6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Tran Kim Bang

Department of Engineering Mechanics (DEM),
Faculty of Applied Sciences,
Ho Chi Minh City University of Technology,
Email: tkbang@hcmut.edu.vn

Structural Analysis Chapter 6. Structural Vibration and Dynamics 1

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Chapter 6. Structural
Vibration and Dynamics

Structural Analysis Chapter 6. Structural Vibration and Dynamics 2

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Case Study with ANSYS Workbench

• Musical instruments such
as acoustic guitars create
sound by means of
vibration and resonance.
The body of an acoustic
guitar acts as a resonating
chamber when the strings
are set into oscillation at
their natural frequencies.
• The guitar has a wall
thickness of 3 mm, and is
made of Douglas fir wood
(E = 13.1 GPa, Poison’s
ratio ν = 0.3, density = 470
kg/m3).
• Assuming the back
surface of the guitar is
fixed, find the first 10 • Suppose a harmonic pressure loading of magnitude
natural frequencies and 1 MPa is applied to a side wall of the guitar. Plot the
plot the first five vibration frequency response of the z displacement (along
modes of the guitar. the surface normal direction) of the front surface.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 9

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 1: Start an ANSYS Workbench Project

Launch ANSYS Workbench and save the blank project as “Guitar.wbpj.”
Step 2: Create a Modal Analysis System
Drag the Modal icon from the Analysis Systems Toolbox window and drop it inside the
highlighted green rectangle in the Project Schematic window to create a standalone
modal analysis system.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 10

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 3: Add a New Material

Double-click on the Engineering Data cell to add a new material. In the following
Engineering Data interface which replaces the Project Schematic, type “Wood” as the
name for the new material, and double-click Isotropic Elasticity under Linear Elastic in
the leftmost Toolbox window. Enter “13.1E9” for Young’s Modulus and “0.3” for
Poisson’s Ratio in the Properties window. Double-click Density under Physical
Properties. Enter “470” for Density in the Properties window.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 11

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 4: Launch the DesignModeler Program

Ensure Surface Bodies is checked in the Properties of Schematic A3: Geometry
window (select Properties from the View drop-down menu to enable display of this
window). Choose 3D as the Analysis Type in this Properties window. Doubleclick the
Geometry cell to launch DesignModeler, and select “Millimeter” in the Units pop-up
window.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 12

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 5: Create a Profile Sketch

Click on the Sketching tab. Select the Draw toolbox and then Construction Point.
Draw 10 construction points A through J, as shown below. Draw a spline passing
through points A through J; right-click at the last construction point and choose Open
End from the context menu to finish the spline creation.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 13

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 6: Create a Replicate Curve

Select the Modify toolbox and then Replicate. Click on the spline from the Graphics
window. Right-click anywhere in the Graphics to show the context menu. Select
End/Use Plane Origin as Handle as shown below. A replicate spline will appear in the
Graphics window.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 14

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Next, right-click anywhere in the Graphics, and select Flip Vertical in the context
menu. A vertically flipped spline will appear.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 15

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click on the origin point in the Graphics to place the flipped spline, right click and
chose End. A closed-loop curve is now formed as shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 16

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 7: Create an Extruded Body

Switch to the Modeling tab and click on the Extrude feature. The default Base Object is
set as Sketch1 in the Details of Extrude1. Change the extrusion depth to 50 mm in the
field of FD1, Depth and click Generate. A solid body is created as shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 17

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 8: Create an Extruded Cut on the Front Face

Create a new plane by selecting New Plane from the Create drop-down menu.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 18

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

A new plane named Plane4 is now added to the Tree Outline. In the Details of Plane4,
set the Type to From Face. Click the front face of the guitar from the Graphics
window, and apply it to the Base Face selection in the Details of Plane4. Click
Generate.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 19

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

To create a new sketch under Plane4 in the Tree Outline, click on the New Sketch icon.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 20

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Switch to the Sketching tab for Sketch2. In the sketch, draw a horizontal line by
connecting points A and B as shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 21

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Then draw a circle of diameter 45 mm centered at point C, located 170 mm to the left
of point A along line AB.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 22

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Next, choose Trim under the Modify tab, and click on line AB in the Graphics window.
The sketch line AB will disappear.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 23

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Switch to the Modeling tab, and click on the Extrude feature. The default Base Object is
set as Sketch2 in the Details of Extrude2. Set the Operation to Cut Material. Enter an
extrusion depth of 10 mm in the field of FD1, Depth and click Generate. An extruded cut
feature is now added to the front face as shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 24

