6th Sem M&a LABmanual 15MEL68

ACHARYA INSTITUTE OF TECHNOLOGY
DEPARTMENT OF MECHANICAL ENGINEERING

Acharya Dr.Sarvepalli Radhakrishanan Marg,
Soldevanahalli, Hesarghatta Road, Bengaluru-107
LABORATORY MANUAL
MODELING AND ANALYSIS LAB (FEA)

(Subject Code: 15MEL68)
For SIXTH SEMESTER B.E – MECHANICAL
Prepared by
Pranesh K G. B.E., M.Tech., (Ph.D.)
Asst. Professor Grade-III
and
Hulluraiah H.
Instructor
Modeling and Analysis lab (FEA) ( 15MEL68)
Syllabus
Modeling and Analysis Lab (FEA)
[AS PER CHOICE ASED CREDIT SYSTEM (CBCS) SCHEME]
SEMESTER – VI
Subject Code 15MEL68 IA Marks 20
Number of Lecture Hrs / Week 01 Exam Marks 80
No of Practical Hours / Week 02 Exam Hours 03
CREDITS – 02
PART – A
Study of a FEA package and modeling and stress analysis of:
1. Bars of constant cross section area, tapered cross section area and stepped bar
2. Trusses – (Minimum 2 exercises of different types)
3. Beams – Simply supported, cantilever, beams with point load , UDL, beams with varying
load etc (Minimum 6 exercises different nature)
4. Stress analysis of a rectangular plate with a circular hole
PART - B
1) Thermal Analysis – 1D & 2D problem with conduction and convection boundary
conditions (Minimum 4 exercises of different types )
2) Dynamic Analysis to find
a) Fixed – fixed beam for natural frequency determination
b) Bar subjected to forcing function
c) Fixed – fixed beam subjected to forcing function
PART – C (only for demo and oral exam)

1) Demonstrate the use of graphics standards ( IGES, STEP etc ) to import the model from
modeler to solver
2) Demonstrate one example of contact analysis to learn the procedure to carry out contact
analysis.
3) Demonstrate at least two different type of example to model and analyze bars or plates
made from composite material
Scheme for Examination:

One Question from Part A - 32 Marks (08 Write up +24)
One Question from Part B - 32 Marks (08 Write up +24)
Viva-Voce - 16 Marks
Total 80 Marks
Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 1

Getting Started with ANSYS

Performing a Typical ANSYS Analysis
The ANSYS program has many finite element analysis capabilities, ranging from a simple, linear, static
analysis to a complex, nonlinear, transient dynamic analysis. The analysis guide manuals in the ANSYS
documentation set describe specific procedures for performing analyses for different engineering
disciplines.
A typical ANSYS analysis has three distinct steps:

i) Build the model.
ii) Apply loads and obtain the solution.
iii) Review the results.
Building a Model
Building a finite element model requires more of an ANSYS user's time than any other part of the analysis.
First, you specify a jobname and analysis title. Then, you use the PREP7 preprocessor to define the element
types, element real constants, material properties, and the model geometry.
Specifying a Jobname and Analysis Title

This task is not required for an analysis, but is recommended.
Defining the Jobname

The jobname is a name that identifies the ANSYS job. When you define a jobname for an analysis, the
jobname becomes the first part of the name of all files the analysis creates. (The extension or suffix for these
files' names is a file identifier such as .DB.) By using a jobname for each analysis, you insure that no files
are overwritten.
If you do not specify a jobname, all files receive the name FILE or file, depending on the operating system.
Command(s): /FILNAME
GUI: Utility Menu>File>Change Jobname
Defining Element Types The ANSYS element library contains more than 100 different element types. Each
element type has a unique number and a prefix that identifies the element category: BEAM4, PLANE77,
SOLID96, etc.
The element type determines, among other things:

i) The degree-of-freedom set (which in turn implies the discipline-structural, thermal, magnetic,
electric, quadrilateral, brick, etc.)
ii) Whether the element lies in two-dimensional or three-dimensional space
For example, BEAM4, has six structural degrees of freedom (UX, UY, UZ, ROTX, ROTY, ROTZ), is a line
element, and can be modeled in 3-D space. PLANE77 has a thermal degree of freedom (TEMP), is an eight-
node quadrilateral element, and can be modeled only in 2-D space.
Defining Element Real Constants

Element real constants are properties that depend on the element type, such as cross-sectional properties of
a beam element. For example, real constants for BEAM3, the 2-D beam element, are area (AREA), moment
of inertia (IZZ), height (HEIGHT), shear deflection constant (SHEARZ), initial strain (ISTRN), and added
mass per unit length (ADDMAS). Not all element types require real constants, and different elements of the
same type may have different real constant values.
As with element types, each set of real constants has a reference number, and the table of reference number
versus real constant set is called the real constant table. While defining the elements, you point to the
appropriate real constant reference number using the REAL command (Main Menu>
Preprocessor>Create>Elements>Elem Attributes).
Defining Material Properties

Most element types require material properties. Depending on the application, material properties may be:
 Linear or nonlinear
 Isotropic, orthotropic, or anisotropic
 Constant temperature or temperature-dependent
As with element types and real constants, each set of material properties has a material reference number.
The table of material reference numbers versus material property sets is called the material table. Within one
analysis, you may have multiple material property sets (to correspond with multiple materials used in the
model). ANSYS identifies each set with a unique reference number
Main Menu> Preprocessor> Material Props> Material Models
Creating the Model Geometry

Once you have defined material properties, the next step in an analysis is generating a finite element model-
nodes and elements-that adequately describes the model geometry.

