SEMBODAI RUKMANI VARATHARAJAN ENGINEERING

COLLEGE
SEMBODAI, VEDARANIAM [T.K],
NAGAPATTINAM [Dist] -614809,

DEPARTMENT OF CIVIL ENGINEERING

2021-2022

ST4211 - NUMERICAL AND FINITE ELEMENT ANALYSIS

LABORATORY

NAME

REG.NO

BRANCH

YEAR SEMESTER
 SEMBODAI RUKMANI VARATHARAJAN
ENGINEERING COLLEGE,
SEMBODAI- 614809, VEDARANYAM-TK, NAGAPATTINAM -DT

BONAFIDE CERTIFICATE

This is to certify that Bonafide Record of work done

by Selvan /Selvi. ___________________________________________
in the ______________________________________________________
Practical Class of this Institution during the academic
year ____________________________

Internal
Register No. Assessment
Marks

Staff In-charge Head of the Department

Examination held on .............................................................

Internal Examiner External Examiner

 TABLE OF CONTENT

EXP. TITLE PAGE MARKS SIGN

NO. NO.
Ex No: 01 STUDY OF BASICS IN ANSYS
Date :

Aim:
To study about the basic procedure to perform the analysis in 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. The next few sections of this chapter cover general steps that are common
to most analyses.

A typical ANSYS analysis has three distinct steps:

1.Build the model.

2.Apply loads and obtain the solution.
3.Review the results.

Build the model:

1. Defining the Job name:
The job name is a name that identifies the ANSYS job. When you define a jobname for an analysis,
the job
name 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
ensure
that no files are overwritten.
2. Defining an Analysis Title:
The TITLE command (Utility Menu> File> Change Title), defines a title for the
analysis.ANSYS
includes the title on all graphics displays and on the solution output. You can issue the /STITLE
command to add subtitles; these will appear in the output, but not in graphics displays.
3. Defining Units:
The ANSYS program does not assume a system of units for your analysis. Except inmagnetic field
analyses,
you can use any system of units so long as you make sure that you use that system for all the data you
enter. (Units must be consistent for all input data.)
4. Defining Element Types:
The ANSYS element library contains more than 150 different element types. Each element type has a
unique number and a prefix that identifies the element category: BEAM4, PLANE77, SOLID96, etc.
The following element categories are available:

CONTACT PLANE

FLUID PRETS (Pretension)

HF (High Frequency) SHELL

HYPERelastic SOLID

INFINite SOURCe

INTERface SURFace

LINK TARGEt

MASS TRANSducer

MATRIX USER

VISCO elastic (or viscoplastic)

The element type determines, among other things:
The degree-of-freedom set (which in turn implies the discipline - structural, thermal,magnetic, electric,
quadrilateral, brick, etc.)Whether the element lies in 2-D or 3-D space.
4. 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.
6. Defining Material Properties:
Most element types require material properties. Depending on the application, material properties can
be linear (see Linear Material Properties) or nonlinear (see Nonlinear Material Properties).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.
7. 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. The graphic below shows
some sample finite element models.
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 in the
elements that the program creates. With direct generation, you "manually"define the
location of each node and the connectivity of each element.Several conveniences operations, such as
copying patterns of existing nodes and elements, symmetry reflection, etc. are available.
Sample Finite Element Models
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.
1. Defining the Analysis Type and Analysis Options:
You choose the analysis type based on the loading conditions and the response you wish to calculate.
For example, if natural frequencies and mode shapes are to be calculated, you would choose a modal
analysis. You can perform the following analysis types in the ANSYS program: static (or steady-state),
transient, harmonic, modal, spectrum, buckling, and sub structuring. Not all analysis types are valid for
all disciplines. Modal analysis, for example, is not valid for a thermal model. The analysis guide
manuals in the ANSYS documentation set describe the analysis types available for each discipline and
the procedures to do those analyses. Analysis options allow you to customize the analysis type. Typical
analysis options are the method of solution, stress stiffening on or off, and Newton-Raphson options.
2. Applying Loads
The word loads as used in ANSYS documentation 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).
3. Specifying Load Step Options:
Load step options are options that you can change from load step to load step, such as number of
substeps, time at the end of a load step, and output controls. Depending on the type of analysis you are
doing, load step options may or may not be required. The analysis procedures in the analysis guide
manuals describe the appropriate load step options as necessary.

4. Initiating the Solution:

To initiate solution calculations, use either of the following:
Command(s): SOLVE
GUI:Main Menu> Solution & gt; Solve> Current
LS Main Menu & gt; Solution & gt; solution method
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 (Job name.RST, Job name.
RTH, Job name. RMG, or Job name. 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
sub steps) to the results file.
Review the Results:
Once the solution has been calculated, you can use the ANSYS postprocessors to review the results.
Two postprocessors are available: POST1 and POST26.
You use POST1, the general postprocessor, to review results at one sub step (time step) over the entire
model or selected portion of the model. The command to enter POST1 is /POST1 (Main Menu & gt;
General Post proc), valid only at the Begin level. You can obtain contour displays, deformed shapes,
and tabular listings to review and interpret the results of the analysis. POST1 offers many other
capabilities, including error estimation, load case combinations, calculations among results data, and
path operations. You use POST26, the time history postprocessor, to review results at specific points in
the model over all time steps. The command to enter POST26 is /POST26 (Main Menu> Time Hist
Postpro), valid only at the Begin level. You can obtain graph plots of results data versus time (or
frequency) and tabular listings. Other POST26 capabilities include arithmetic calculations and complex
algebra.

