The document provides an overview of buckling analysis in ANSYS. It discusses buckling of columns with well-defined end conditions, buckling of a special column, and second order analysis of a simple beam. The preprocessing, solution, and postprocessing phases of ANSYS are outlined. Step-by-step instructions are given for modeling each example and obtaining the buckling load using eigenvalue buckling analysis. Manual calculations are also shown for comparison.

1. ANSYS TUTORIAL
BUCKLING ANALYSIS
ENG. MAHA MODDATHER HASSAN
T.A. CAIRO UNIVERSITY, EGYPT

2. SESSION OUTLINE

Introduction

Buckling of Column with well-defined End Conditions.

Buckling of Special Column.

Second Order Analysis of a Simple Beam.

Buckling of Frame.

Home Work

3. INTRODUCTION

ANSYS is a finite element program that can perform:
 Static Linear Analyses
 Static Nonlinear Analyses
 Dynamic Linear Analyses
 Dynamic Nonlinear Analyses
 Heat Transfer Problems
 Fluid Problems
 Electromagnetic Problems

4. INTRODUCTION
ANSYS can be used for analyzing
Skeletal Structures Non-skeletal Structures
2D 3D
Domes
Slabs
Beams Trusses
Frames

5. INTRODUCTION
ANSYS
Preprocessing Post processing
Analysis Steps
Solution
Geometry
Material Properties Apply Boundary
Conditions (Restraints)
Obtaining Results
Type of Problem
Apply Loads
Choose Elements
Solution Control

6. INTRODUCTION
General View of ANSYS Program :

7. INTRODUCTION
Preprocessing Phase

8. INTRODUCTION
Solution Phase

9. INTRODUCTION
Post processing Phase

10. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
Column Section
20 cm
10 cm
P
P
Get Pcr using Eigen buckling analysis in Ansys and
compare with manual solution? (E = 2000 t/cm2
)

11. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
P
P
Exact Solution:
Pcr = Π2
EI/L2
Pcr = Π2
(2000)I/6002
= 91.4 ton
Ix = 10(20)3
/12 = 6666.67 cm4
Iy = 20(10)3
/12 = 1666.67 cm4

12. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
P
P
Using ANSYS 12.0:Preprocessing Phase:
1.Define key points
Preprocessor > Modeling > create >
keypoints > In active CS
Y
X
1
2
POINT ( X , Y)
1 ( 0 , 0)
2 ( 0 , 600)

13. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
P
P
Y
X
1
2
POINT ( X , Y)
1 ( 0 , 0)
2 ( 0 , 600)

14. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
P
P
Y
X
1
2
POINT ( X , Y)
1 ( 0 , 0)
2 ( 0 , 600)

15. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
600cm
P
P
Y
X
1
2
Using ANSYS 12.0:Preprocessing Phase:
2. Define line between keypoints
Preprocessor > Modeling > Create > Lines > Lines
> In Active Coord

16. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
2. Pick points 1,2

17. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
3. Define type of element
Preprocessor > Element Type > Add/Edit/Delete
For this problem we will use the BEAM3 (Beam 2D
elastic) element. This element has 3 degrees of
freedom (translation along the X and Y axes, and
rotation about the Z axis).

18. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS

19. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
4. Define real constants
Preprocessor > Real Constants... > Add
In the 'Real Constants for BEAM3' window, enter the following
geometric properties:
i. Cross-sectional area AREA: 200
ii. Area moment of inertia IZZ: 1666.67
iii. Total Beam Height HEIGHT: 20

20. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS

21. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
5. Define Material Properties
Preprocessor > Material Props > Material Models > Structural > Linear
> Elastic > Isotropic
In the window that appears, enter the following geometric properties :
i. Young's modulus EX: 2000
ii. Poisson's Ratio PRXY: 0.3

22. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
6. Define Mesh
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All
Lines...
For this example we will specify an element edge length of 10 cm (10
element divisions along the line).

23. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Preprocessing Phase:
7. Apply Mesh
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

24. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Solution Phase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
2. Activate prestress effects
To perform an eigenvalue buckling analysis, prestress effects must be
activated.
Select Solution > Analysis Type > sol’n control
change the [SSTIF][PSTRES] item to 'Prestress ON', which ensures the stress
stiffness matrix is calculated. This is required in eigenvalue buckling

25. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS

26. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 1 and Fix Ux and Uy.

27. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 2 and Fix in X direction.

28. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Solution Phase:
4. Apply Loads
Solution > Define Loads > Apply > Structural > Force/Moment > On
Keypoints
The eignenvalue solver uses a unit force to determine the necessary
buckling load. Applying a load other than 1 will scale the answer by a
factor of the load. Apply a vertical (FY) point load of -1 ton to the top of
the beam (keypoint 2).

29. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0:Solution Phase:
5. Solve the system
Solution > Solve > Current LS

30. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0: Post Processing Phase:
1. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu.
Normally at this point you enter the post processing phase. However,
with a buckling analysis you must re-enter the solution phase
and specify the buckling analysis. Be sure to close the solution menu
and re-enter it or the buckling analysis may not function
properly.

31. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0: Second SolutionPhase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Eigen Buckling
2. Specify Buckling Analysis Options
Select Solution > Analysis Type > Analysis Options

32. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0: Second SolutionPhase:
Complete the window as shown below:
3. Solve the system
Solution > Solve > Current LS

33. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0: Second SolutionPhase :
4. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu as before
Using ANSYS 12.0: Post Processing Phase:
1. View the buckling load
To display the minimum load required to buckle the beam select
General Postproc > List Results > Detailed Summary
Buckling load as
calculated before

34. BUCKLING OF COLUMN WITH WELL-DEFINED END
CONDITIONS
Using ANSYS 12.0: Post Processing Phase:
2. Display buckling mode
Select General Postproc > Read Results > Last Set to bring up the
data for the last mode calculated
Select General Postproc > Plot Results > Deformed Shape

35. BUCKLING OF SPECIAL COLUMN
450cm
Section 10 cm
10 cm
P
Get Pcr using approximate analysis, exact analysis,
and Eigen buckling analysis in Ansys and compare?
(E = 2000 t/cm2
)
P
300cm

36. BUCKLING OF SPECIAL COLUMN
Approximate Solution:
Pcr = Π2
EI/Lmax
2
Pcr = Π2
(2000)I/4502
= 81.231 ton
Ix = 10(10)3
/12 = 833.333 cm4
Exact Solution:
From lecture notes :
Pcr = 5.89EI/Lmin
2
= 5.89 (2000)x833.33/3002
= 109.0 ton

37. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Preprocessing Phase:
1.Define key points
Preprocessor > Modeling > create > keypoints > In active
CS
450cm
1
300cm
2 3
POINT ( X , Y)
1 ( 0 , 0)
2 ( 300 , 0)
3 ( 750 , 0)
Y
X

38. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Preprocessing Phase:
2. Define line between keypoints
Preprocessor > Modeling > Create > Lines > Lines > In Active Coord
Define line between (1 and 2) then between (2 and 3)

39. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Preprocessing Phase:
3. Define type of element
Preprocessor > Element Type > Add/Edit/Delete
For this problem we will use the BEAM3 (Beam 2D elastic) element. This
element has 3 degrees of freedom (translation along the X and Y axes,
and rotation about the Z axis).

40. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Preprocessing Phase:
4. Define real constants
Preprocessor > Real Constants... > Add
In the 'Real Constants for BEAM3' window, enter the following geometric
properties:
i. Cross-sectional area AREA: 100
ii. Area moment of inertia IZZ: 833.33
iii. Total Beam Height HEIGHT: 10

41. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Preprocessing Phase:
5. Define Material Properties
Preprocessor > Material Props > Material Models > Structural > Linear >
Elastic > Isotropic
In the window that appears, enter the following geometric properties :
i. Young's modulus EX: 2000
ii. Poisson's Ratio PRXY: 0.3
6. Define Mesh
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All
Lines...
For this example we will specify an element edge length of 10 cm (10
element divisions along the line).
7. Apply Mesh
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

42. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
2. Activate prestress effects
To perform an eigenvalue buckling analysis, prestress effects must be
activated.
Select Solution > Analysis Type > sol’n control
change the [SSTIF][PSTRES] item to 'Prestress ON', which ensures the stress
stiffness matrix is calculated. This is required in eigenvalue buckling

43. BUCKLING OF SPECIAL COLUMN

44. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 1 and Fix Ux and Uy.

45. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 2 and 3, then Fix Uy.

46. BUCKLING OF SPECIAL COLUMN

47. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
4. Apply Loads
Solution > Define Loads > Apply > Structural > Force/Moment > On
Keypoints
The eignenvalue solver uses a unit force to determine the necessary
buckling load. Applying a load other than 1 will scale the answer by a
factor of the load. Apply a vertical (Fx) point load of -1 ton to the top of
the beam (keypoint 3).

48. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
5. Solve the system
Solution > Solve > Current LS

49. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0: Post Processing Phase:
1. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu.
Normally at this point you enter the post processing phase. However,
with a buckling analysis you must re-enter the solution phase
and specify the buckling analysis. Be sure to close the solution menu
and re-enter it or the buckling analysis may not function
properly.

50. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0: Second SolutionPhase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Eigen Buckling
2. Specify Buckling Analysis Options
Select Solution > Analysis Type > Analysis Options

51. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0: Second SolutionPhase:
Complete the window as shown below:
3. Solve the system
Solution > Solve > Current LS

52. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0: Second SolutionPhase :
4. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu as before
Buckling load as
calculated before
Using ANSYS 12.0: Post Processing Phase:
1. View the buckling load
To display the minimum load required to buckle the beam select
General Postproc > List Results > Detailed Summary

53. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0: Post Processing Phase:
2. Display buckling mode
Select General Postproc > Read Results > Last Set to bring up the
data for the last mode calculated
Select General Postproc > Plot Results > Deformed Shape

54. SECOND ORDER ANALYSIS
200cm
Section
50 cm
30 cm
10ton
Get the value of max bending moment and deflection using : first
order analysis, exact analysis, and ANSYS? (E = 2000 t/cm2
(
300cm 300cm
10ton
P = 80 ton P = 80 ton

55. SECOND ORDER ANALYSIS
Using first order Analysis:
Mmax = 3000 t.cm
Ymax = 0.312 cm
Exact Solution:
From lecture notes : using superposition or exact analysis:
Mmax = 3025 t.cm
Ymax = 0.3146 cm

56. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Preprocessing Phase:
1.Define key points
Preprocessor > Modeling > create > keypoints > In active
CS
1 2 4
POINT ( X , Y)
1 ( 0 , 0)
2 ( 300 , 0)
3 ( 500 , 0)
4 ( 800 , 0)
Y
X
200cm
10ton
300cm 300cm
10ton
3

57. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Preprocessing Phase:
2. Define line between keypoints
Preprocessor > Modeling > Create > Lines > Lines > In Active Coord
Define line between (1 and 2( then between (2 and 3( then between (3 and 4(

58. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Preprocessing Phase:
3. Define type of element
Preprocessor > Element Type > Add/Edit/Delete
For this problem we will use the BEAM3 (Beam 2D elastic( element. This
element has 3 degrees of freedom (translation along the X and Y axes,
and rotation about the Z axis(.

59. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Preprocessing Phase:
4. Define real constants
Preprocessor > Real Constants... > Add
In the 'Real Constants for BEAM3' window, enter the following
geometric properties:
i. Cross-sectional area AREA: 1500
ii. Area moment of inertia IZZ: 312500
iii. Total Beam Height HEIGHT: 50

60. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Preprocessing Phase:
5. Define Material Properties
Preprocessor > Material Props > Material Models > Structural > Linear >
Elastic > Isotropic
In the window that appears, enter the following geometric properties :
i. Young's modulus EX: 2000
ii. Poisson's Ratio PRXY: 0.3
6. Define Mesh
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All
Lines...
For this example we will specify an element edge length of 10 cm (10
element divisions along the line(.
7. Apply Mesh
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

61. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Solution Phase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
2. Activate prestress effects
To perform an large deflection analysis, prestress effects must be activated.
Select Solution > Analysis Type > sol’n control
change the [SSTIF][PSTRES] item to 'Prestress ON', which ensures the stress
stiffness matrix is calculated. This is required in eigenvalue buckling
analysis.

