ME 475 Optimization of a Truss

Tags

ME 475 Optimization of a Truss

ME 475 - Optimization of a Frame

Analysis Problem Statement:

The following problem will be analyzed using Abaqus.

Figure 1. Full frame geometry and loading (gravity load not shown). All units are in meters.

Not shown is a gravity load. The structural members are made of a material with the following properties: E = 200 GPa, G = 166.7 GPa, ρ = 7,860 kg/m3). The members are labeled as to what area cross-sectional properties will be assigned to them, listed below.
Section-1: Shape = Pipe, radius = 0.1 m, thickness = 0.00635 m

Output points: (0, 0.00635); (0, -0.00635)

Section-2: Shape = Pipe, radius = 0.162 m, thickness = 0.0127 m

Output points: (0, 0.162); (0, -0.162)

Section-3: Shape = Pipe, radius = 0.1 m, thickness = 0.004 m

Output points: (0, 0.1); (0, -0.1)

Section-4: Shape = Pipe, radius = 0.16 m, thickness = 0.008 m

Output points: (0, 0.16); (0, -0.16)

Section-5: Shape = Pipe, radius = 0.08 m, thickness = 0.004 m

Output points: (0, 0.08); (0, -0.08)

Section-6: Shape = Pipe, radius = 0.1 m, thickness = 0.00635 m

Output points: (0, 0.1); (0, -0.1)

Section-7: Shape = I, l = 0.178 m, h = 0.356 m, b1 = b2 = 0.369 m, t1 = t2 = 0.018 m, t3 = 0.011 m

Output points: (0, 0.178); (0, -0.178)

Analysis Procedure:

  1. Create a folder called “BeamFEA” in C:\Temp. This will be the working directory for this lab.
  2. Open Abaqus/CAE and create a new project.
  3. File  Set Work Directory. Change this to C:\Temp\BeamFEA.
  4. In the Part Module, draw the geometry as shown in Figure 1 using the sketcher for a 2D, Deformable, Wire Part. Be sure the geometry is fully constrained (all lines will turn green as they become fully constrained).
  5. In the Property Module, create seven different Profiles, named “Profile-1”, “Profile-2”, etc., corresponding to those listed in the analysis problem statement.
  6. In the Property Module, create seven different sections, named “Section-1”, “Section-2”, etc.
  7. Use beam sections with section integration occurring before the analysis.
  8. Choose the corresponding profile for the section (for example, Profile-3 goes with Section-3).
  9. Enter the Young’s Modulus, Shear Modulus, and Section Material Density.
  10. Enter the output points as noted in the analysis problem statement. These are locations on the cross-section where stress will be calculated.
  11. In the Property Module, assign each section to the corresponding member, based on the numbering shown in Figure 1.
  12. Finally, assign the beam orientation for all of the members, use an n1 direction vector of (0,0,-1).
  13. This affects the orientation of the profile on the beam elements. In this problem, only the section with an I-beam profile would be affected by different a different beam orientation because pipe sections are rotationally symmetric.
  14. To verify that the profiles and beam orientations were input properly, turn on beam profile rendering.
  15. View menu  Part Display Options, check the box next to “Render beam profiles” toward the bottom of the General tab.
  16. In the Assembly Module, instance the part as an independent part instance.
  17. In the Step Module, create a Static Linear Perturbation step after the Initial step.
  18. In the Load Module, apply the loading shown in Figure 1, as well as the gravity load (applied to the entire structure, -9.81 in the 2-direction).
  19. Apply boundary conditions as shown in Figure 1.
  20. In the Mesh Module, use a mesh seed of 0.25 on the assembly.
  21. In the Mesh Module, assign the entire frame the element B23, a 2D beam element that uses the cubic formulation.
  22. Mesh the assembly.
  23. In the Job Module, create a job named: Kframe.
  24. Save the CAE database.
  25. Submit the job.

Results:

  1. Visualize the results in Abaqus/Viewer.
  2. Maximum U2 displacement magnitude in the frame: ______
  3. Maximum S11 stress in the frame: ______
  4. Minimum S11 stress in the frame: ______
  1. In the working directory are several files. Open KFrame.dat in a text editor, such as Notepad or Notepad++. Find the total mass of the frame and report it.
  2. Total mass of the frame: ______
  3. Print a contour plot of the S11 component of stress (use the automatically computed scale factor). Show both the deformed and undeformed geometry on the plot. Turn it in with this worksheet.
  1. Print a second plot, the same as the first with the 2-component of displacement contours instead of S11. Turn it in with this worksheet.
  1. Based on the results from 1 and 2, modify three section property values (such as radius or thickness) so the total volume is reduced and abs(MaxS11) < abs(MaxS11 from 1).
  2. Section number: ______, Property: ______, New value: ______
  3. Section number: ______, Property: ______, New value: ______
  4. Section number: ______, Property: ______, New value: ______
  5. New mass:______
  6. New maximum absolute value of S11 stress: ______
  1. For the new design, include a contour plot of the S11 component of stress with the deformed and undeformed geometry shown on the same plot.
  1. Remove the gravity load from the model. Change the job name to “KFrame_nograv”. Submit this new job.
  1. Use the model without the gravity load to validate the FEA. To find the displacement at a node in Abaqus/Viewer, go to Tools  Query  Node. Then choose a node from the viewport. The relevant information is output to the window at the bottom of the screen. Look for the 2-component of the displacement (unscaled).
  2. Vertical displacement at A: ______
  3. Vertical displacement at B: ______
  4. (Disp @ A) – (Disp @ B): ______
  5. Predicted displacement for theoretical bar: ______
  6. Percent difference between displacement found by FEA and that predicted for the theoretical bar: ______

Model Validation:

It is not necessary to solve the entire structure to validate the FE solution. In fact, that would make performing the FEA redundant for anything except visualization of the deformed state. To validate this structure, a comparison will be made to a vertical uniform bar under a compressive axial load. We will focus on the center region of the frame, highlighted in Figure 2. For the area of the bar, use the following value:

where Acolumn is the cross-sectional area of one of the outer columns (section 4),

Acenter is the cross-sectional area of one of the inner supports (section 5),

and θ1 and θ2 are shown on Figure 2.

The areas can be calculated from the section properties and the angles can be found through geometry or the Tools  Query  Angle command in used in the Part module.

The cos2() terms are used to rotate the stiffness of members into different coordinate systems, and will be further explained in lecture when FEA of trusses is covered.

Figure 2. Regions for comparing to validation calculations.

Use the following formula to find the predicted deflection of the bar:

where P is the total vertical load applied to the structure,

L is the height of the section of interest,

E is the modulus of elasticity of the material,

and δ is the axial deflection.

Compare this value to the y-deflection of the center part of the frame, after rerunning without the gravity load. This means taking the difference in 2-displacement at the circled nodes in Figure 2 (labeled A and B). You should find that the frame deflection found through FEA is within 10% that of the theoretical bar with a cross-sectional area of Aeffective.

1

Top View