Result:
Thus the basic steps to perform the analysis in ANSYS like
Build the model.
Apply loads and obtain the solution.
Review the results. are studied.
EX.NO.: 2 DYNAMIC ANALYSIS

DATE : MODAL ANALYSIS OF CANTILEVER BEAM

Modal Analysis of Cantilever beam for natural frequency determination. Modulus of elasticity
= 200GPa, Density = 7800 Kg/m3

Step 1: Ansys Utility Menu

File – clear and start new – do not read file – ok – yes.
Step 2: Ansys Main Menu – Preferencesselect – STRUCTURAL - ok

Step 3: Preprocessor
Element type – Add/Edit/Delete – Add – BEAM – 2D elastic 3 – ok- close.
Real constants – Add – ok – real constant set no – 1 – c/s area – 0.01*0.01 moment of inertia –
0.01*0.01**3/12 – total beam height – 0.01 – ok.
Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX – 200e9
PRXY – 0.27 – Density – 7800 – ok – close.

Step 4: Preprocessor
Modeling – Create – Key points – in Active CS – x,y,z locations – 0,0 – apply – x,y,z locations –1,0
– ok(Key points created).
Create – Lines – lines – in Active Coord – pick key points 1 and 2 – ok.
Meshing – Size Cntrls – Manual Size – Lines – All Lines – element edge length – 0.1 – ok. Mesh
Lines – Pick All – ok.

Step 5: Solution
Solution – Analysis Type – New Analysis – Modal – ok.
Solution – Analysis Type – Subspace – Analysis options – no of modes to extract – 5 – no of
modes toexpand – 5 – ok – (use default values) – ok.
Solution – Define Loads – Apply – Structural – Displacement – On Key points – Pick first key
point– apply – DOFs to be constrained – ALL DOF – ok.
Solve – current LS – ok (Solution is done is displayed) – close.
Step 7: General Post Processor
Result Summary

Step 8: General Post Processor

Read Results – First Set Plot Results – Deformed Shape – def+ undeformed – ok. Plot Ctrls –
Animate – Deformed shape – def+undeformed- ok .Read Results – Next Set Plot Results –
Deformed Shape –def + undeformed – ok.
Plot Ctrls – Animate – Deformed shape – def + undeformed-ok.

Natural frequency of particular mode shapes

The first mode shape at natural frequency

The second mode shape at natural frequency 207.58 Hz

 The forth mode shape at natural frequency 570.47 Hz

The fifth mode shape at natural frequency 823.64 Hz

RESULT:
Thus the convective heat transfer analysis of Cantilever Beam is done by using the ANSYS
Software.
EX.NO.: 3 FIXED- FIXED BEAM SUBJECTED TO FORCING FUNCTION
DATE :

Conduct a harmonic forced response test by applying a cyclic load (harmonic) at the end of
the beam. The frequency of the load will be varied from 1 - 100 Hz. Modulus of elasticity =
200GPa, Poisson‟s ratio = 0.3, Density = 7800 Kg/m3.

Step 1: Ansys Utility Menu

File – clear and start new – do not read file – ok – yes.

Step 2: Ansys Main Menu – Preferences

select – STRUCTURAL - ok

Step 3: Preprocessor
Element type – Add/Edit/Delete – Add – BEAM – 2D elastic 3 – ok – close.
Real constants – Add – ok – real constant set no – 1 – c/s area – 0.01*0.01 moment of inertia –
0.01*0.01**3/12 – total beam height – 0.01 – ok.
Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX –
200e9 – PRXY – 0.3 – Density – 7800 – ok.

Step 4: Preprocessor
Modeling – Create – Keypoints – in Active CS – x,y,z locations – 0,0 – apply – x,y,z locations
–1,0 – ok(Keypoints created).
Create – Lines – lines – in Active Coord – pick keypoints 1 and 2 – ok.

Meshing – Size Cntrls – ManualSize – Lines – All Lines – element edge length – 0.1 – ok.
Mesh Lines – Pick All – ok.

Step 5: Solution
Solution – Analysis Type – New Analysis – Harmonic – ok.
Solution – Analysis Type – Subspace – Analysis options – Solution method – FULL – DOF
printout format – Real + imaginary – ok – (use default values) – ok.
Solution – Define Loads – Apply – Structural – Displacement – On Keypoints – Pick first
keypoint – apply – DOFs to be constrained – ALL DOF – ok.
Solution – Define Loads – Apply – Structural – Force/Moment – On Keypoints – Pick
second node – apply – direction of force/mom – FY – Real part of force/mom – 100 –
imaginary part of force/mom – 0 – ok.

Solution – Load Step Opts – Time/Frequency – Freq and Substps... – Harmonic frequency
Range – 0 – 100 – number of substeps – 100 – B.C – stepped – ok. Solve –current LS – ok
(Solution is done is displayed) – close.

Step 6: Time Hist Postpro

Select „Add‟ (the green '+' sign in the upper left corner) from this window – Nodal
solution -DOFsolution – Y component of Displacement – ok. Graphically select node 2 –
ok.Select „List Data‟ (3 buttons to the left of 'Add') from the window.
'Time History Variables' window click the 'Plot' button, (2 buttons to the left of 'Add')

Step 7: Utility Menu – PlotCtrls – Style – Graphs – Modify Axis – Y axis scale –
Logarithmic –ok. Utility Menu – Plot – Replot.

