Chapter Seven Linear Buckling Analysis Linear Buckling Analysis

Chapter Seven Linear Buckling Analysis

Linear Buckling Analysis Chapter Overview Training Manual – In Simulation, performing a linear buckling analysis is similar to a stress analysis. – It is assumed that the user has already covered Chapter 4 Linear Static Structural Analysis prior to this section. • The capabilities described in this section are generally applicable to ANSYS Design. Space Entra licenses and above. – Some options discussed in this chapter may require more advanced licenses, but these are noted accordingly. ANSYS Workbench – Simulation • In this chapter, performing linear buckling analyses in Simulation will be covered. – Harmonic and nonlinear static structural analyses are not discussed here but in their respective chapters. March 29, 2005 Inventory #002215 7 -2

Linear Buckling Analysis A. Background on Buckling Training Manual • At the onset of instability (buckling) a structure will have a very large change in displacement { x} under essentially no change in the load (beyond a small load perturbation). F F Stable Unstable ANSYS Workbench – Simulation • Many structures require an evaluation of their structural stability. Thin columns, compression members, and vacuum tanks are all examples of structures where stability considerations are important. March 29, 2005 Inventory #002215 7 -3

Linear Buckling Analysis … Background on Buckling Training Manual • The eigenvalue formulation determines the bifurcation points of a structure. This method corresponds to the textbook approach of linear elastic buckling analysis. – The eigenvalue buckling solution of a Euler column will match the classical Euler solution. ANSYS Workbench – Simulation • Eigenvalue or linear buckling analysis predicts theoretical buckling strength (the bifurcation point) of an ideal linear elastic structure. March 29, 2005 Inventory #002215 7 -4

Linear Buckling Analysis … Background on Buckling Training Manual – Consider the buckling of a soda can: • Material response is inelastic. Geometrically nonlinear effects need to be considered. Contact is also required. Hence, these type of nonlinear behavior are not considered. • There may be slight imperfections in the soda can, such as a small dent, which would influence the response and not make the model symmetric. However, these small imperfections are also not usually considered in a linear buckling analysis. ANSYS Workbench – Simulation • However, imperfections and nonlinear behavior prevent most real world structures from achieving their theoretical elastic buckling strength. Linear buckling generally yields unconservative results, and should be used with caution. March 29, 2005 Inventory #002215 7 -5

Linear Buckling Analysis … Background on Buckling Training Manual – It is computationally cheaper than a nonlinear buckling analysis, and should be run as a first step to estimate the critical load (load at the onset of buckling). • Relative comparisons can be made of the effect of differences in design to buckling – Linear buckling can be used as a design tool to determine what the possible buckling mode shapes may be. • The way in which a structure may buckle can be used as a possible guide in design ANSYS Workbench – Simulation • Although unconservative, linear buckling has various advantages: March 29, 2005 Inventory #002215 7 -6

Linear Buckling Analysis … Basics of Linear Buckling Training Manual This results in certain assumptions related to the analysis: – [K] and [S] are constant: • Linear elastic material behavior is assumed • Small deflection theory is used, and no nonlinearities included • The response based on loading {F} is a linear function of i – Some additional restrictions: • Nonzero displacement supports or thermal loads are not allowed ANSYS Workbench – Simulation • For a linear buckling analysis, the eigenvalue problem below is solved to get the buckling load multiplier i and buckling modes yi: • It is important to remember these assumptions related to performing linear buckling analyses in Simulation. March 29, 2005 Inventory #002215 7 -7

Linear Buckling Analysis B. Buckling Analysis Procedure Training Manual – Attach Geometry – Assign Material Properties – Define Contact Regions (if applicable) – Define Mesh Controls (optional) – Include Loads and Supports – Request Buckling Results – Solve the Model – Review Results ANSYS Workbench – Simulation • The linear buckling analysis procedure is very similar to performing a linear static analysis, so not all steps will be covered in detail. The steps in yellow italics are specific to buckling analyses. March 29, 2005 Inventory #002215 7 -8

Linear Buckling Analysis … Geometry and Material Properties Training Manual – Solid bodies – Surface bodies (with appropriate thickness defined) – Line bodies (with appropriate cross-sections defined) • Only buckling modes and displacement results are available for line bodies. – Although Point Masses may be included in the model, only inertial loads affect point masses, so the applicability of this feature may be limited in buckling analyses • For material properties, Young’s Modulus and Poisson’s Ratio are required as a minimum ANSYS Workbench – Simulation • Similar to linear static analyses, any type of geometry supported by Simulation may be used in buckling analyses: March 29, 2005 Inventory #002215 7 -9

Linear Buckling Analysis … Contact Regions Training Manual • It is important to note the following: – The pinball region will influence some types of contact – All nonlinear contact types are reduced to either “Bonded” or “No Separation” contact. • No Separation contact should be used with caution in buckling analyses, as it provides no stiffness in the tangential direction. This may produce some superfluous buckling modes. Consider using bonded contact instead, if appropriate. ANSYS Workbench – Simulation • Contact regions are available in buckling analyses. However, since this is a purely linear analysis, contact behavior will differ for the nonlinear contact types: March 29, 2005 Inventory #002215 7 -10