62. SECOND ORDER ANALYSIS

63. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 1 and Fix Ux and Uy.

64. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 4, then Fix Uy.

65. BUCKLING OF SPECIAL COLUMN

66. BUCKLING OF SPECIAL COLUMN
Using ANSYS 12.0:Solution Phase:
4. Apply Loads
Solution > Define Loads > Apply > Structural > Force/Moment > On
Keypoints
Apply -10 tons at points (2 and 3( in Fy direction.

67. SECOND ORDER ANALYSIS
Using ANSYS 12.0:Solution Phase:
5. Solve the system
Solution > Solve > Current LS

68. SECOND ORDER ANALYSIS
Using ANSYS 12.0: Post Processing Phase:
1. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu.
Normally at this point you enter the post processing phase. However,
with a buckling analysis you must re-enter the solution phase
and specify the buckling analysis. Be sure to close the solution menu
and re-enter it or the buckling analysis may not function
properly.

69. SECOND ORDER ANALYSIS
Using ANSYS 12.0: Post Processing Phase:
1. Display deformed shape
select General Postproc > Plot Results > Deformed Shape
Max y = 0.3148 cm

70. SECOND ORDER ANALYSIS
Using ANSYS 12.0: Post Processing Phase:
2. Display moment
select General Postproc > element table > define table

71. SECOND ORDER ANALYSIS

72. SECOND ORDER ANALYSIS
Using ANSYS 12.0: Post Processing Phase:
2. Display moment
select General Postproc > element table > plot elem table

73. SECOND ORDER ANALYSIS
Max Moment = 3025 t.cm

74. BUCKLING OF FRAMES
Section
50 cm
30 cm
600cm
600cm
P P
Get Pcr using Eigen buckling analysis in Ansys and
compare with manual solution? (E = 2000 t/cm2
(
Also, compare with the value extracted from alignment
charts.

75. BUCKLING OF FRAMES
Exact Solution:
Pcr = 1.815EI/L2
= 1.82x2000x I /6002
= 3151 ton
I = 30(50(3
/12 = 312500 cm4
Using Alignment Charts:
For sway frame Case:
GA = 10
GB = EI/Lcol/EI/Lbeams = 1
K = 1.88
Pcr = 1.88EI/L2
= 1.83x2000x I /6002
= 3264 ton

76. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
1.Define key points
Preprocessor > Modeling > create > keypoints > In active
CS
POINT ( X , Y)
1 ( 0 , 0)
2 ( 0 , 600)
3 ( 600 , 600)
4 ( 600 , 0)
2 3
1 4X
Y

77. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
2. Define line between keypoints
Preprocessor > Modeling > Create > Lines > Lines > In Active Coord

78. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
2. Pick points 1,2 then 2,3 then 3,4

79. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
3. Define type of element
Preprocessor > Element Type > Add/Edit/Delete
For this problem we will use the BEAM3 (Beam 2D elastic) element. This
element has 3 degrees of freedom (translation along the X and Y axes,
and rotation about the Z axis).

80. BUCKLING OF FRAMES

81. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
4. Define real constants
Preprocessor > Real Constants... > Add
In the 'Real Constants for BEAM3' window, enter the following
geometric properties:
i. Cross-sectional area AREA: 1500
ii. Area moment of inertia IZZ: 312500
iii. Total Beam Height HEIGHT: 50

82. BUCKLING OF FRAMES

83. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
5. Define Material Properties
Preprocessor > Material Props > Material Models > Structural > Linear
> Elastic > Isotropic
In the window that appears, enter the following geometric properties :
i. Young's modulus EX: 2000
ii. Poisson's Ratio PRXY: 0.3

84. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
6. Define Mesh
Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All
Lines...
For this example we will specify an element edge length of 10 cm (10
element divisions along the line).