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 9: Create a Surface Body

Select Surface from Faces from the Concept drop-down menu. In the Graphics
window, Ctrl-click to select four faces, that is, the front, back, top, and bottom faces
that enclose the solid body as shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 25

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click Apply next to Faces in the Details of SurfFromFaces1. Then click Generate. A
surface body will be generated in the Tree Outline under 2 Parts, 2 Bodies.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 26

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Solid under 2 Parts, 2 Bodies in the Tree Outline. In the context menu,
select Suppress Body.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 27

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click on Surface Body under 2 Parts, 2 Bodies in the Tree Outline. Change the
Thickness to 3 mm in the Details of Surface Body. Save and exit the DesignModeler.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 28

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 10: Launch the Modal–Mechanical

Program Double-click on the Model cell to launch the Modal–Mechanical program.
Click on the Surface Body under Geometry in the Outline tree. In the Details of
“Surface Body,” click to the right of the Material Assignment field and select Wood
from the drop-down menu.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 29

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 11: Generate Mesh

Right click on Mesh in the Project Outline. Select Insert and then Sizing from the
context menu.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 30

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

In the Details of “Face Sizing,” enter “5e-3 m” for the Element Size. Click on the front,
back, top, and bottom faces of the guitar in the Graphics window and apply the four
faces to the Geometry selection.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 31

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Mesh in the Outline, and select Generate Mesh from the context menu.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 32

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 12: Set Up Modal Analysis and Apply Boundary Conditions

Click on Analysis Settings under Modal in the Outline tree. Change the Max Modes to
Find to 10 in the Details of “Analysis Settings.”

Structural Analysis Chapter 6. Structural Vibration and Dynamics 33

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Modal(A5). Choose Insert and then Fixed Support from the context
menu. Apply the back face to the Geometry selection.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 34

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 13: Retrieve Results from Modal Analysis

Insert Total Deformation by right-clicking on Solution (A6) in the Outline. In the Details
of “Total Deformation,” set Mode to 1. Insert another Total Deformation item. In the
Details of “Total Deformation 2,” set Mode to 2. Repeat this step three more times. Set
Mode to 3, 4, and 5, respectively, for each new insertion. Right click on Solution (A6) in
the Outline and Solve

Structural Analysis Chapter 6. Structural Vibration and Dynamics 35

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click on Total Deformation in the Outline to review results. The results below show
the first natural frequency of 1038.7 Hz and the corresponding mode shape.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 36

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click on Tabular Data and Graph on the right edge of the Graphics window, and then
click on the push pin labeled AutoHide to display the Tabular data and the Graph as
shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 37

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

The Tabular data gives the first 10 natural frequencies of the guitar under the fixed
bottom boundary condition. The Play/Stop control interface in the Graph window
allows animation of mode shapes. Click on each different Total Deformation item in the
Outline to review results.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 38

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 14: Create a Harmonic Response Analysis System

Drag the Harmonic Response icon from the Analysis Systems Toolbox window and
drop it onto the Solution cell of the highlighted Modal system in the Project
Schematic.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 39

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

This creates a Harmonic Response system that shares data with Modal system as
shown below.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 40

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 15: Set Up Harmonic Response Analysis and Assign Loads

Double-click on the Setup cell of the Harmonic Response system to launch the Multiple
Systems–Mechanical program. In the program, select Analysis Settings from the
Outline. Set the Range Minimum to 1000 Hz, Range Maximum to 4000 Hz, and
Solution Intervals to 300. Click on Analysis Settings under Modal in the Outline tree.
Change the Max Modes to Find to 15 in the Details of “Analysis Settings.”

Structural Analysis Chapter 6. Structural Vibration and Dynamics 41

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Harmonic Response (B5). Choose Insert and then Pressure from the
context menu. In the Details of “Pressure,” set magnitude as 1e6 Pa, and apply the
top face to the Geometry selection.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 42

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 16: Retrieve Results from Harmonic Response

Right-click on Solution (B6). Choose Insert and Frequency Response and then
Deformation from the context menu. In the Details of “Frequency Response,” set the
Orientation of the directional deformation to Z-Axis. Click on the front face and apply
it to the Geometry selection.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 43

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Solution (B6) and select Solve. After solution is done, click on
Frequency Response in the Outline to review the harmonic response of the guitar.

