create seven responses as shown in Figure 5. Note the formula based responses, which are defined in the Formula Definition window to the right of the Project Responses window. An example where TotalVolume is being defined is shown in Figure 6. Figure 5. Project responses for the truss optimization. Figure 6. Example defining TotalVolume response based on a formula. 5

6 7. Move on to the Tagging tab. The design variables should be tagged in Truss.inp. Look for the section definition keywords(*solid Section ) and one line below is the value Tag this value for each section. There is a comment above each section definition (marked by two asterisks in front of it) that lists the section name above it (see Figure 7 and Figure 8). Be careful, because the section definitions may not be in order. Figure 7 Section definition for Section-4 before tagging. Figure 8 Section definition for Section-4 after tagging. 8. Design variable tagging is complete. Change to the volumes response. 9. Choose Truss.odb as the output file. 10. Change the tagging mode from Mark to Portal. a. A command window should appear. The Abaqus output database is being parsed so the HEEDS Abaqus Portal can display all information available in the file. 11. Define the response as shown in Figure 9. Be sure to click the TAG button when finished or the definition will not be saved. 6

7 Figure 9. Portal definition for volumes response. 12. Change to the displacements response. 13. Define the response as shown in Figure 10. Be sure to click the TAG button when finished or the definition will not be saved. Figure 10. Portal definition for displacements response. 14. Change to the stresses response. 15. Define the response as shown in Figure 11. Be sure to click the TAG button when finished or the definition will not be saved. 7

8 Figure 11. Portal definition for stresses response. 16. Now that all responses have been tagged, it is good practice to test that the portal definitions are correct. Change to the TotalVolume response. Click the Extract Value button. When finished, a value of e-001 should be displayed in the output window. If an ERROR is detected, then there is likely a problem with the portal definition of volumes or the formula used to define TotalVolume. 17. Extract the values of MaxTensileStress, MaxCompStress, and MaxDisplacement. Values of e+008, e+008, and e-002 should be displayed, respectively. 18. Move on to the Assembly tab. Process_1 is automatically assigned to the optimization agent. 19. Choose SHERPA as the optimization method with 150 evaluations. 20. Leave the resolution of the design variables at the default value, Define the responses as shown in Figure 12. The values for the maximum stresses were chosen based upon the yield stress for the material of the trusses (450 MPa) and a factor of safety of 3.0. a. The last value in the TotalVolume row is a normalizing factor. In this case, it is the baseline value of the response that was extracted in Step 16. In general, it is good to add a normalizing factor when using optimization, as it encourages robustness in the search. 8

9 Figure 12. Response definition for truss optimization. 22. The HEEDS project definition is complete. Save the Modeler project. 23. Move on to the Run tab. Click the Run button, and the optimization should begin. a. Each evaluation should take 10s - 30s to complete. Monitor the progress of the optimization periodically. If the working directory is on a network drive (such as the course space for this lab, or your personal M: drive), the evaluations may take substantially longer. 24. When the optimization is finished, Abaqus/CAE or Abaqus/Viewer to view the output for the best design. a. The files for the best design can be found in <working_directory>\heeds_0\bestdesign Note: Remember to save your entire project (Abaqus and HEEDS files) to the course space provided. The course space is backed up, but everything in C:\Temp is automatically deleted on a regular basis by DECS. 9

10 Report Requirements: A full report is required for this lab (see ME 475 Lab Report Format Guidelines). 1. Present plots of the S11 component of stress (with Quilt contours) for the baseline design and the best design found using optimization. 2. Present plots of the U2 component of displacement (with banded contours) for both the baseline design and the best design found using optimization. 3. Present a table comparing the values of the design variables and responses for the baseline and best design. Include a column for percent difference between the two. 4. Include in your discussion whether constraints are active and if particular variables are at extreme values. Validation: Solve for the stresses in the Truss by hand calculations for the baseline design. Compare these to the stress values found by FEA. 10