This is the response at node 2 for the cyclic load applied at this node from 0 - 100 Hz.
EX.NO.: 4 TRUSSES

DATE :

Consider the four bar truss shown in figure. For the given data, find Stress in each element,
Reactionforces, Nodal displacement. E = 210 GPa, A = 0.1 m2.

Step 1: Ansys Utility Menu

File – clear and start new – do not read file – ok – yes.

Step 2: Ansys Main Menu – Preferencesselect – STRUCTURAL - ok

Step 3: Preprocessor
Element type – Add/Edit/Delete – Add – Link – 2D spar 1 – ok – close.
Real constants – Add – ok – real constant set no – 1 – c/s area – 0.1 – ok – close.
Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX –
210e9
– ok – close.
Step 4: Preprocessor
Modeling – Create – Nodes – In Active CS – Apply (first node is created) – x,y,z location in
CS
– 4 (x value w.r.t first node) – apply (second node is created) – x,y,z location in CS – 4, 3
(x, y value w.r.t first node) – apply (third node is created) – 0, 3 (x, y value w.r.t first node)
– ok (forth node is created).
Create – Elements – Elem Attributes – Material number – 1 – Real constant set number – 1
– ok Auto numbered – Thru Nodes – pick 1 & 2 – apply – pick 2 & 3 – apply – pick 3 & 1 –
apply – pick 3 & 4 – ok (elements are created through nodes).
Step 5: Preprocessor
Loads – Define loads – apply – Structural – Displacement – on Nodes – pick node 1 & 4 –
apply
– DOFs to be constrained – All DOF – ok – on Nodes – pick node 2 – apply – DOFs to be
constrained – UY – ok.
Loads – Define loads – apply – Structural – Force/Moment – on Nodes- pick node 2 – apply
– direction of For/Mom – FX – Force/Moment value – 2000 (+ve value) – ok – Structural –
Force/Moment – on Nodes- pick node 3 – apply – direction of For/Mom – FY –
Force/Moment value – -2500 (-ve value) – ok.

Step 6: Solution
Solve – current LS – ok (Solution is done is displayed) – close.

Step 7: General Post Processor

Element table – Define table – Add – „Results data item‟ – By Sequence num – LS – LS1 – ok.

Step 8: General Post Processor

Plot Results – Deformed Shape – def+undeformed – ok. Plot results – contour plot – Line
Element Results – Elem table item at node I – LS1 – Elem table item at node J – LS1 – ok
(Line Stress diagram will be displayed).
Plot results – contour plot – Nodal solution – DOF solution – displacement vector sum – ok.
List Results – reaction solution – items to be listed – All items – ok (reaction forces
will be displayed with the node numbers).
List Results – Nodal loads – items to be listed – All items – ok (Nodal loads will be
displayed with thenode numbers).

Step 9: PlotCtrls – Animate – Deformed shape – def+undeformed-ok

2.For the given data, find internal stresses developed, Nodal displacement in the planar truss
shown infigure when a vertically downward load of 10000 N is applied as shown.
 Step 1: Ansys Utility Menu

File – clear and start new – do not read file – ok – yes.

Step 2: Ansys Main Menu – Preferences

select – STRUCTURAL - ok
Step 3: Preprocessor
Element type – Add/Edit/Delete – Add – Link – 2D spar 1 – ok – close.
Real constants – Add – ok – real constant set no – 1 – c/s area – 200 – apply – real
constant setno – 2 –c/s area – 100 – ok – close.
Material Properties – material models – Structural – Linear – Elastic – Isotropic – EX – 2e5
–PRXY –0.27 – ok – close.
Step 4: Preprocessor
Modeling – Create – Nodes – In Active CS – Apply (first node is created) – x,y,z location
in CS 1000 (x value w.r.t first node) – apply (second node is created) – 500, 500 (x, y value
w.r.t firstnode) – apply (third node is created) – 2000, 1000 (x, y value w.r.t first node) – ok
(forth node is created).Create – Elements – Elem Attributes – Material number – 1 – Real
constant set number – 1 – ok.
– Auto numbered – Thru Nodes – pick 1 & 3 – apply – pick 2 & 3 – ok – Elem
Attributes – Material number – 1 – Real constant set number – 2 – ok – Auto numbered
– Thru Nodes – pick3 & 4 – apply – pick 2 & 4 – ok (elements are created through
nodes).

Step 5: Preprocessor
Loads – Define loads – apply – Structural – Displacement – on Nodes – pick node 1 & 2 –
apply
– DOFs to be constrained – All DOF – ok.
Loads – Define loads – apply – Structural – Force/Moment – on Nodes- pick node 4 –
apply –direction of For/Mom – FY – Force/Moment value – -10000 (-ve value) – ok.

Step 6: Solution
Solve – current LS – ok (Solution is done is displayed) – close.

Step 7: General Post Processor

Element table – Define table – Add – „Results data item‟ – By Sequence num – LS – LS1 –
ok.

Step 8: General Post Processor

Plot Results – Deformed Shape – def+undeformed – ok.
Plot results – contour plot – Line Element Results – Elem table item at node I – LS1 –
Elem table item atnode J – LS1 – ok (Line Stress diagram will be displayed).
Plot results – contour plot – Nodal solution – DOF solution – displacement vector sum – ok.
List Results – reaction solution – items to be listed – All items – ok (reaction forces
will be displayedwith the node numbers).

Step 9: Plot Ctrls – Animate – Deformed shape – def+undeformed-ok

 EX.NO.: 5 TWO DIMENSIONAL TRUSS ANALYSIS

DATE :

AIM
To conduct the two dimensional truss analysis of a 2D component by using
ANSYS software.