Structural Analysis Chapter 6. Structural Vibration and Dynamics 44

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics
Homework 1

Structural Analysis Chapter 6. Structural Vibration and Dynamics 47

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Homework 2

Structural Analysis Chapter 6. Structural Vibration and Dynamics 48

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Structural Analysis Chapter 6. Structural Vibration and Dynamics 49

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Tran Kim Bang

Department of Engineering Mechanics (DEM),
Faculty of Applied Sciences,
Ho Chi Minh City University of Technology,
Email: tkbang@hcmut.edu.vn

Structural Analysis Chapter 8. Failure Analysis 1

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Chapter 8. Failure
Analysis

Structural Analysis Chapter 8. Failure Analysis 2

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Case Studies with ANSYS Workbench

A dog-bone shaped specimen is examined for static,
fatigue, and buckling failures. The specimen is made
of structural steel with geometric dimensions shown
below. The bottom face of the specimen is fixed, and
the top face of the specimen is applied a static
pressure load of 50 MPa.
(a) Determine whether or not the specimen
undergoes plastic deformation under the given
static pressure load.
(b) If the static pressure load is changed into a fully
reversed cyclic load with a magnitude of 50 MPa,
find the life of the specimen, and also determine
whether or not fatigue failure occurs in the
specimen assuming a design life of 106 cycles.
(c) Determine whether or not the specimen buckles
under the given static pressure load, and obtain
the first three buckling mode shapes.

Structural Analysis Chapter 8. Failure Analysis 15

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics
Solution steps for portion (A and B):
Step 1: Start an ANSYS Workbench Project
Launch ANSYS Workbench and save the blank project as “Dogbone.wbpj.”
Step 2: Create a Static Structural Analysis System
Drag the Static Structural icon from the Analysis Systems Toolbox window and drop
it inside the highlighted green rectangle in the Project Schematic window.

Structural Analysis Chapter 8. Failure Analysis 16

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 3: Launch the DesignModeler Program

Double-click the Geometry cell to launch DesignModeler, and select “Millimeter” in
the Units pop-up window.

Structural Analysis Chapter 8. Failure Analysis 17

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 4: Create the Geometry

Click on the Sketching tab. Draw a sketch of the dog bone shape on the XY Plane, as
shown below. An entity named Sketch1 will be shown underneath XY Plane of the
model’s Tree Outline.

Structural Analysis Chapter 8. Failure Analysis 18

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Extrude Sketch1 to create a 0.75 mm thick solid body, as shown below.

Structural Analysis Chapter 8. Failure Analysis 19

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 5: Launch the Static Structural Program

Double-click on the Model cell to launch the Static Structural program. Change the
Units to Metric (mm, kg, N, s, mV, mA).

Structural Analysis Chapter 8. Failure Analysis 20

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 6: Generate Mesh

Click on Mesh in the Outline tree. In the Details of “Mesh,” enter “0.5 mm” for the
Element Size. Right-click on Mesh and select Generate Mesh.

Structural Analysis Chapter 8. Failure Analysis 21

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 7: Apply Boundary Conditions

Right-click on Static Structural (A5). Choose Insert and then Fixed Support from the
context menu. Click on the bottom face, and apply it to the Geometry selection in the
Details of “Fixed Support.” The bottom face of the dog bone shape is now fixed as
shown below.

Structural Analysis Chapter 8. Failure Analysis 22

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 8: Apply Loads

Right-click on Static Structural (A5). Choose Insert and then Pressure. In the Details
of “Pressure,” apply a 50 MPa pressure to the top face, as shown below.

Structural Analysis Chapter 8. Failure Analysis 23

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 9: Retrieve Static Analysis Results

First, insert a Total Deformation item by right-clicking on Solution (A6) in the project
Outline. Then, insert an Equivalent Stress item by right-clicking on Solution (A6) in
the project Outline.

Structural Analysis Chapter 8. Failure Analysis 24

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Next, right-click on Solution (A6) in the project Outline, and select Insert -> Stress
Tool -> Max Equivalent Stress. The initial yielding in the test sample may be
predicted by comparing the maximum von-Mises stress in the specimen with the
tensile yield strength of the specimen material. The Stress Tool is used here to
show the safety factor results.

Structural Analysis Chapter 8. Failure Analysis 25

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Solution (A6) and select Solve. The computed total deformation, von-
Mises stress and safety factor distributions are shown below. From the static
analysis results, it is apparent that the neck portion of the specimen will not yield if
loaded statically.

Structural Analysis Chapter 8. Failure Analysis 26

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 10: Retrieve Fatigue Analysis Solution

Right-click on Solution (A6) in the Outline, and select Insert -> Fatigue -> Fatigue Tool.

Structural Analysis Chapter 8. Failure Analysis 27

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

In the Details of “Fatigue Tool,” set the Mean Stress Theory to Goodman. Note that
the default loading type is Fully Reversed constant amplitude load, and that the
default analysis type is the Stress Life type using the von-Mises stress calculations.

