Linear%20Buckling

1
Linear Buckling

• Workshop 7

2
Workshop 7 - Goals

• 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.

3
Workshop 7 - Assumptions

• 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
• OD 4.5 in ID 3.5 in. E 30e6 psi, I 12.7
  in4, L 120 in.
• In this case we assume the pipe conforms to the
  following handbook formula where P is the
  critical load
• For the case of a fixed / free beam the parameter
  K 0.25.

4
. . . Workshop 7 - Assumptions

• Using the formula and data from the previous page
  we can predict the buckling load will be

5
Workshop 7 - Start Page

• From the launcher start Simulation.
• Choose Geometry gt 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.

6
Workshop 7 - Preprocessing

• Set the working unit system to the U.S. customary
  system
• Units gt U.S. Customary (in, lbm, psi, F, s).
• To make the material property match that of our
  hand calculation highlight the Solid branch in
  the tree
• Details gt Material gt Edit Structural Steel . . .
  

1
2
7
. . . Workshop 7 - Preprocessing

• In the field for Youngs Modulus type in the
  value 3e7.
• 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.

3
8
Workshop 7 - Environment

• Fix one end of the pipe
• Highlight the Environment branch.
• Select the surface on one end of the pipe.
• RMB gt Insert gt Fixed Support.

4
5
6
9
. . . Workshop 7 - Environment

• Add a unit force to one end of the pipe
• Select the surface on the free end of the pipe.
• RMB gt Insert gt Force.
• In the force detail change the Define by field
  to Components.
• In the force detail enter 1 in the Magnitude
  field.

7
8
10
Workshop 7 - Solution

• Insert the buckling tool into the solution
  branch
• Highlight the solution branch.
• RMB gt Insert gt Buckling.
• Solve.
• Notice the default setting for buckling is to
  find the first buckling mode.

12
11
Workshop 7 - Results

• When the solution completes review the buckling
  result.
• Highlight the 1st Buckled Mode result object.
• 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.

12
. . . Workshop 7 - Results

• Change the force value to the expected load
  (10000 lbf).
• Highlight the Force branch.
• In the detail field for the Z Component enter
  10000.
• Solve

15
13
. . . Workshop 7 - Results

• When the solution completes note the Load
  Multiplier field now shows a value of 6.56.
  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.

14
Workshop 7 - Verification

• 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.

15
. . . Workshop 7 - Verification

• Highlight the Buckling branch and delete it.
• RMB gt Delete
• RMB gt Insert gt Stress gt Equivalent (von Mises)

18
16
. . . Workshop 7 - Verification

• Insert total deformation
• RMB gt Insert gt Deformation gt Total
• 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.

17
. . . Workshop 7 - Verification

• 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.

18
(No Transcript)