Linear Buckling Analysis … Loads and Supports Training Manual – All structural loads will be multiplied by the load factor to determine the buckling load. Hence, non-proportional or constant loading is not directly supported (see next slide) – No Given Displacement supports are allowed – No Thermal loading is allowed – Compression-only supports are nonlinear, so they are not recommended for use in buckling analyses • The structure should also be fully constrained – No rigid-body motion should be present in the model. Be sure to constrain the model appropriately. ANSYS Workbench – Simulation • At least one structural load, which causes buckling, should be applied to the model: March 29, 2005 Inventory #002215 7 -11

Linear Buckling Analysis … Loads and Supports Training Manual – The user may iterate on the buckling solution, adjusting the variable loads until the load multiplier becomes 1. 0 or nearly 1. 0. – Consider the example of a pole with self weight WO and an externally applied force A. You can iterate, adjusting the value of A until l = 1. 0. ANSYS Workbench – Simulation • Special considerations must be given if constant and proportional loads are present. March 29, 2005 Inventory #002215 7 -12

Linear Buckling Analysis … Requesting Results Training Manual – The Buckling tool adds another branch to the Solutions branch – The Details view of the Buckling branch allows the user to specify the number of buckling modes to find. The default is to find the first buckling mode. Increasing the number of modes to calculate will increase the solution time. However, usually only a few buckling modes are usually desired. Although most users are only concerned with the first buckling mode, it is generally a good idea to request the first 2 or 3 buckling modes. There may be closely-space buckling modes, so this would tell the user if the model may be susceptible to more than one failure mode. ANSYS Workbench – Simulation • Most of the options for buckling analyses are similar to that of static analysis. However, Simulation knows to perform a buckling analysis when the Buckling tool is selected under the Solutions Branch: March 29, 2005 Inventory #002215 7 -13

Linear Buckling Analysis … Requesting Results – The buckling modes are controlled by the number of modes to find under the Details view of the Buckling branch – Stress, strain, or directional displacement results can be requested additionally under the Buckling branch • The buckling mode is specified for each stress, strain, or displacement result requested • If stresses or strains are requested for a model already solved, another solution is required. – No result may be requested directly under the “Solution” branch. ANSYS Workbench – Simulation • Requested results are located under the Buckling branch: Training Manual March 29, 2005 Inventory #002215 7 -14

Linear Buckling Analysis … Solution Options Training Manual – For a buckling analysis, none of the options in the Details view of the Solution branch usually need to be changed. • In the majority of cases, “Solver Type” should be left on the default option of “Program Controlled”. It only controls the solver used in the initial static analysis but not the buckling solution method. • “Weak springs” is also meant for the initial static analysis. • “Large Deflection” is not supported for a buckling analysis. – The “Analysis Type” will display “Buckling” for the case of a linear buckling analysis. ANSYS Workbench – Simulation • The solution branch provides details on the type of analysis being performed March 29, 2005 Inventory #002215 7 -15

Linear Buckling Analysis … Solving the Model Training Manual – A linear buckling analysis is more computationally expensive than a static analysis on the same model. This is because a static analysis and a buckling analysis are both performed. – If a “Solution Information” branch was requested, detailed solution output is available in the Worksheet tab of that branch, including the amount of memory used and no. of modes have already been extracted – If stress or strain results or more buckling modes are requested after a solution is performed, a new solution is required. ANSYS Workbench – Simulation • After setting up the model, one can solve the buckling analysis just like any other analysis by selecting the Solve button. March 29, 2005 Inventory #002215 7 -16

Linear Buckling Analysis … Reviewing Results Training Manual – The Load Multiplier for each buckling mode is shown in the Details view. The load multiplier times the actual loads represent the critical load. – The buckling modes do not represent actual, realistic magnitudes. However, these can be used to determine what the failure modes may look like. Model shown is from a sample Inventor part. ANSYS Workbench – Simulation • After the solution, the buckling modes can be reviewed March 29, 2005 Inventory #002215 7 -17

Linear Buckling Analysis … Reviewing Results Training Manual – The tower model below has been solved twice. In the first case a unit load is applied. In the second an expected load applied (see next page) ANSYS Workbench – Simulation • Interpreting the Load Multiplier ( ): March 29, 2005 Inventory #002215 7 -18

Linear Buckling Analysis … Reviewing Results Training Manual • In the first case the load Multiplier is simply interpreted as the buckling load. • In the second case the Load Multiplier is interpreted as a safety factor. ANSYS Workbench – Simulation • Interpreting the Load Multiplier ( ): March 29, 2005 Inventory #002215 7 -19

Linear Buckling Analysis … Reviewing Results Training Manual – All requested modes will be summarized in the table below – As mentioned earlier, it may be advisable to request more than just the first buckling mode. This allows the user to see if the structure may be able to buckle in more than one way under a given applied load. ANSYS Workbench – Simulation • The buckling load multipliers can be reviewed in the Worksheet tab of the Bucking branch. March 29, 2005 Inventory #002215 7 -20

Linear Buckling Analysis C. Workshop 7 Training Manual • Goal: – Verify linear buckling results in Simulation for the pipe model shown below. Results will be compared to closed form calculations from a handbook. ANSYS Workbench – Simulation • Workshop 7 – Linear Buckling March 29, 2005 Inventory #002215 7 -21

March 29, 2005 Inventory #002215 7 -22