Structural Analysis Chapter 8. Failure Analysis 28

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on the Fatigue Tool in the Outline, and select Insert -> Life.

Structural Analysis Chapter 8. Failure Analysis 29

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Next, right-click on the Fatigue Tool and select Insert -> Safety Factor. In the Details of
“Safety Factor,” change the Design life from the default value of 109 cycles to 106
cycles.

Structural Analysis Chapter 8. Failure Analysis 30

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Finally, right-click on the Fatigue Tool and select Evaluate All Results. From the fatigue
analysis results, the shortest life is at the undercut fillets (19,079 cycles) followed by
the neck portion of the specimen. The neck portion of the specimen has a fairly small
safety factor with a minimum value of 0.3973. The results show that the specimen will
not survive the fatigue testing assuming a design life of 106 cycles.

Structural Analysis Chapter 8. Failure Analysis 31

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Solution steps for portion (C):

Step 1: Create a Eigenvalue (linear) Buckling Analysis System
In the Project Schematic window, right-click on the Solution cell of the Static
Structural analysis system and select Transfer Data to New -> Eigenvalue Buckling.

Structural Analysis Chapter 8. Failure Analysis 32

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

An Eigenvalue buckling analysis system will be added, with the static structural
results being used as initial conditions. The engineering data, geometry, and model
will be shared by both analyses.

Structural Analysis Chapter 8. Failure Analysis 33

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Step 2: Launch the Multiple Systems–Mechanical Program

Double-click the Setup cell of the Eigenvalue Buckling system to launch the Multiple
Systems– Mechanical program.

Structural Analysis Chapter 8. Failure Analysis 34

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Click on the Analysis Settings under Eigenvalue Buckling (B5) in the Outline. In the
Details of “Analysis Settings,” set the Max Modes to Find to 3 and Include Negative
Load Multiplier to No

Structural Analysis Chapter 8. Failure Analysis 35

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Right-click on Solution (B6) and select Solve to view the buckling modes. To use the
default window layout as shown below, select View -> Windows -> Reset Layout from
the top menu bar. Note that the load multiplier for the first buckling mode is found to
be 0.78173.

Structural Analysis Chapter 8. Failure Analysis 36

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

To find the load required to buckle the structure, multiply the applied load by the load
multiplier. For example, the first buckling load will be 39.0865 MPa (0.78173 × 50
MPa), thus the applied pressure of 50 MPa will cause the specimen to buckle. In the
Graph window, you can play the buckling animation.

Structural Analysis Chapter 8. Failure Analysis 37

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

The following figures show the first three buckling mode shapes. The corresponding
load multipliers for the first, second, and third mode shapes are 0.78173, 2.0094,
and 5.7321, respectively.

Note that the max value in the total deformation plots is scaled to 1 when displaying
the buckling mode shapes. Here, the deformation plot is used for mode shape
visualization, with the actual values of deformation carrying no physical meaning.

Structural Analysis Chapter 8. Failure Analysis 38

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Homework 1

Structural Analysis Chapter 8. Failure Analysis 43

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Homework 2

Structural Analysis Chapter 8. Failure Analysis 44

 6/11/2021

Vietnam National University Ho Chi Minh City Faculty of Applied Science

University of Technology Department of Engineering Mechanics

Homework 3

Structural Analysis Chapter 8. Failure Analysis 45

 Chapter 6. STRUCTURAL VIBRATION AND DYNAMICS

HOMEWORK 1:

The following figure shows a simple plate made of structural steel with Young’s modulus

E = 200 GPa, Poisson’s ratio ν = 0.3, and density ρ = 7850 kg/m3. The plate has a thickness of

5 mm and is fixed on the left side. Suppose a harmonic force of magnitude 100 N is applied to

the right edge along the plate’s surface normal direction. Use a solid model and a shell model to

compute:

a. The first five natural frequencies and the corresponding normal modes

b. The frequency response of the z directional deformation (along the surface normal

direction of the plate) of the plate surface under the given harmonic load

Compare the results between the two models.

122
SOLVE:

Step 1:

Step 2:

123
Step 3:

124
125
126
127
128
 HOMEWORK 2:

The following clevis assembly consists of a yoke, a pin, and a u-shape. The assembly

components are made of structural steel with Young’s modulus E = 200 GPa, Poisson’s ratio ν

= 0.3, and density ρ = 7850 kg/m3. The profile sketches of the yoke and the u-shape are shown

below. Both components have an extrusion depth of 5 cm. The pin has a diameter of 2 cm and a

length of 16 cm, and is centered 2.5 cm away from both the front and the side faces of the u-

shape. Assume that the yoke is fixed on the left end, and the u-shape is applied a harmonic

pressure load of magnitude 100 N/cm2 on the right end.