There are two methods to create the finite element model: solid modeling and direct generation. With solid
modeling, you describe the geometric shape of your model, then instruct the ANSYS program to
automatically mesh the geometry with nodes and elements. You can control the size and shape of the
elements that the program creates. With direct generation, you "manually" define the location of each node
and the connectivity of each element. Several convenience operations, such as copying patterns of existing
nodes and elements, symmetry reflection, etc. are available
Apply Loads and Obtain the Solution
In this step, you use the SOLUTION processor to define the analysis type and analysis options, apply loads,
specify load step options, and initiate the finite element solution. You also can apply loads using the PREP7
preprocessor.
Applying Loads
The word loads as used in this manual includes boundary conditions (constraints, supports, or boundary
field specifications) as well as other externally and internally applied loads. Loads in the ANSYS program
are divided into six categories
 DOF Constraints
 Forces
 Surface Loads
 Body Loads
 Inertia Loads
 Coupled-field Loads
You can apply most of these loads either on the solid model (keypoints, lines, and areas) or the finite
element model (nodes and elements).
Two important load-related terms you need to know are load step and substep. A load step is simply a
configuration of loads for which you obtain a solution. In a structural analysis, for example, you may apply
wind loads in one load step and gravity in a second load step. Load steps are also useful in dividing a
transient load history curve into several segments.
Substeps are incremental steps taken within a load step. You use them mainly for accuracy and convergence
purposes in transient and nonlinear analyses. Substeps are also known as time stepssteps taken over a period
of time.

Initiating the Solution

To initiate solution calculations, use either of the following:
Command(s): SOLVE
GUI: Main Menu>Solution>Current LS
When you issue this command, the ANSYS program takes model and loading information from the database
and calculates the results. Results are written to the results file (Jobname.RST, Jobname.RTH,
Jobname.RMG, or Jobname.RFL) and also to the database. The only difference is that only one set of results
can reside in the database at one time, while you can write all sets of results (for all substeps) to the results
file.
Review the Results

Once the solution has been calculated, you can use the ANSYS postprocessors to review the results
GENERAL STEPS
Step 1: Ansys Utility Menu
File – clear and start new – do not read file – ok File – change job name – enter new job name – xxxx – ok
File – change title – enter new title – yyy – ok
Step 2: Ansys Main Menu – Preferences select – STRUCTURAL - ok
Step 3: Preprocessor Element type – select type of element from the table and the required options Real
constants – give the details such as thickness, areas, moment of inertia, etc. required depending on the
nature of the problem. Material Properties – give the details such as Young‟s modulus, Poisson‟s ratio etc.
depending on the nature of the problem.
Step 4: Modeling – create the required geometry such as nodes elements, area, volume by using the
appropriate options.
Step 5: Generate – Elements/ nodes using Mesh Tool if necessary (in 2D and 3D problems)
Step 6: Apply boundary conditions/loads such as DOF constraints, Force/Momentum, Pressure etc.
Step 7: Solution – Solve the problem
Step 8: General Post Processor – plot / list the required results.
Step 9: Plot ctrls – animate – deformed shape – def+undeformed-ok
Step 10: to save the solution ansys tool bar- save,,,,model

PART – A
Modeling and stress analysis of Bars of constant cross section area, tapered cross
section area and stepped bar
Exercise 1
Find Nodal displacement, reaction forces and axial stresses for the following problem using LINK180
element. [Use 2 Elements to model the bar] Given Data: E = 2 x 105 N/mm2.
SOLUTION:
1. File > change job name > Enter “Axial – Exercise 1”
2. ANSYS main menu > Preferences > structural > ok
3. ANSYS Main Menu > preprocessor > ELEMENT type > Add/edit/delete >add > link > 3D finit stn 180 >
Ok > Close.
4. ANSYS main menu > preprocessor >Real Constants > Add/edit/delete >Add > select Type 1 LINK180 >
Ok >Real constant Set No: = 1, cross sectional area = 200 > Ok > close.
5. ANSYS Main Menu > Preprocessor > Material Properties > Material Models > Single click on structural
> Single click on linear > Elastic >Isotropic > EX = 2E5; PRXY = 0.3 > Ok > Close.
6. ANSYS Main Menu > Preprocessor > Modeling > Create > Nodes > In
active CS > Set Node No: = 1, X = 0, Y = 0, Z = 0 > Apply Set Node No: = 2, X = 50, Y =0, Z = 0 > Apply
Set Node No: = 3, X = 100, Y = 0, Z = 0 > Ok.
7. ANSYS Main Menu > Preprocessor > Modeling > Create > Elements >Auto Numbered > Thru Nodes >
Pick node1 & node2 (with help of mouse)> Apply > Now Pick node2 & node3 > Ok. Come out of Modeling
8. ANSYS Main Menu > Preprocessor> Loads > Define loads > Apply >Structural > Displacements > On
Nodes > Pick Node 1 (Use Mouse) >Ok > Highlight All DOF (Fixed boundary Condition) > OK.
9. ANSYS Main Menu > Preprocessor > Loads > Define loads > Apply >Structural > Force/Moment > On
Nodes > Pick Node 3 > Ok > Select FX Apply as constant value and select value of Force/Moment = -1000
N (Force is along X axis and in Negative X direction).Come out of Preprocessor.

10. ANSYS Main Menu > Solution > Solve Current LS (Load Step) > Ok.
11. ANSYS Main Menu > General Postprocessor > Plot results > Contourplot > Nodal Solu > Single click
on DOF Solution > Highlight X –Component of displacement > Ok. [This gives the deformed shape of the
bar]
12. ANSYS Main Menu > General Postprocessor > List results > Nodal Solution > Single click on
DOF Solution > Highlight X – Component of displacement > Ok. [This gives the list of
nodal displacement values].
13. ANSYS Main Menu > General Postprocessor > List results > Reaction Solu > Highlight All items > Ok.
[This gives the reaction at the supports].
14. File > Save as > Select the user directory > Exercise-axial1 > Ok.
Results: Nodal Solution – Displacements
Node No. Ux Uy
Results: Reaction Solution
Node No Fx Fy
Results: Elemental Solution – Stresses
Element No. Stress

