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
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).
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
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
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
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.
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
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
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).
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
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).
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
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).
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