Using the FEA, compute:

a. The first five natural frequencies and normal modes of the assembly

b. The frequency response of the x directional deformation (along the load direction) of the

cylindrical pin surface under the given harmonic load

129
SOLVE:

1.

2.

130
3.

4.

131
5.

6.

132
7.

8.

133
9.

10.

134
11.

12.

135
13.

14.

136
15.

137
 Chapter 8. THERMAL ANALYSIS

HOMEWORK 1

Dạng bài toán

159
Tạo mô hình

160
Chia lưới mô hình

Câu a:

Đặt điều kiện biên

161
162
Độ an toàn

Tuổi thọ

163
Câu b:

Điều kiện biên:

164
Độ an toàn

165
Tuổi thọ

166
HOMEWORK 2

Dạng bài toán

167
Tạo mô hình

Chia lưới mô hình

168
Điều kiện biên

169
Kết quả tổng chuyển vị

Kết quả ứng suất von-Mises

170
Độ an toàn

Tuổi thọ

171
172
173
HOMEWORK 3

Dạng bài toán

174
Tạo mô hình

Chia lưới cho mô hình

175
Đặt điều kiện biên

176
Kết quả tổng chuyển vị tổng

Kết quả ứng suất von-Mises

177
Độ an toàn

Tuổi thọ

178
179
 LÝ THUYẾT CUỐI KÌ TÍNH TOÁN KẾT CẤU (AS3013)

1. Tại sao trong một số trường hợp phân tích vật rắn, cần đưa về bài toán
phẳng? Hãy cho một số ví dụ.
Đáp án: Trong trường hợp tấm có chiều dày nhỏ, tải trọng và điều kiện biên đồng
phẳng, ta đưa về ứng suất phẳng. Trong trường hợp chiều dày lớn, tải trọng và điều kiện
biên đồng phẳng, ta đưa về biến dạng phẳng.
Ví dụ:
- Ứng suất phẳng:
+ Tấm kim loại mỏng, chịu tải trọng phân bố đều và đặt trong điều kiện đồng
phẳng.
+ Tấm cánh quạt mỏng được đặt trong điều kiện đồng phẳng và chịu tải trọng từ
luồng không khí.
- Biến dạng phẳng:
+ Tấm bê tông dày, đặt trong điều kiện đồng phẳng và chịu tải trọng.
+ Tấm thép có chiều dày lớn, được đặt trong điều kiện đồng phẳng và chịu tải trọng
từ một hệ thống cố định.

2. Giải thích sự khác nhau giữa phần tử tấm phẳng (plate) và phần tử tấm vỏ
(shell) mà anh/chị đã được học trong bài giảng.
Đáp án: Phần tử tấm phẳng chỉ có ứng xử uốn còn phần tử tấm vỏ vừa ứng xử
uốn, vừa chịu kéo và nén.

3. Hãy nêu sự liên quan giữa phân tích tần số riêng và phân tích dao động
điều hòa.
Đáp án: Phân tích dao động điều hòa tìm sự cộng hưởng khi tải điều hòa có tần số
trùng tần số riêng.

4. Giải thích sự khác nhau giữa truyền nhiệt ổn định (steady state) và truyền
nhiệt quá độ (transient).
 Đáp án: Truyền nhiệt ổn định không phụ thuộc thời gian còn truyền nhiệt quá độ
phụ thuộc vào thời gian.

5. Phân biệt lý thuyết dầm Euler và lý thuyết dầm Timoshenko.

Đáp án: Lý thuyết dầm Euler giả định các dầm cứng và bỏ qua biến dạng cắt và
biến dạng trái phương, trong khi lý thuyết dầm Timoshenko xem xét cả biến dạng cắt
và biến dạng trái phương, cho phép mô hình hóa các dầm mềm hơn. Việc lựa chọn giữa
hai lý thuyết này phụ thuộc vào tính chất và các yêu cầu cụ thể của vấn đề được nghiên
cứu.

6. Phân tích đáp ứng động lực học quá độ.

Đáp án: Phân tích đáp ứng động lực học quá độ (dynamic response analysis of
overloading) là quá trình nghiên cứu và đánh giá phản ứng của hệ thống cơ học khi chịu
một lực hoặc tải trọng vượt quá giới hạn mà hệ thống được thiết kế để chịu đựng.