Workshop 7 Linear Buckling Linear Buckling Workshop 7 - Goals Workshop Supplement The goal in this workshop is to verify linear buckling results in ANSYS Workbench. Results will be compared to closed form calculations from a handbook. Next we will apply an expected load of 10,000 lbf to the model and determine its factor of safety. Finally we will verify that the structure will not fail structurally before buckling occurs. ANSYS Workbench - Simulation

March 29, 2005 Inventory #002216 WS7-2 Linear Buckling Workshop 7 - Assumptions Workshop Supplement OD = 4.5 in ID = 3.5 in. E = 30e6 psi, I = 12.7 in^4, L = 120 in. In this case we assume the pipe conforms to the following handbook formula where P is the critical load: 2EI P ' K 2 L

ANSYS Workbench - Simulation The model is a steel pipe that is assumed to be fixed at one end and free at the other with a purely compressive load applied to the free end. Dimensions and properties of the pipe are: For the case of a fixed / free beam the parameter K = 0.25. March 29, 2005 Inventory #002216 WS7-3 Linear Buckling . . . Workshop 7 - Assumptions Using the formula and data from the previous page we can predict the buckling load will be:

2 30e6 12.771 P' 0.25 65648.3lbf 2 (120) ANSYS Workbench - Simulation Workshop Supplement March 29, 2005 Inventory #002216 WS7-4 Linear Buckling Workshop 3 - Start Page From the launcher start Simulation.

Choose Geometry > From File . . . and browse to the file Pipe.x_t. When DS starts, close the Template menu by clicking the X in the corner of the window. ANSYS Workbench - Simulation Workshop Supplement March 29, 2005 Inventory #002216 WS7-5 Linear Buckling Workshop 7 - Preprocessing Workshop Supplement

Units > U.S. Customary (in, lbm, psi, F, s). 1 2. To make the material property match that of our hand calculation highlight the Solid branch in the tree: Details > Material > Edit Structural Steel . . . ANSYS Workbench - Simulation 1. Set the working unit system to the U.S. customary system: 2 March 29, 2005 Inventory #002216 WS7-6 Linear Buckling . . . Workshop 7 - Preprocessing Workshop Supplement

3 Note, changing this property on the fly does not effect the stored value for Structural Steel. To save a material for future use we would Export the properties as a new material to the material library. Since we only need the value for this workshop we will not do that in this case. ANSYS Workbench - Simulation 3. In the field for Youngs Modulus type in the value 3e7. March 29, 2005 Inventory #002216 WS7-7 Linear Buckling Workshop 7 - Environment Fix one end of the pipe: 4. Highlight the Environment branch.

5. Select the surface on one end of the pipe. 6. RMB > Insert > Fixed Support. 5 4 ANSYS Workbench - Simulation Workshop Supplement 6 March 29, 2005 Inventory #002216 WS7-8 Linear Buckling . . . Workshop 7 - Environment Add a unit force to one end of the pipe: 7. Select the surface on the free end of the

pipe. 8. RMB > Insert > Force. 7 9. In the force detail change the Define by field to Components. 10. In the force detail enter 1 in the Magnitude field. 8 9 ANSYS Workbench - Simulation Workshop Supplement 10 March 29, 2005 Inventory #002216 WS7-9

Linear Buckling Workshop 7 - Solution Insert the buckling tool into the solution branch: 11. Highlight the solution branch. 12. RMB > Insert > Buckling. Solve. ANSYS Workbench - Simulation Workshop Supplement 11 12 Notice the default setting for buckling is to find the first buckling mode. March 29, 2005 Inventory

#002216 WS7-10 Linear Buckling Workshop 7 - Results ANSYS Workbench - Simulation Workshop Supplement When the solution completes review the buckling result. 13. Highlight the 1st Buckled Mode result object. 14. The result detail indicates a Load Multiplier value of 65610. Recall that we applied a unit (1) force thus the result compares well with our closed form calculation of 65648 lbf. 14 13 March 29, 2005 Inventory #002216 WS7-11

Linear Buckling . . . Workshop 7 - Results Change the force value to the expected load (10000 lbf). 15. Highlight the Force branch. 16. In the detail field for the Z Component enter 10000. Solve 15 ANSYS Workbench - Simulation Workshop Supplement 16 March 29, 2005 Inventory #002216

WS7-12 Linear Buckling . . . Workshop 7 - Results Workshop Supplement When the solution completes note the Load Multiplier field now shows a value of 6.561. Since we now have a real world load applied, the load multiplier is interpreted as the buckling factor of safety for the applied load. Given that we have already calculated a buckling load of 65610 lbf, the result is obviously trivial (65610 / 10000). It is shown here only for completeness. ANSYS Workbench - Simulation March 29, 2005 Inventory #002216

WS7-13 Linear Buckling Workshop 7 - Verification Workshop Supplement A final step in the buckling analysis is added here as a best practices exercise. We have already predicted the expected buckling load and calculated the factor of safety for our expected load. The results so far ONLY indicate results as they relate to buckling failure. To this point we can say nothing about how our expected load will affect the stresses and deflections in the structure. As a final check we will verify that the expected load (10000 lbf) will not cause excessive stresses or deflections before it is reached.

ANSYS Workbench - Simulation March 29, 2005 Inventory #002216 WS7-14 Linear Buckling . . . Workshop 7 - Verification Highlight the Buckling branch and delete it. 17. RMB > Delete 17 18. RMB > Insert > Stress > Equivalent (von Mises) 18 ANSYS Workbench - Simulation Workshop Supplement

March 29, 2005 Inventory #002216 WS7-15 Linear Buckling . . . Workshop 7 - Verification Insert total deformation: 19. RMB > Insert > Deformation > Total 19 Solve. Note, we deleted the buckling tool because it cannot be combined with other results (stress, deformation, etc.) in the same solution branch. In actual practice, it may be desirable to duplicate the environment branch and modify the duplicate. This would allow you to keep the original buckling results as well as the structural solution.

ANSYS Workbench - Simulation Workshop Supplement March 29, 2005 Inventory #002216 WS7-16 Linear Buckling . . . Workshop 7 - Verification Workshop Supplement A quick check of the stress results shows the model as loaded is well within the mechanical limits of the material being used. As stated, this is not a required step in a buckling analysis but should be regarded as good engineering practice.

ANSYS Workbench - Simulation March 29, 2005 Inventory #002216 WS7-17