Exercise 2
Determine the Nodal displacement, Axial Stress, Strain in each element and Support reactions for the
following problem. The modulus of elasticity (E) of Aluminum as 69 GPa and Poisson‟s ratio as 0.3
1 2 3
2
3KN
A1=300mm 2 A2=150mm
400mm 200mm
SOLUTION:
1. File > change job name > Enter “Axial – Exercise 2”
Ok > Close.
4. ANSYS main menu > preprocessor > Real Constants > Add/edit/delete >Add > select Type 1 LINK180 >
Ok > Real constant Set No: = 1, cross sectional area = 300 > Apply >
Change real constant No: = 2 > Cross sectional area = 150 > Ok > Close.
> Single click on linear > Elastic >
Isotropic > EX = 69E3; PRXY = 0.3 > Ok > Close.
6. ANSYS Main Menu > Preprocessor > Modeling > Create > Nodes > Inactive CS > Set Node No: = 1, X
= 0, Y = 0, Z = 0 > Apply
Set Node No: = 2, X = 400, Y =0, Z = 0 > Apply
Set Node No: = 3, X = 600, Y = 0, Z = 0 > ok
Pick node1 & node2 (with help of mouse)> Apply > Now Pick node2 & node3 > Ok.
8. ANSYS Main Menu > Preprocessor > Modeling > Create > Elements >Element attributes > Set Element
type No. 1 LINK180
Set Material No. 1Set Real Constant set No: = 2 > Ok.
9. ANSYS Main Menu > Preprocessor > Loads > Define loads > Apply >Structural > Displacements > On
Nodes > Pick Node 1 (Use Mouse) > Ok> Highlight All DOF (Fixed boundary Condition) > OK.
Nodes > Pick Node 3 > Ok > Select FX Apply as constant value and select value of Force/Moment = 3000
N

on DOF Solution > Highlight X –Component of displacement > Ok. [This gives the deformed shape of the
bar]
13. ANSYS Main Menu > General Postprocessor > List results > Nodal Solution > Single click on DOF
Solution > Highlight X – Component of displacement > Ok. [This gives the list of nodal displacement
values].
14. ANSYS Main Menu > general postprocessor > Element Table > Define table > Add > Set user label for
item = STRESS, Select item, comp, results data item = by sequence Number – Select LS, 1 (Type 1 after
selecting LS) > Ok > Close.
15. ANSYS Main Menu > General postprocessor > Element table > List Element table > Select STRESS >
Ok > Note the stress in elements.
17. File > Save as > Select the user directory > Exercise-axial 2 > Ok.
Node No. Ux Uy
Element No. Stress
Node No Fx Fy

Exercise 3
For steel stepped bar shown in figure, Determine the Nodal displacement, Axial Stress, Strain in each
element and Support reactions. The modulus of elasticity of Steel as 200 GPa and Poisson‟s ratio as 0.3
1 2 3 4
60KN 75KN
A3 =600mm 2
A2 = 1200mm2
A1 = 2400mm 2
800mm 600mm 400mm
Exercise 4
For steel stepped bar shown in figure, Determine the Nodal displacement, Axial Stress, Strain in each
element and Support reactions. The modulus of elasticity of Steel as 200 GPa and Poisson‟s ratio as 0.3
A2 = 400 mm2
A1 = 200 mm2
1 2 3 4
20KN
200mm 200mm 250mm
Exercise 5
Determine the Nodal displacement, Axial Stress, Strain in each element and Support reactions for the
following problem. The modulus of elasticity (E) of Steel as 200 GPa and Poisson‟s ratio as 0.3
600 KN
E : 200 x 103 N/mm2
Area: 250 mm2
150 mm 150 mm
1.2 mm

Exercise 6
Consider the Tapered bar shown in figure below. Determine the Nodal Displacement,
Stress in each element, Reaction forces E = 2 x 105 N/mm2, Area at root, A1 = 1000 mm2, Area at the end,
A2 = 500 mm2.
Solution: The tapered bar is modified into 2 elements as shown below with modified area of cross section.
(A1 + A2)/2= (1000+500)/2=750 mm2
A1 = (1000+750)/2= 875 mm2
A2= (500+750)/2=625 mm2
L1 = 187.5 mm & L2 = 187.5 mm
1. Ansys Main Menu – Preferences-Select – STRUCTURAL- h method– ok

2. Element type – Add/Edit/Delete – Add – link, 3D Finit stn 180 – ok- close.
3. Real constants – Add – ok – real constant set no – 1 – cross-sectional AREA1 – 875 – apply-ok
4. Add – ok – real constant set no – 2 – cross-sectional AREA 2 – 625-ok
5. Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX – 2e5 –PRXY – 0.3
– ok – close.
6. Modeling – Create – keypoints– In Active CS, =0, Y=0 – Apply (first key point is created) – location in
active CS, X= 187.5, Y=0, apply (second key point is created) - location in active CS X=375, Y=0(third key
point is created) -ok.
7. Modeling-Create – lines-straight lines-pick key points 1 & 2-ok- pick key points 2 & 3-ok
8. Meshing-mesh attributes-picked lines (pick the lines)-ok-material no= 1, real constants set no = 1,
element type no =1, link 1, element section= none defined-pick the other line-ok-material number 2-define
material id 2- real constants set no = 2, element type no =2-element section= none defined-ok.
9. Meshing-size controls-manual size-lines-all lines- no of element divisions=10 (yes)-ok
10. Meshing-mesh tool-mesh-pick the lines-ok (the color changes to light blue)

11. Loads – Define loads – apply – Structural – Displacement – on key points- pick key point 1 – apply –
DOFs to be constrained – ALL DOF, displacement value=0 – ok.
12. Loads – Define loads – apply – Structural – Force/Moment – on key points- pick last key point – apply –
direction of For/Mom – FX – Force/Moment value – 1000 (+ve value) – ok.
13. Solve – current LS – ok (Solution is done is displayed) – close.
14. Element table – Define table – Add –„Results data item‟ – By Sequence num – LS – LS1 – ok.
15. Plot results – contour plot –Element table – item to be plotted LS,1, avg common nodes- yes average-
ok.
16. List Results – reaction solution – items to be listed – All items – ok (reaction forces will be displayed
with the node numbers).
17. Plot results- nodal solution-ok-DOF solution- x component of displacement-ok.
18. Animation: PlotCtrls – Animate – Deformed shape – def+undeformed-ok.
Node
Ansys Theoritiical
No. Ux Uy Ux Uy
Results: Elemental Solution – Stresses and Strains
Stress Strains
Element
No.
Ansys Theoritiical Ansys Theoritiical