SYSTEM CONFIGURATION

Ram : 2 GB
Processor : Core 2 Quad / Core 2 Duo
Operating system: Window XP Service Pack 3
Software : ANSYS (Version10)

PROCEDURE

The three main steps to be involved are

1. Pre Processing
2.Solution
3.Post Processing
Start - All Programs –ANSYS 10 - Mechanical APDL Product Launcher –Set the
Working Directory as E Drive, User - Job Name as Roll No., Ex. No. –Click Run.

PREPROCESSING
1.preference_- structural-ok
2.Pre processor-Element type-Add/Edit/Del-Add-link-2D spral-ok
3.Real constant-Add/Edit/Del -Add 3250-ok
4.Material prop-Material modeling-Structual-Linear-Elastic-Isontropic-200000000-0.3-ok
5.Modeling-Create-Keypoint-1-Apply
We are going to define 7 keypoints for the simplified structure as given in the following table
(these keypoints are depicted by numbers in the above figure)
 key point coordinate
x y
1 0 0
2 1800 3118
3 3600 0
4 5400 3118
5 7200 0
6 9000 3118
7 10800 0

6.Line-straightline-ok

7.Meshing-Mesh tool click all lines -ok

8.Load-Define load-Apply-Structual-Displacement-On key point-All DOF-OK

Force/moment-fy(- value)-ok

9.Solution-solve-Current LS-ok

10.General prop-Plot Result-Contour plat-Nodal solution-Stress-y components-DOF

solution-ok
RESULT:
Thus the convective heat transfer analysis of a 2D component is done by using the
ANSYS Software.
 EX NO:6 ANALYSIS OF A 3-D TRUSS STRUCTURE
DATE:

AIM:

In this example you will learn to use the 3-D Truss element in ANSYS.

PROBLEM DESCRIPTION:

The tower is made up of trusses. You may recall that a truss is a structural element that
experiencesloading only in the axial direction.

Units: Use S.I. units ONLY

Geometry:

The cross sections of each of the truss members is 1.56e-3 sq meter.

Material:

Assume the structure is made of aluminum with modulus of elasticity E=75GPa.

Boundary conditions: The structure is constrained in the X, Y and Z directions at the bottom
threecorners.

Loading:

The tower is loaded at the top tip. The load is in the YZ plane and makes an angle of 75with
the negative Y axis direction. The load value is 2500 N.

Objective:

 To determine deflection at each joint.

 To determine stress in each member.
 To determine reaction forces at the base.
Give three examples where similar 3D trusses are used in practice. Model one of them
(withreasonable assumptions of dimensions, material properties and loading) using ANSYS.
Youdon't have to solve it. You can do so to check whether your assumptions were
reasonable!!
You are required to hand in print outs for the above.
STARTING ANSYS
Click on ANSYS 6.1 in the programs menu.
Select Interactive.
The following menu that comes up. Enter the working directory. All your files will be stored
in this directory. Also enter 64 for Total Workspace and 32 for Database. Give your file an
appropriate job name.

Click on Run

MODELING THE STRUCTURE

Go to ANSYS Utility Menu. Click on Workplane>Change Active CS to..>Global

Cartesian.

Go to the ANSYS Main Menu.

Click Preprocessor>Modeling>Create>Keypoints>In active CS
The following window comes up.

Fill in thekeypoint number (1,2,3...) and the coordinates. Make sure you get the correct
coordinatesfrom the figure. Create all the 10 keypoints. Make sure the numbering of your
keypoints matches thenumbering of the joints in the figure.

If you cannot see the grid then go to Utility Menu>Display Working Plane

Fill in thekeypoint number (1,2,3...) and the coordinates. Make sure you get the correct
coordinatesfrom the figure. Create all the 10 keypoints. Make sure the numbering of your
keypoints matches thenumbering of the joints in the figure.

If you cannot see the grid then go to Utility Menu>Display Working Plane

If you cannot see the complete figure then go to Utility Menu>PlotCntrls>Pan Zoom
Rotateand zoom out to see the entire figure.Now create lines connecting the keypoints
Click on Preprocessor>Modeling>Create>Lines>Lines>In ActiveCoord.
Pick the endpoints of each element to create the lines. Rotate the figure for more
accessibleviews.

You can use theUtility Menu>PlotCtrls>Pan Zoom Rotate window to rotate the model and
seeits 3D nature.

MATERIAL PROPERTIES

Go to the ANSYS Main Menu

Click Preprocessor>Material Props>Material Models. In the window that comes up which
is shown below, forMaterial Model 1, choose Structural>Linear>Elastic>Isotropic.

Double click Isotropic for Material Model 1.

Fill in 7.5e10 for the Young's modulus and 0.3 for minor Poisson's Ratio. Click OK
Now the material 1 has the properties defined in the above table. We will use this material for
the elements of thestructure.

ELEMENT PROPERTIES:

Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that

opens clickon Add... The following window opens.
RESULT:
Thus the convective heat transfer analysis of a 3D component is done by using the
ANSYS Software.
 STRESS ANALYSIS OF BEAM
EX.NO.: 7
DATE :

AIM
To conduct the stress analysis in a beam using ANSYS software.

PROCEDURE

The three main steps to be involved are

1. Pre Processing
2. Solution
3. Post Processing
Start - All Programs –ANSYS 10 - Mechanical APDL Product Launcher –Set the
Working Directory as E Drive, User - Job Name as Roll No., Ex. No. –Click Run.

