Abaqus/CAE (ver. 6.11) Nonlinear Buckling Tutorial

Transcription

1 Abaqus/CAE (ver. 6.11) Nonlinear Buckling Tutorial Problem Description This is the NAFEMS 1 proposed benchmark (Lee s frame buckling) problem. The applied load is based on the normalized (EI/L 2 ) value of F = N. The analysis will investigate post-buckling nonlinear behavior of the frame at the applied load location. This tutorial will also describe x-y plotting capability in Abaqus/CAE, including combining variables to generate load-displacement plots. E = N/m 2 ν = 0.0 L = 1.2 m 0.2 L 0.8 L F L National Agency for Finite Element Methods and Standards, NAFEMS Non-Linear Benchmarks (Glasgow: NAFEMS, Oct., 1989, Rev. 1.) Test No. NL Hormoz Zareh & Jenna Bell 1 Portland State University, Mechanical Engineering

2 Analysis Steps 1. Start Abaqus and choose to create a new model database 2. In the model tree double click on the Parts node (or right click on parts and select Create) 3. In the Create Part dialog box (shown above) name the part and a. Select 2D Planar b. Select Deformable c. Select Wire d. Set approximate size = 10 e. Click Continue 4. Create the geometry shown below (not discussed here) 2011 Hormoz Zareh & Jenna Bell 2 Portland State University, Mechanical Engineering

3 5. Double click on the Materials node in the model tree a. Name the new material and give it a description b. Click on the Mechanical tab Elasticity Elastic i. Enter a Young s modulus of , and Poisson s ratio of 0 c. Click OK 6. Double click on the Profiles node in the model tree a. Name the profile and select Rectangular b. Click Continue c. Enter 0.03 for a and 0.02 for b d. Click OK 2011 Hormoz Zareh & Jenna Bell 3 Portland State University, Mechanical Engineering

4 7. Double click on the Sections node in the model tree a. Name the section beam and select Beam for the category and Beam for the type b. Click Continue c. Select the profile created above (rect_beam) and the material created above (Material-1) d. Click OK 8. Expand the Parts node in the model tree, expand the node of the part just created, and double click on Section Assignments a. Select the entire geometry in the viewport and press Done in the prompt area b. Select the section created above (beam) c. Click OK 9. In the toolbox area click on the Assign Beam Orientation button a. Select all the geometry b. Click Done 2011 Hormoz Zareh & Jenna Bell 4 Portland State University, Mechanical Engineering

5 c. d. e. f. Leave the default values of 0.0,0.0,-1.0 Press the Enter key The beam normals should be oriented as shown below. Click OK to confirm 10. Create a set for the upper-center vertex a. Expand the Assembly node in the model tree, and then double click on sets b. Name the set and select geometry for the type, Click Continue c. Select the vertex where the load is applied, Click Done 2011 Hormoz Zareh & Jenna Bell 5 Portland State University, Mechanical Engineering

6 11. Expand a. b. the Assembly node in the model treee and then double click on Instances Select Dependent for the instance type Click OK 12. Double a. b. click on the Steps node in the model tree Name the step, set the procedure to General, andd select Static, Riks, Click Continue On the Basic tab i. Give the step a description and ii. Set geometric nonlinearities on (Nlgeom = ON) iii. Under Stopping criteria check Maximumm load proportionality factor and set to Hormoz Zareh & Jenna Bell 6 Portland State University, Mechanical Engineering

7 c. On the Incrementation tab, i. Set the initial arc length increment size to 0.1 ii. Set the maximum arc length increment size to 2 iii. Set the maximum number of increments to 200 d. Click OK 13. Double click on the BCs node in the model tree d. Name the boundary conditioned Pinned and select Displacement/Rotation for the type e. Click Continue f. Select the two free ends of the frame and click Done i. Note: to select multiple items, hold the shift key g. Select U1 and U2 and set to zero, click OK 2011 Hormoz Zareh & Jenna Bell 7 Portland State University, Mechanical Engineering

8 14. Double click on the Loads node in the model tree a. Name the load and select Concentrated force as the type b. Click Continue c. Select the point along the top beam near the corner, Click Done d. Set CF1 to 0 and CF2 to e. Click OK 2011 Hormoz Zareh & Jenna Bell 8 Portland State University, Mechanical Engineering