Ansys Theoritiical
Node
No.
Fx Fx Fx Fx

Modeling and stress analysis of Trusses
TRUSSES
A truss is a structure comprising of one or more triangular units constructed with straight members whose
ends are connected at joints referred to as nodes. External forces and reactions to those forces are considered
to act only at the nodes and result in forces in the members which are either tensile or compressive forces.
In finite element analysis trusses are modeled using LINK elements only since link elements are meant to
take axial loads.
In ANSYS 14.0 trusses are modeled using LINK180 element. This is a 3D spar that is useful in a variety of
engineering applications. The element can be used to model trusses, sagging cables, links, springs, and so
on. The element is a uniaxial tension – compressive element with three degrees of freedom at each node:
translation in the nodal X, Y, and Z directions. As in pin jointed structure, no bending of the element is
considered. Plasticity, creep, rotation, large deflection, and large strain capabilities are included.
Exercise 7
Find Nodal displacement, Support reactions and Elemental stresses for the following Aluminum truss
problem using LINK180 element. E = 70 GPa, Poisson‟s ratio as 0.3 and Area = 200 mm2
12 KN
1 1 2
500 mm
300 mm
400 mm
SOLUTION:
1. File > change job name > Enter “Truss – Exercise 7”
Ok > Close.
4. ANSYS main menu > preprocessor > Real Constants > Add/edit/delete >Add > select Type 1 LINK180 >
Ok > Real constant Set No: = 1, cross sectional area = 200 > Ok.
> Single click on linear > Elastic >Isotropic > EX = 70e3; PRXY = 0.3 > Ok > Close.

6. ANSYS Main Menu > Preprocessor > Modeling > Create > Nodes > Inactive CS > Set Node No: = 1, X
= 0, Y = 0, Z = 0 > Apply
Set Node No: = 2, X = 500, Y =0, Z = 0 > Apply
Set Node No: = 3, X = 900, Y = -300, Z = 0 > Ok.
Pick node1 & node2 (with help of mouse)> Apply > Now Pick node2 & node3 > Ok.
Nodes > Pick Node 1& Node 3 (Use Mouse) > Ok > Highlight All DOF (Fixed boundary Condition) > OK.
Nodes> Pick Node 2 > Ok > Select FY Apply as constant value and select value of Force/Moment= -12e3 N
on DOF Solution > Highlight Displacement vector sum > Ok.
12. ANSYS Main Menu > General Postprocessor > List results > Contour plot> Nodal Solu > Single click
on DOF Solution > Highlight Displacement vector sum > Ok.[Note down the nodal displacement of each
node]
Node No. Ux Uy
Element No. Stress

Node No Fx Fy
Exercise 8
Find Nodal displacement, Support reactions and Elemental stresses for the following Steel truss problem
using LINK180 element. E = 200 x 103 N/mm2, Poisson‟s ratio as 0.3 and Area A1 = 2000 mm2,
A2 = 2000 mm2, A3 = 1500 mm2
150 KN
400 mm
2
1
1 3 3
400 mm 400 mm
Exercise 9
using LINK180 element. E = 200 x 103 N/mm2, Poisson‟s ratio as 0.3 and Area = 250 mm2,
450 mm 450 mm 350 mm
1 3 4
1
600 mm
2 3
18 KN

Exercise 10
using LINK180 element. E = 200 x 103 N/mm2, Poisson‟s ratio as 0.3 and Area = 1000 mm2
400 mm
2
m
m
90° 50 KN
0
40
1
45°
Exercise 11
using LINK180 element. E = 200 x 103 N/mm2, Poisson‟s ratio as 0.3 and Area = 1000 mm2,
50 KN 50 KN
400 mm 400 mm
300 mm
200 mm 400 mm 200 mm

Exercise 12
using LINK180 element. E = 70 x 109 N/m2, Poisson‟s ratio as 0.3 and Area = 0.1 m2
2
1m
1 3 3
1m 1000 N

Modeling and stress analysis of Beams

BEAMS
Beams are structural members that carry transverse load i.e. this type of loads produce bending effect. The
members are loaded perpendicular to the axis of the member that bends the structural member. Examples
include, structural member that connects two pillars, trees can also be considered as beam since it take
transverse wind loads, wing of an aircraft, construction cranes etc.
In finite element analysis [FEA] beams are modeled usingBEAM188/BEAM189 elements since BEAM
elements are meant to take transverse loads.
In ANSYS 14.0 structural beams are modeled using BEAM188 element. It is suitable for analyzing slender
to moderately stubby /thick beam structures. The element is based on Timoshenko beam theory which
includes shear –deformation effects. The element provides options for unrestrained warping of cross –
sections.
The element is a linear, quadratic, or cubic two – node beam element in 3D.BEAM188 has six or seven
degrees of freedom at each node. These include translations in the x, y, and z directions and rotations about
the x, y, and z directions. A seventh degree of freedom (warping magnitude) is optional. This element is
well – suited for linear, large rotation, and/or large strain nonlinear applications.
Exercise 13
A cantilever beam of rectangular cross section is shown in Figure, the width of beam is 0.10466 m, height
is 0.20932 m and length is 5 m take E = 200 x 109 N/m and Poisson‟s ratio is 0.3. A load of 50 KN is
applied at the free end of the cantilever. Determine
1. Nodal displacements at end load.
2. Shear Force & Bending Moment
3. Draw the Shear Force Diagram & Bending Moment Diagram.
4. Max. Deflection.
50 KN
b = 0.10466 m
1 2 h h = 0.20932 m
E = 200 x 109 Pa
5m
b
SOLUTION:
1. File > change job name > Enter “Beams – Exercise 13”
3. ANSYS Main Menu > preprocessor > ELEMENT type > Add/edit/delete >add > Beam > 2 node 188 >
Ok > Close.
4. ANSYS main menu > preprocessor > Sections > Beam > Common Sections > In the popup menu enter
the cross section details of the beam> OK.