PRE PROCESSING

1. Preference - Structural- h-Method - Ok.

2. Preprocessor - Element type - Add/Edit/Delete –Add –Beam, 2D elastic 3 –Ok –

Options – Ok - Close.

3. Sections –beam –Common sections –Select the correct section of the beam and input
the
Of “w1, w2,w3”–Previewand–Note“t1,downthe valuest2,of area,t3”Iyy.

4. Real constants - Add/Edit/Delete –Add –Ok –Enter the values of area=5500,

Izz=0.133e8, height=3 –Ok -Close.

5. Material props - Material Models –Structural –Linear –Elastic –Isotropic - EX 2e5,

PRXY 0.3 - Ok.

6. Modeling –Create –Key points –In active CS –Enter the values of CS of each key
points – Apply –Ok. Lines –Lines –Straight line –Pick the all points –Ok.

7. Meshing –Mesh attributes –All lines –Ok. Meshing –Size cntrls –Manual size – Lines
–All lines –Enter the value of element edge length [or] Number of element divisions –
Ok. Mesh tool –Mesh –Pick all.

SOLUTION

8. Solution –Define Loads –Apply –Structural –Displacement - On key points –Select

the 1st key point –ALL DOF –Ok. On key points –select the 2nd key point–UY – Ok.
 Force/Moment –On key points –Select the key point –Ok –direction of force/moment
FY, Value = -1,000 (- sign indicates the direction of the force) –Ok.

9. Solve –Current LS –Ok –Solution is done –Close.

WWW.VIDYARTHIPLUS.COM

POST PROCESSING

11. General post proc –Element table –Define table –Add –By sequence num –
SMISC,6 –Ok –SMISC,12 –Ok –LS,2 –Ok –LS,3 - Ok –Close. Plot results –
Contour plot –Nodal solution –DOF solution –Y component of displacement –
Ok.Contour plot –Line element Res –Node I SMIS 6, Node J SMIS 12 –Ok.
Contour plot –Line element Res –Node I LS 2, Node J LS 3 –Ok

FOR REPORT GENERATION

12. . File –Report Generator –Choose Append –OK –Image Capture –Ok - Close.
RESULT
Thus the stress analysis of a BEAM is done by using the ANSYS Software.
EX NO :8 MODE FREQUENCY ANALYSIS OF BEAM
DATE : WWW.VIDYARTHIPLUS.COM

AIM
To conduct the Mode frequency analysis of beam using ANSYS software.

SYSTEM CONFIGURATION

Ram : 2 GB
Processor : Core 2 Quad / Core 2 Duo
Operating system: Window XP Service Pack 3
Software : ANSYS (Version10)

PROCEDURE

The three main steps to be involved are

1. Pre Processing
2. Solution
3. Post Processing

Start - All Programs –ANSYS 10 - Mechanical APDL Product Launcher –Set the
Working Directory as E Drive, User - Job Name as Roll No., Ex. No. –Click Run.

PREPROCESSING

1. Preprocessor - Element type - Add/Edit/Delete –Add –Beam, 2D elastic 3 –Ok –

Close.

2. Real constants - Add/Edit/Delete –Add –Ok –Area 0.1e-3, Izz 0.833e-9, Height
0.01 – Ok –Close.

3. Material props - Material Models –Structural –Linear –Elastic - Isotropic –EX

206e9, PRXY 0.25 –Ok –Density –DENS 7830 –Ok.

4. Modeling –Create –Key points –Inactive CS –Enter the coordinate values - Ok.
Lines -lines –Straight Line –Join the two key points –Ok.

5. Meshing –Size Cntrls –manual size –lines –all lines –Enter the value of no of
element divisions 25 –Ok. Mesh –Lines –Select the line –Ok.
SOLUTION

6. Solution –Define Loads –Apply –Structural –Displacement - On nodes –Select

the node point –Ok –All DOF –Ok. Analysis type –New analysis –Modal –Ok.
Analysis type –Analysis options –Block Lanczos –enter the value no of modes to
extract as 3 or 4 or 5 –Ok –End Frequency 10000 –Ok.
7. Solve –Current LS –Ok –Solution is done –Close.

POST PROCESSING
8. General post proc –Read results –First set - Plot results –Deformed shape –Choose
Def+undeformed –Ok.Read results –Next set - Plot results –Deformed shape –
Choose Def+undeformed –Ok and so on.

FOR REPORT GENERATION

9. File –Report Generator –Choose Append –OK –Image Capture –Ok - Close.
(Capture all images)
RESULT
Thus the Mode frequency analysis of a BEAM is done by using the ANSYS
Software.
EX.NO : 9 STRESS ANALYSIS OF A PLATE WITH CIRCULAR HOLE
DATE :

AIM
To conduct the stress analysis in a plate with a circular hole using ANSYS software.

SYSTEM CONFIGURATION

Ram : 2 GB
Processor : Core 2 Quad / Core 2 Duo
Operating system: Window XP Service Pack 3
Software : ANSYS (Version10)

PROCEDURE

The three main steps to be involved are

1. Pre Processing
2. Solution
3. Post Processing
Start - All Programs –ANSYS 10 - Mechanical APDL Product Launcher –Set the
Working Directory as E Drive, User - Job Name as Roll No., Ex. No. –Click Run.

PREPROCESSING

1. Preference - Structural- h-Method - Ok.

2. Preprocessor - Element type - Add/Edit/Delete –Add –Solid, 8 node 82 –Ok –

Option
–Choose Plane stress w/thk - Close.