9 15. In the model tree double click on Mesh for the frame part, and in the toolbox area click on the Assign Element Type icon a. Select the entire geometry b. Select Standard for element type c. Select Linear for geometric order d. Select Beam for family e. Note that the name of the element (B21) and its description are given below the element controls f. Click OK 2011 Hormoz Zareh & Jenna Bell 9 Portland State University, Mechanical Engineering

10 16. In the toolbox area click on the Seed Part icon h. Enter 0.08 for Approximate global size, click OK 17. In the toolbox area click on the Mesh Part icon, Click Yes 18. Expand the History Output Requests node in the model tree, and then right click on H-Output-1 (H-Output-1 was automatically generated when creating the step) and select Delete 19. Double click on the History Output Requests node i. Name the history and select Continue j. Set the domain to Sets and select the set created above k. Leave the frequency set to every increment (n=1) l. For the output variables select the U2 displacement 2011 Hormoz Zareh & Jenna Bell 10 Portland State University, Mechanical Engineering

11 20. In the model tree double click on the Job node a. Name the job frame_buckle b. Give the job a description 2011 Hormoz Zareh & Jenna Bell 11 Portland State University, Mechanical Engineering

12 21. In the model tree right click on the job just created and select Submit m. While Abaqus is solving the problem right click on the job submitted, and select Monitor n. In the Monitor window check that there are no errors or warnings i. If there are errors, investigate the cause(s) before resolving ii. If there are warnings, determine if the warnings are relevant, some warnings can be safely ignored iii. In the far right column, note how Abaqus adjusted the increment 2011 Hormoz Zareh & Jenna Bell 12 Portland State University, Mechanical Engineering

13 22. In the model tree right click on the submitted and successfully completed job, and select Results 23. Display the deformed contour of the (Von) Mises stress a. In the toolbox area click on the following icons i. Plot Contours on Deformed Shape b. Note that when including the effects of geometric nonlinearities, the deformation scale factor defaults to a value of Click on the arrows on the context bar to change the time step being displayed a. Click on the three squares to bring up the frame selector slider bar 2011 Hormoz Zareh & Jenna Bell 13 Portland State University, Mechanical Engineering

14 25. On the results tree, expand the History Output node and double click on the displacement history created a. Notice that displacement it plotted against Arc Length, not Load or Load Proportionality Factor. b. To plot load against displacement, we will need to extract the values for Load and displacement from the Field Outputs. 26. In the Toolbox area click on the Create XY Data icon a. Choose ODB field output for Source and click Continue b. On the Variables tab i. Select Unique Nodal for Position ii. Expand CF: Point loads and select CF2 iii. Expand U: Spatial displacement and select U Hormoz Zareh & Jenna Bell 14 Portland State University, Mechanical Engineering

15 c. Select the Elements/Nodes tab iv. Select Node Sets for Method v. Select the set created earlier Top 2011 Hormoz Zareh & Jenna Bell 15 Portland State University, Mechanical Engineering

16 d. Click Save, then OK on the next window e. Click Dismiss on the XY Data from ODB Field Output window 27. Expand the XY Data node on the results tree. a. There should now be two sets of data under the node as shown. b. Double click the XY Data node c. For Source select Operate on XY data d. From the Operators list select combine(x,x), It should appear in the expression box at the top of the window. vi. The combine(x,x) operator combines two sets of saved XY data vii. The Y values of the first argument become the X values of the new XY data viii. The Y values of the second argument become the Y values of the new XY data ix. The values are combined wherever the X values of the two arguments align x. For more detail see Abaqus/CAE User s Manual section , Combining two X-Y data objects 2011 Hormoz Zareh & Jenna Bell 16 Portland State University, Mechanical Engineering

17 e. Select U:U2 P1: PART. From the XY Data section and click Add to Expression f. Select CF:CF2 PI: PART. From the XY Data section and click Add to Expression g. Since the load and displacement both increase in the negative direction, they need to be multiplied by -1 to make load and displacement increase in the positive direction. h. The final expression should look like: i. Click Save As, name it load-displacement, click OK j. Close the Operate on XY Data window 28. Right click on load-displacement under the XY Data node and select Plot k. The buckling behavior can be seen in the plot Hormoz Zareh & Jenna Bell 17 Portland State University, Mechanical Engineering

18 29. This data can also be copied into Excel or other programs. l. Right click on load-displacement under the XY Data node and select Edit m. Select all the data in the edit window, right click and choose Copy n. Open Excel, right click in an empty cell and choose Paste 2011 Hormoz Zareh & Jenna Bell 18 Portland State University, Mechanical Engineering