> Single click on linear > Elastic >Isotropic > EX = 2 e11; PRXY = 0.3 > Ok > Close.
6. ANSYS Main Menu > Preprocessor > Modeling > Create > Keypoints > Inactive CS > Set Keypoint No:
= 1, X = 0, Y = 0, Z = 0 > Apply Set Keypoint No: = 2, X = 5, Y =0, Z = 0 > Ok.
7. ANSYS Main Menu > Preprocessor > Modeling > Create >Lines > Lines > Pick Keypoint 1 and
Keypoint 2 > Ok.
8. ANSYS Main Menu > Preprocessing > Meshing> Size Cntrls > Manual Size> Lines > pick Lines> Enter
0.1 into the Element edge length field.> OK
9. ANSYS Main Menu > Preprocessing > Meshing > Mesh> Lines> > Pick line
Keypoints > Pick Keypoint 1 (Use Mouse) > Ok > Highlight All DOF (Fixed boundary Condition) > Ok.
Keypoints > Pick Keypoint 2 (Use Mouse) > Ok > Select FY. Apply as constant value and select value of
Force/Moment = -50e3 N.
node]
16. Element table – Define table – Add – „Results data item‟ – By Sequence num –
SMISC –SMISC, 6 – apply, By Sequence num – SMISC – SMISC, 19 – apply, By
Sequence num –SMISC – SMISC, 3 – apply, By Sequence num – SMISC – SMISC,
16 – ok – close.
17. Plot results – contour plot – Line Element Results – Elem table item at node I –
SMIS6 – Elem table item at node J – SMIS19 – ok (Shear force diagram will be
displayed).
SMIS3 – Elem table item at node J – SMIS16 – ok (bending moment diagram will be
displayed).

Results: Deflection at the Keypoints
Key point No. Ux Uy Uz

1
2
Node No. Fx Fx My Mz
1
2
Exercise 14
A Beam fixed at both ends of circular cross section is shown in Figure, the diameter of beam is 0.1 m
and length is 6 m, take E = 200 x 109 Pa and Poisson‟s ratio is 0.3. A load of 50 KN is applied at the
centre of the beam. Determine
1. Nodal displacements
4. Max. Deflection.
50 KN
1 2 0.1 m
3
9
E = 200 x 10 Pa
3m 3m
Exercise 15
A beam of rectangular cross section is shown in Figure, the width of beam is 0.04949 m, height is
0.09898 m and length is 2 m take E = 200 x 109 Pa and Poisson‟s ratio is 0.3. A Uniformly Distributed
load (UDL) of 12 KN/m is applied at the end of the beam on Roller support. Determine
4. Max. Deflection.
12 KN/m
b = 0.04949 m
1 2 3
h h = 0.09898 m
9
E = 200 x 10 Pa
1m 1m
b
Exercise 16
A Cantilever beam of rectangular cross section is shown in Figure, the width of beam is 0.1m, height is
0.2 m and length is 2 m, take E = 200 x 109 Pa and Poisson‟s ratio is 0.3. A end load of 2 KN and a
moment load of 1 KN-m is applied at the end of Cantilever beam. Determine

4. Max. Deflection.
2 KN
b = 0.1 m
1 KN-m h h = 0.2 m
2 E = 200 x 10 9 Pa
1
b
2m
Exercise 17
A Simply supported beam of T shape in cross section is shown in Figure, length is 1100 mm take
E = 70 x 103 Pa and Poisson‟s ratio is 0.3. A UDL of 1 KN/mm is applied at one end and the Inclined
Load of 1 KN at an angle of 300 as shown in Fig. Determine
4. Max. Deflection.
1 KN/mm
20 mm
1000 N
200 mm
30°
1 2 3 4
250 mm
400 mm 400 mm 300 mm
10 mm
E=70 X 10 3 Pa
1. Ansys Main Menu – Preferences select – STRUCTURAL – ok

2. Element type – Add/Edit/Delete – Add – BEAM – 2node 188 – ok – close.
3. Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX
– 70e3– PRXY – 0.3 –ok – close.
4. Sections-Beams-common sections- sub type- T-section - enter the values-ok.
5. ANSYS Main Menu > Preprocessor > Modeling > Create > Keypoints > Inactive CS > Set Keypoint No:
= 1, X = 0, Y = 0, Z = 0 > Apply Set Keypoint No: = 2, X = 400, Y =0, Z = 0 > apply> Set Keypoint No: =
3, X = 800, Y =0, Z = 0 > apply> Set Keypoint No: = 4, X = 1100, Y =0, Z = 0 > ok
7. ANSYS Main Menu > Preprocessor > Modeling > Create >Lines > Lines > Pick Keypoint 1 and 2, 2 and
3, 3and 4 > Ok.
8. ANSYS Main Menu > Preprocessing > Meshing> Size Cntrls > Manual Size> Lines > pick Lines> Enter
0.1 into the Element edge length field.> OK
9. ANSYS Main Menu > Preprocessing > Meshing > Mesh> Lines> > Pick line
Keypoints > Pick Keypoint 1 and (Use Mouse) > Ok > Highlight UX,UY,UZ,ROTX,ROTY (simply
supported boundary Condition) > Ok.