3. Real constants - Add/Edit/Delete –Add –Ok –THK 0.5 –Ok - Close.

4. Material props - Material Models –Structural –Linear –Elastic –Isotropic - EX

2e5, PRXY 0.3 - Ok.

5. Modeling –Create –Areas –Rectangle - by 2 corner - X=0, Y=0, Width=100,

Height=50 - Ok. Circle - Solid circle - X=50, Y=25, Radius=10 - Ok.

Operate – Booleans –Subtract –Areas - Select the larger area (rectangle) –Ok –
Ok - Select Circle –Next –Ok - Ok.
 WWW.VIDYARTHIPLUS.COM

6. Meshing - Mesh Tool –Area –Set - Select the object –Ok - Element edge length
2/3/4/5 –Ok - Mesh Tool -Select TRI or QUAD - Free/Mapped –Mesh - Select the
object - Ok.
SOLUTION
7. Solution –Define Loads –Apply –Structural –Displacement - On lines -
Select the boundary where is going to be arrested –Ok - All DOF - Ok.
Pressure - On lines - Select the load applying area –Ok - Load PRES valve = 1
N/mm2-Ok.

8. Solve –Current LS –Ok –Solution is done –Close.

THIPLUS
Young‟s Modulus = 200 GPa
Poisson‟s Ratio = 0.3
 RESULT

Thus the stress analysis of rectangular plate with a circular hole is done by
using the ANSYS Software.
EX. NO : 10 INTRODUCTION TO MATLAB

DATE:

AIM
To Study the capabilities of Mat Lab Software.

INTRODUCTION

The MATLAB is a high-performance language for technical computing integrates

computation, visualization, and programming in an easy-to-use environment where
problems and solutions are expressed in familiar mathematical
notation. Typical uses include
• Math and computation
• Algorithm development
• Data acquisition
• Modeling, simulation, and prototyping
• Data analysis, exploration, and visualization
• Scientific and engineering graphics
• Application development,

Including graphical user interface building MATLAB is an interactive system whose basic
data element is an array that does not require dimensioning. It allows you to solve many
technical computing problems, especially those with matrix and vector formulations, in a
fraction of the time it would take to write a program in a scalar noninteractive language
such as C or FORTRAN.

The name MATLAB stands for matrix laboratory. MATLAB was originally written to
provide easy access to matrix software developed by the LINPACK and EISPACK
projects. Today, MATLAB engines incorporate the LAPACK and BLAS libraries,
embedding the state of the art in software for matrix computation.
SIMULINK INTRODUCTION:

Simulink is a graphical extension to MATLAB for modeling and simulation of

systems. In Simulink, systems are drawn on screen as block diagrams. Many elements of
block diagrams are available, such as transfer functions, summing junctions, etc., as well as
virtual input and output devices such as function generators and oscilloscopes. Simulink is
integrated with MATLAB and data can be easily transferred between the programs. In
these tutorials, we will apply Simulink to the examples from the MATLAB tutorials to
model the systems, build controllers, and simulate the systems. Simulink is supported on
Unix, Macintosh, and Windows environments; and is included in the student version of
MATLAB for personal computers.
The idea behind these tutorials is that you can view them in one window while running
Simulink in another window. System model files can be downloaded from the tutorials and
opened in Simulink. You will modify and extend this system while learning to use
Simulink for system modeling, control, and simulation. Do not confuse the windows, icons,
and menus in the tutorials for your actual Simulink windows. Most images in these
tutorials are not live - they simply display what you should see in your own Simulink
windows. All Simulink operations should be done in your Simulink windows.
1. Starting Simulink
2. Model Files
3. Basic Elements
4. Running Simulations
5. Building Systems
Starting Simulink

Simulink is started from the MATLAB command prompt by entering the following
command:

>> Simulink

Alternatively, you can hit the Simulink button at the top of the MATLAB window as
shown below:

When it starts, Simulink brings up the Simulink Library browser.

 WWW.VIDYARTHIPLUS.COM

Open the modeling window with New then Model from the File menu on the Simulink
Library Browser as shown above.

This will bring up a new untitled modeling window shown below.

Model Files

In Simulink, a model is a collection of blocks which, in general, represents a system. In addition to

drawing a model into a blank model window, previously saved model files can be loaded either
from the File menu or from the MATLAB command prompt.

You can open saved files in Simulink by entering the following command in the MATLAB
command window. (Alternatively, you can load a file using the Open option in the File menu in
Simulink, or by hitting Ctrl+O in Simulink.)

>> filename
The following is an example model window.

A new model can be created by selecting New from the File menu in any Simulink window (or by
hitting Ctrl+N).

Basic Elements
WWW.VIDYARTHIPLUS.COM
There are two major classes of items in Simulink: blocks and lines. Blocks are used to generate,
modify, combine, output, and display signals. Lines are used to transfer signals from one block to
another.

Blocks

There are several general classes of blocks:

 Continuous
 Discontinuous
 Discrete
 Look-Up Tables
 Math Operations
 Model Verification
 Model-Wide Utilities
 Ports & Subsystems
 Signal Attributes
 Signal Routing
 Sinks: Used to output or display signals
 Sources: Used to generate various signals
 User-Defined Functions
 Discrete: Linear, discrete-time system elements (transfer functions, state-space models, etc.)
 Linear: Linear, continuous-time system elements and connections (summing junctions, gains,
etc.)
 Nonlinear: Nonlinear operators (arbitrary functions, saturation, delay, etc.)
 Connections: Multiplex, Demultiplex, System Macros, etc.