85. BUCKLING OF FRAMES
Using ANSYS 12.0:Preprocessing Phase:
7. Apply Mesh
Preprocessor > Meshing > Mesh > Lines > click 'Pick All'

86. BUCKLING OF FRAMES

87. BUCKLING OF FRAMES
Using ANSYS 12.0:Solution Phase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Static
2. Activate prestress effects
To perform an eigenvalue buckling analysis, prestress effects must be
activated.
Select Solution > Analysis Type > sol’n control
change the [SSTIF][PSTRES] item to 'Prestress ON', which ensures the stress
stiffness matrix is calculated. This is required in eigenvalue buckling

88. BUCKLING OF FRAMES

89. BUCKLING OF FRAMES
Using ANSYS 12.0:Solution Phase:
3. Apply Constraints
Solution > Define Loads > Apply > Structural > Displacement > On
Keypoints
Select Keypoint 1 and 4 and Fix Ux and Uy.

90. BUCKLING OF FRAMES

91. BUCKLING OF FRAMES
Using ANSYS 12.0:Solution Phase:
4. Apply Loads
Solution > Define Loads > Apply > Structural > Force/Moment > On
Keypoints
The eignenvalue solver uses a unit force to determine the necessary
buckling load. Applying a load other than 1 will scale the answer by a
factor of the load. Apply a vertical (FY) point load of -1 ton to the top of
the beam (keypoint 2 and 3).

92. BUCKLING OF FRAMES

93. BUCKLING OF FRAMES
Using ANSYS 12.0:Solution Phase:
5. Solve the system
Solution > Solve > Current LS

94. BUCKLING OF FRAMES
Using ANSYS 12.0: Post Processing Phase:
1. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu.
Normally at this point you enter the post processing phase. However,
with a buckling analysis you must re-enter the solution phase
and specify the buckling analysis. Be sure to close the solution menu
and re-enter it or the buckling analysis may not function
properly.

95. BUCKLING OF FRAMES
Using ANSYS 12.0: Second SolutionPhase:
1. Define Analysis Type
Solution > Analysis Type > New Analysis > Eigen Buckling
2. Specify Buckling Analysis Options
Select Solution > Analysis Type > Analysis Options

96. BUCKLING OF FRAMES
Using ANSYS 12.0: Second SolutionPhase:
Complete the window as shown below:
3. Solve the system
Solution > Solve > Current LS

97. BUCKLING OF FRAMES
Using ANSYS 12.0: Second SolutionPhase :
4. Exit solution phase
Close the solution menu and click FINISH at the bottom of the Main
Menu as before
Using ANSYS 12.0: Post Processing Phase:
1. View the buckling load
To display the minimum load required to buckle the beam select
General Postproc > List Results > Detailed Summary
Buckling load as
calculated before

98. BUCKLING OF FRAMES
Using ANSYS 12.0: Post Processing Phase:
2. Display buckling mode
Select General Postproc > Read Results > Last Set to bring up the
data for the last mode calculated
Select General Postproc > Plot Results > Deformed Shape

99. HOME WORK
400cm
Column Section
40 cm
20 cm
P
P
Get Pcr using Eigen buckling analysis in Ansys and
compare with manual solution? (E = 2100 t/cm2
)

100. HOME WORK
700cm
Section 20 cm
20 cm
P
Get Pcr using approximate analysis, exact analysis, and Eigen
buckling analysis in Ansys and compare? (E = 2000 t/cm2
)
P
350cm
EI 2EI

101. HOME WORK
Section
60 cm
25 cm
Get the value of max bending moment and deflection using : first
order analysis, exact analysis, and ANSYS? (E = 2000 t/cm2
)
400cm 400cm
10ton
P = 90 ton P = 90 ton

102. THANK YOU