11. ANSYS Main Menu > Preprocessor > Loads > Define loads > Apply >Structural > pressure > On beam
> Pick line (Use Mouse) > Ok > set load key 2> enter pressure value 1000>ok
12. Ansys main menu>modeling>create>node>rotate node>by angle>pick keypoint no3>enter angle of -
60o>ok
ANSYS Main Menu > Preprocessor > Loads > Define loads > Apply >Structural > force > On node > Pick
rotated node (Use Mouse) > Ok > enter force(FY) value 1000>ok
node]
17. Element table – Define table – Add – „Results data item‟ – By Sequence num –
SMISC –SMISC, 6 – apply, By Sequence num – SMISC – SMISC, 19 – apply, By
Sequence num –SMISC – SMISC, 3 – apply, By Sequence num – SMISC – SMISC,
16 – ok – close.
SMIS6 – Elem table item at node J – SMIS19 – ok (Shear force diagram will be
displayed).
SMIS3 – Elem table item at node J – SMIS16 – ok (bending moment diagram will be
displayed).
Results: Deflection at the Keypoints
Keypoint No. Ux Uy Uz
1
2
Node No. Fx Fx My Mz
1
2

Exercise 18
A simply supported beam of I shape in cross section is shown in Figure, the length is 10 m take E =
200 x 109 Pa and Poisson‟s ratio is 0.3. A Uniformly Distributed Load of 40 KN/m is applied
throughout the beam. Determine
4. Max. Deflection.
0.02
40 KN/m
0.4
1 2 0.01
10 m
E=200 X 109 Pa 0.2
0.02

Stress analysis of a rectangular plate with a circular hole
PLANE 182 (Quad 4 node 182) is used for 2D modeling of solid structures. The element can be used either
as a plane element (Plane stress or Plane strain) or as an axisymmetric element. Four nodes having two
degrees at each node defines the element translations in the nodal X and Y directions. The element has
plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities. An option is
available to suppress the extra displacement shapes
PLANE 182 Geometry
PLANE 182 Input Summaries
Nodes I, J, K, L
Degrees of Freedom UX, UY
Real Constants THK – Thickness (Used only if KEYOPT(3) = 1)

HGSTF – Hourglass stiffness scaling factor
Materials Properties EX – Young‟s Modulus
PRXY – Poison‟s Ratio
DENS – Density
Surface loads Pressures
Body Loads Temperatures
Body force densities

Excersice 19
A steel plate with a hole is shown below. The plate is subjected to stresses along X direction. Determine the
stress distribution and maximum deflection.
Max. Max.
Sl W a Thickness a/W
Nominal
L σ (N/mm2) Stress Stress Kσ
Stress
No (mm) (mm) h (mm) Ratio
(mm) (Theory) (ANSYS)
1 100 150 10 5 σx =
1000
2 100 150 20 10 σ x = 800
1. Ansys Main Menu – Preferences-Select – STRUCTURAL-h method – ok

2. Element type – Add/Edit/Delete – Add – Solid – Quad 4 node – 182 – ok – option –
element behavior K3 – Plane stress with thickness – ok – close.
3. Real constants – Add – ok – real constant set no – 1 – Thickness – 5 – ok.
4. Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX – 2e5 –PRXY – 0.3
– ok – close.
5. Modeling –Create – Area – Rectangle – by dimensions – X1, X2, Y1, Y2 – 0, 150, 0, 100 – ok.
6. Create – Area – Circle – solid circle – X, Y, radius – 75, 50, 5 – ok.
7. Operate – Booleans – Subtract – Areas – pick area which is not to be deleted (rectangle) – apply – pick
area which is to be deleted (circle) – ok.
8. Meshing – Mesh Tool – Mesh Areas – Quad – Free – Mesh – pick all – ok. Mesh Tool – Refine – pick all
– Level of refinement – 3 – ok.
9. Loads – Define loads – apply – Structural – Displacement – on Nodes – select box – drag the left side of
the area – apply – DOFs to be constrained – ALL DOF – ok.
10. Loads – Define loads – apply – Structural – pressure – on Nodes – select box – drag the right side of the
area – apply – value – 1000 (+ve value) – ok.


12. Deformed shape-Plot Results – Deformed Shape – def+undeformed – ok.
13. Plot results – contour plot – Element solu – Stress – Von Mises Stress – ok (the stress
distribution diagram will be displayed).
Results
Ansys Theoretical
Deformation
Stress
Excersice 17
A steel plate with a hole is shown below. The plate is subjected to stresses along X direction and Y
directions. Determine the maximum stress and compare it with the theoretical value.
Thickn Max. Max.

Sl W a ess a/W Nomin
L σ (N/mm2) Stress Stress al Kσ
No (mm) (mm) h Ratio Stress
(mm) (mm) (Theory) (ANSYS)
1 100 150 10 5 σ x = 1000

σ y = 800
2 100 150 20 10 σ x = 800

σ y = 1000

Excersice 18
A steel plate as shown in the figure below is subjected to axial load along X direction. Determine the
stresses at critical locations and compare it with the theoretical value.
a/W Max.
Sl W a Thickness Max. Stress Kσ
Load Stress
L Rati ( KN) Nominal
No (mm) (mm) h (mm) (ANSYS) (DHB)
(mm) o (Theory) Stress
1 25 40 3, 5, 10 15 20
Exercise 22
A plate, 10 mm thick, subjected to a tensile load of 20 KN as shown in figure. Determine the stress
concentration factor and compare it the theoretical values using design data handbook.
Fillet
Sl Thickness D/d Max. Stress Max. Stress Nominal Kσ
Radius Load
( KN) Stress
No h (mm) Ratio (Theory) (ANSYS) (DHB)
r (mm)
1 7.5 10 20

PART – B
THERMAL ANALYSIS
Exercise 23
Solve the 2D heat conduction problem for the temperature distribution within the rectangular plate. Thermal
conductivity of the plate, Kxx = 401 W/m-K. Also find the temperature at the midpoint of the plate.
1. Ansys Main Menu – Preferences-select – THERMAL- h method– ok

2. Element type – Add/Edit/Delete – Add – Solid – Quad 4 node – 55 – ok – option – Element behavior K3
– Plane stress with thickness – ok – close.
3. Material Properties – material models – Thermal – Conductivity – Isotropic – KXX – 401.
4. Modeling – Create – Area – Rectangle – by dimensions – X1, X2, Y1, Y2 – 0, 10, 0, 20 – ok.
5. Meshing – Mesh Tool – Mesh Areas – Quad – Free – Mesh – pick all – ok. Mesh Tool – Refine – pick all
– Level of refinement – 3 – ok.
6. Loads – Define loads – apply – Thermal – Temperature – on Lines – select 1000 C
lines – apply – DOFs to be constrained – TEMP – Temp value – 1000 C – ok.
7. Loads – Define loads – apply – Thermal – Temperature – on Lines – select 2000 C
lines – apply – DOFs to be constrained – TEMP – Temp value – 2000 C – ok.
9. Read results-last set-ok
10. List results-nodal solution-select temperature-ok
11. Observe the nodal solution per node.
12. From the menu bar-plot ctrls-style-size and shape-display of the element-click on real constant
multiplier = 0.2, don‟t change other values-ok.