Blocks have zero to several input terminals and zero to several output terminals. Unused input
terminals are indicated by a small open triangle. Unused output terminals are indicated by a small
triangular point. The block shown below has an unused input terminal on the left and an unused
output terminal on the right.

Lines
Lines transmit signals in the direction indicated by the arrow. Lines must always transmit signals
from the output terminal of one block to the input terminal of another block. One exception to this
is a line can tap off of another line, splitting the signal to each of two destination blocks, as shown
below.

Lines can never inject a signal into another line; lines must be combined through the use of a block
such as a summing junction.

A signal can be either a scalar signal or a vector signal. For Single-Input, Single-Output systems,
scalar signals are generally used. For Multi-Input, Multi-Output systems, vector signals are often
used, consisting of two or more scalar signals. The lines used to transmit scalar and vector signals
are identical. The type of signal carried by a line is determined by the blocks on either end of the
line.
Simple Example

The simple model (from the model files section) consists of three blocks: Step, Transfer Fcn, and
Scope. The Step is a source block from which a step input signal originates. This signal is
transferred through the line in the direction indicated by the arrow to the Transfer Function linear
block. The Transfer Function modifies its input signal and outputs a new signal on a line to the
Scope. The Scope is a sink block used to display a signal much like an oscilloscope.

There are many more types of blocks available in Simulink, some of which will be discussed later.
Right now, we will examine just the three we have used in the simple model.

Running Simulations
To run a simulation, we will work with the following model file: simple2.mdl

Download and open this file in Simulink following the previous instructions for this file. You
should see the following model window.

Before running a simulation of this system, first open the scope window by double-clicking on the
scope block. Then, to start the simulation, either select Start from the Simulation menu (as shown
below) or hit Ctrl-T in the model window.
 .VIDYARTHIPLUS.COM
The simulation should run very quickly and the scope window will appear as shown below. If it
doesn't, just double click on the block labeled "scope."

Note that the simulation output (shown in yellow) is at a very low level relative to the axes of the
scope. To fix this, hit the auto scale button (binoculars), which will rescale the axes as shown
below?

Note that the step response does not begin until t=1. This can be changed by double-clicking
on the "step" block. Now, we will change the parameters of the system and simulate the system
again. Double-click on the "Transfer Fcn" block in the model window and change the denominator
to [1 20 400]

Re-run the simulation (hit Ctrl-T) and you should see what appears as a flat line in the
scope window. Hit the auto scale button, and you should see the following in the scope window.

Notice that the auto scale button only changes the vertical axis. Since the new transfer
function has a very fast response, it compressed into a very narrow part of the scope window. This
is not really a problem with the scope, but with the simulation itself. Simulink simulated the system
for a full ten seconds even though the system had reached steady state shortly after one second.

To correct this, you need to change the parameters of the simulation itself. In the model
window, select Parameters from the Simulation menu. You will see the following dialog box.
WW.VIDYARTHIPLUS.

There are many simulation parameter options; we will only be concerned with the start and
stop times, which tell Simulink over what time period to perform the simulation. Change Start time
from 0.0 to 0.8 (since the step doesn't occur until t=1.0. Change Stop time from 10.0 to 2.0, which
should be only shortly after the system settles. Close the dialog box and rerun the simulation.

After hitting the auto scale button, the scope window should provide a much better display
of the step response as shown below.

Result
Thus the features of MATLAB are studied.
EX. NO : 11 ANALYSIS OF AIRCRAFT WING STRUCTURE
DATE:

OBJECTIVES
a. To perform the static structural analysis of a aircraft wing.

b. To study the shear stress distributions over the wing surface.

RESOURCE:
ANSYS 16.0 Academic

PROBLEM DESCRIPTION:

 Perform the static analysis of aircraft wing of span 550m and taper
ratio 0.4.
PROCEDURE:
Preferences: Structural Preprocessor:
 Element  Add  Beam 3
 Material Properties Material Models  Structural  LinearElastic  Isotropic  Ex
= 2e11  PRXY =
0.33 Density = 7850kg/(m^3)Ok
 Modeling Create  Key points  Inactive CS  (0,0,0);(100,0,0)  Ok  Lines
Areas  Ok
 Meshing Size Controls  Manual Sizing  Lines  Picked Lines  No. of elements =
20  Ok Mesh 
Lines  Ok
 Select parameters  select functions define

SOLUTION:
 Analysis Type  New analysis Transient Ok
 Parameters functions define/edit type in result= 1000 k sin({pi}/4*{time})
 Select file file name= transient save
 Parameters functions read from file open transient give table parameter name
cantilever
 Select loads define loads apply structural displacement on keypoints
all DOF keypoint 1 ok
 Solve Current LS  Ok Results
 AIRCRAFT WING

RESULT

Thus the analysis of Shell structure of aircraft wing structure with is done by using the
ANSYS Software.
EX. NO : 12 ANALYSIS OF FUSELAGE
DATE :

OBJECTIVE:
a. To perform the variant analysis of a Aircraft fuselage.
b. To interpret the results of the analysis and study the behavior of the Strucutre

RESOURCE:
ANSYS 16.0 Academic

PROBLEM DESCRIPTION:
 To calculate the deformation of the aluminum fuselage section under the
application of internal load of 100000 Pa.

PROCEDURE:
PREPROCESSING

STEP 1: From the Main menu select preferences Select structural and press OK

STEP 2: From the main menu select Pre-processor

Element type  Add / edit/Delete  Add  Solid – 10 node 92 Apply Add  Beam 2
Node 188  Apply  Add  Shell Elastic 4 node 63

Real Constants  Add  Select shell  give thickness (I) = 1 ok  close.