13. Plot results-contour plot-nodal solution-temperature-deformed shape only-ok

14. Element table-define table-add-enter user label item=HTRANS, select by sequence no
SMISC, 1 - ok-close.
15. Element table-list table-select HTRANS-ok
Results: Temperature at the midpoint of the palte
Node No Temperature in 0C
Exercise 24
For 2D stainless – steel shown below, determine the temperature distribution. The left and right sides are
insulated. The top surface is subjected to heat transfer by convection. The bottom and internal portion
surfaces are maintained at 3000C. Thermal conductivity of stainless steel = 16 W/m K.

Exercise 25
An insulated wall is constructed of three homogeneous layers as shown in figure. Under steady state
conditions, temperature of media in contact at the left and right surfaces and the respective film coefficients
are shown in the figure. Find the Temperatures at the two surfaces and also at interfaces. Also compare heat
transfer per unit area through the wall.
T’ = 30 0C
T’ = 100 0C k1 = k2 = k3 = h2= 20 W/m2
0
h1 = 15 C
40 35 60
W/m2 0C
W/m0C W/m0C W/m0C
50 70 mm 50 mm
mm
Exercise 26
Determine the nodal temperature distribution. Assume that the heat generated inside
the steel container is 400 0C. Steel thermal conductivity of 20 W/m K. The fins are made
of aluminum with thermal conductivity of 180 W/m K.
Boundary Conditions: There is convection along all boundaries except the bottom, which
is insulated. The film coefficient is 50 W/m2 0C and Bulk temperature is 200C.
Steel k1 = 20 W/m K
Al k2 =180 W/m K
T’ = 20 0C
h1 = 50 W/m2 0C
Temp 400 0C

Exercise 27
A pipe carrying hot fluid with 200 mm internal diameter and 100 mm thick is covered
with a layer of Insulation 80 mm thick. The thermal Conductivities of the pipe and
insulation are 40 W/m K and 0.75 W/m K respectively.
The outside heat transfer coefficient is 50 W/m2 K. If the Temperature of inner Surface
of the pipe is 300 0C and ambient Temperature is 25 0C. Find the Heat Transfer per
unit length of the Pipe and Temperature variation across the pipe and Insulation.
1. Ansys Main Menu – Preferences-select THERMAL- h method – ok

2. Preprocessor - Element type – Add/Edit/Delete – Add – SOLID – Quad 4 node 55–
ok- close.
3. Material Properties – material models – Thermal – Conductivity – Isotropic – KXXX–
40 – ok, Material - Add New Model – Define Material ID – 2 – ok- Click on Isotropic
– KXXX– 0.75 – ok, - close
4. Modeling – Create – Area-Circle-Annulus – WP X=0, WP Y=0, Rad 1 = 0.1, Rad 2 =
0.2, click apply, WP X=0, WP Y=0, Rad 1 = 0.2, Rad 2 = 0.28 - OK
5. Operate – Booleans-Glue – Areas – Pick all.
6. Meshing – Mesh Attributes – Default Attributes – Material No = 1 OK
7. Mesh Tool-Smart Size – Fine – Click on Mesh- Select Area No 1 (On screen) Ok - Ok
8. Mesh Attributes – Default Attributes – Select Material No = 2 - OK.
9. Mesh Tool-Smart Size – Fine – Click on Mesh- Select Area No 2 (Click on screen
Select next) Ok – Ok
10. PlotCtrl-Numbering – Tick on Line Number and Area Numbers-ok
11. Plot - Lines

12. Loads – Define Loads – Apply – Thermal - Temperature – On Lines – Pick inside
circle Lines (4 colored lines) Ok- - DOFs to be constrained - Temp – Load Temp
value =300 -ok
13. Convection - on Lines – Click Outside Circle (4 colored lines) – ok – enter Film
Coefficient = 50 and Bulk Temperature = 25
15. General Post Processor – Plot Results-Countour Plot-Nodal Solu-DOF Solution-
Nodal Temperature -ok
16. Click on Report Generator – Save Image

DYNAMIC ANALYSIS ( Modal Analysis )

Exercise 28
Modal analysis of cantilever beam for different mode shape and natural frequency
determination. Modulus of elasticity = 200 Gpa, Density = 7800 Kg/m3.
1. Ansys Main Menu – Preferences-select – STRUCTURAL- h method – ok

2. Element type – Add/Edit/Delete – Add – BEAM – 2 node 188– ok- close.
3. Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX
– 200e9– PRXY – 0.27 – Density – 7800 – ok – close.
4. Sections-Beams-common sections- sub type- rectangle (1st element) - enter b=0.01,
h=0.01- preview-ok.
5. Modeling – Create – Keypoints – in Active CS – x,y,z locations – 0,0 – apply – x,y,z
locations –1,0 – ok (Keypoints created).
6. Create – Lines – lines – in Active Coord – pick keypoints 1 and 2 – ok.
7. Meshing – Size Cntrls – Manual Size – Lines – All Lines – element edge length – 0.1
– ok. Mesh– Lines – Pick All – ok.
8. Solution – Analysis Type – New Analysis – Modal – ok.
9. Solution – Analysis Type – Subspace – Analysis options – no of modes to extract – 5
– no of modes to expand – 5 – ok – (use default values) – ok.
10. Solution – Define Loads – Apply – Structural – Displacement – On Keypoints – Pick
First keypoint – apply – DOFs to be constrained – ALL DOF – ok.
12. Result Summary
13. Read Results – First Set
14. Plot Results – Deformed Shape – def+undeformed – ok.
15. PlotCtrls – Animate – Deformed shape – def+undeformed-ok.
16. Read Results – Next Set
17. Plot Results – Deformed Shape – def+undeformed – ok.
18. PlotCtrls – Animate – Deformed shape – def+undeformed-ok

Results: Modal Frequencies of the beam
Mode No Frequency in Hz Mode Shape
Exercise 29
Modal analysis of Fixed fixed beam for different mode shape and natural frequency
determination. Modulus of elasticity = 200 Gpa, Density = 7800 Kg/m3.
Results: Modal Frequencies of the beam

Mode No. Frequency in Hz Mode Shape
1
2
3
4
5

Exercise 30
Bar subjected to forcing function: Harmonic analysis
Consider a beam shown in figure below. Conduct a harmonic forced response test by
applying a cyclic load 100 N (Harmonic) at the free end of the beam. The frequency of the
load will be varied from 0 – 100 Hz. Modulus of elasticity = 200 Gpa,Poisson ratio =0.3,
Density = 7800 Kg/m3.
Results: Frequency v/s Amplitude Plot
1. Ansys Main Menu – Preferences-select – STRUCTURAL- h method – ok

2. Preprocessor Element type – Add/Edit/Delete – Add – BEAM – 2 node 188– ok-
close.
3. Material Properties – material models – Structural – Linear – Elastic – Isotropic –
EX– 200e9– PRXY – 0.27 – Density – 7800 – ok – close.
4. Sections-Beams-common sections- sub type- rectangle (1st element) - enter b=0.01,
h = 0.01- preview-ok.
5. Modeling – Create – Keypoints – in Active CS – x, y, z locations – 0,0 – apply – x,y,z
locations –1.2, 0 – ok (Keypoints created).
6. Create – Lines – lines – in Active Coord – pick keypoints 1 and 2 – ok.
7. Meshing – Size Cntrls – Manual Size – Lines – All Lines – element edge length – 0.1
– ok. Mesh– Lines – Pick All – ok.
8. Solution – Analysis Type – New Analysis – HORMONIC – ok.
9. Solution –Load Step Options – Time/ Frequency – Freq and Substeps
Hormonic freq range 0 to 100
Number substeps 100 – Click on Stepped - OK

10. Solution – Define Loads – Apply – Structural – Displacement – On Keypoints – Pick

First keypoint – apply – DOFs to be constrained – ALL DOF – ok.
11. For Cyclic Load - Force/Moment - On Keypoints – Pick Last keypoint – OK –
select FY – Real part of Force/Mom = -100 – ok
13. Result Summary -
14. Time History Postprocessor.
Click on ADD DATA

-Nodal Solution –DOF solution
Click on y-Component of displact
On the Screen Click on Node 2 –
OK – then Click on GRAPH

To Generate Graph - click on Report Generator Show the path to save file - Append – OK - Capture Image
1. Result Summary -

2. Time History Postprocessor.
Click on ADD DATA

-Nodal Solution –DOF solution
Click on y-Component of displact
On the Screen Click on Node 2 –
OK – then Click on GRAPH

To Generate Graph - click on Report Generator Show the path to save file - Append – OK - Capture Image

To Zoom the Graph

PlatCtrls – Style – Graph – Click on Modify Axes-In Y-Axes Scale Change from Linear to Logirthemic-OK
click on Report Generator Show the path to save file - Append – OK - Capture Image
This is the response at node 2 for the cyclic load 100 N applied at this node from 0 - 100 Hz

6th Sem M&a LABmanual 15MEL68

Uploaded by

Copyright:

Available Formats

6th Sem M&a LABmanual 15MEL68

Uploaded by

Document Information

Original Description:

Copyright

Available Formats

Share this document

Share or Embed Document

Sharing Options

Did you find this document useful?

Is this content inappropriate?

Copyright:

Available Formats

6th Sem M&a LABmanual 15MEL68

Uploaded by

Copyright:

Available Formats

ACHARYA INSTITUTE OF TECHNOLOGY

DEPARTMENT OF MECHANICAL ENGINEERING

MODELING AND ANALYSIS LAB (FEA)

PART – C (only for demo and oral exam)

Scheme for Examination:

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 1

Getting Started with ANSYS

A typical ANSYS analysis has three distinct steps:

ii) Apply loads and obtain the solution.

iii) Review the results.

Specifying a Jobname and Analysis Title

Defining the Jobname

GUI: Utility Menu>File>Change Jobname

The element type determines, among other things:

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 2

ii) Whether the element lies in two-dimensional or three-dimensional space

Defining Element Real Constants

Defining Material Properties

 Isotropic, orthotropic, or anisotropic

 Constant temperature or temperature-dependent

Main Menu> Preprocessor> Material Props> Material Models

Creating the Model Geometry

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 3

Apply Loads and Obtain the Solution

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 4

Initiating the Solution

GUI: Main Menu>Solution>Current LS

Review the Results

Step 2: Ansys Main Menu – Preferences select – STRUCTURAL - ok

Step 7: Solution – Solve the problem

Step 8: General Post Processor – plot / list the required results.

Step 9: Plot ctrls – animate – deformed shape – def+undeformed-ok

Step 10: to save the solution ansys tool bar- save,,,,model

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 5

1. File > change job name > Enter “Axial – Exercise 1”

2. ANSYS main menu > Preferences > structural > ok

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 6

Results: Nodal Solution – Displacements

Results: Reaction Solution

Results: Elemental Solution – Stresses

Element No. Stress

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 7

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 8

Results: Nodal Solution – Displacements

Results: Elemental Solution – Stresses

Element No. Stress

Results: Reaction Solution

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 9

800mm 600mm 400mm

200mm 200mm 250mm

Area: 250 mm2

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 10

1. Ansys Main Menu – Preferences-Select – STRUCTURAL- h method– ok

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 11

Results: Nodal Solution – Displacements

Results: Elemental Solution – Stresses and Strains

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 12

Results: Reaction Solution

Department of Mechanical Engg, Acharya Institute of Technology, Bengaluru -107 13