Material properties  material models  Structural  Linear  Elastic 

Isotropic EX = 0.7e11; PRXY = 0.3; Density = 2700

STEP 3: From the main menu select Pre-processor

Pre-processor  modelling  Create  Areas  Circle  Annulus WP x = 0 ; WP y

= 0; Rad – 1 = 2.5; Rad - 2 = 2.3 OK

Pre-processor  Modelling  Create  Circle  Solid –

WP x = 0; X = 2.25; Y = 0 Radius = 0.15Apply WP x = 0; X = -2.25; Y = 0 Radius = 0.15

Apply WP x = 0; X =0; Y = 2.25; Radius = 0.15 Apply WP x = 0; X = 0; Y = -2.25 Radius =
0.15 OK
Pre-processor  Modelling  Operate  Booleans  Add  Areas – Pick all OK Pre-
processor  Modelling  Operate  Extrude  Areas  By XYZ offset X= 0; Y=0; Z = 5
STEP 4: Meshing the Geometry
Pre-processor Meshing  Size controls  Manual Size  All Areas  give element edge
length as 0.15 ok
 Meshing  Size controls  Manual Size  All lines  give element edge length as ok
Meshing  Mesh  areas  free  select box type instead of single  select the total
volume  ok

SOLUTION PHASE:

STEP 5: From the ANSYS main menu open Solution

STEP 6: Loads  define loads  Apply  Structural  Displacement  On areas  select
box type  select box (4 points at centre)  all DOF  ok Select  ALL DOF arrested
Define loads  Apply  Structural  Pressure  on areas  select the internal surface of
the fuselage and give value (100000)  ok

STEP 7: Solving the system Solution Solve 

Current LS POSTPROCESSING: VIEWING

THE RESULTS RESULT:

Case: 1:- To Calculate the deformation of the aluminum fuselage section under the application
of internal load at 1e5.

Y COMPONENT OF DISPLACEMENT

DMX = .194E-04 SMN = -.194E-04 SMX = .194E-04

VON MISSES STRESS

DMX = .194E-04 SMX = .124E+07

 FUSELAGE

RESULT

Thus the analysis of Aircraft fuselage structure with is done by using the ANSYS
Software.
EX. NO : 13 NON-LINEAR FINITE ELEMENT ANALYSIS OF SHELLS
DATE :

FINITE ELEMENT METHOD

The finite element method (FEM) is a numerical technique for finding approximate solutions
to boundary value problems. It uses subdivision of a whole problem domain into simpler
parts, called finite elements. FEM provides methods in which the structure is divided into
very small but finite number of elements, to approximate a more complex equation over a
larger domain. Engineering structures that have complex geometry and loads, are very
difficult to analyze or have no theoretical solution. However, in FEA, a structure of this type
can be analysed
Complex Engineering problems without knowing the governing equations can be solved.
FEA software provides a complete solution including deflections, stresses, reactions etc. FEA
technique facilitates an easier and a more accurate analysis.
METHODOLOGY

Cylindrical shell element will be analysed in both 2D and 3D with possible us of 4 noded, 8
noded, and 20 noded elements. The thickness of concrete is 12.5 cms. The radius of shell (R)
is kept constant at 7.62 m. The shell element will be withheld by span to radius ratio as 1, 2
and 3. Semi central angle (Φ) will be taken as 40 degrees. The length of the span (L) will be
taken according to the span to radius ratio as 7.62 m (short shell),
15.24 m (moderate shell) and 22.86 m (long shell). Young‟s modulus (E) = 0.250 x 108
KN/m2 Poisson;s ratio (µ) = 0.15
Density of concrete (γ) = 0.250 x 102 KN/m3

Loading to be considered:
Self-weight
Self-weight and Wind Load
Self-weight and Earthquake Load
Due to Symmetry only a quarter part of shell is taken for the analysis. The different meshing
sizes taken for the analysis are: 2x2 mesh, 4x4 mesh and 8x8 mesh. The response of these
meshing is studied for different loading conditions in elastic state.
 The meshing of short shell is shown in the figure below:

Figure 1- Geometry of the shell. Figure 2- 2x2 mesh of the shell.

Figure 3- 4x4 mesh of the shell. Figure 4- 8x8 mesh of the shell

4 Noded 2D Shell Element

Transverse disp. for L/R = 1 Transverse disp. for L/R = 2

20 120
100
Displacement in

Displacement in

15
80

10 60
40
5
mm

mm

20
0
0
0 10 20 30 40 50
0 10 20 30 40 50
Angle in degrees Angle in degrees

2x2 mesh 4x4 mesh 8x8 mesh

2x2 mesh 4x4 mesh 8x8 mesh

Transverse Displacement for short shell

 Transverse disp. For L/R =3
450
400

Displacement in
350
300
250
200
mm 150
100
50
0
0 10 20 30 40 50
Angle in degrees

2x2 mesh 4x4 mesh 8x8 mesh

Figure 7- Transverse Displacement for long shell

Its has been observed that as the meshing size is increased we get accurate results for the transverse
displacements. The results for mesh sizes 4x4 and 8x8 gives nearly similar as compared to the 2x2
mesh. The differences in the transverse displacement of the centre of the shell and the edges
decrease as the span/depth ratio increases.
The results of the transverse displacements of the shells shows that we get more accurate results for
8x8 meshing. So we take the values obtained for 8x8 meshing size for different span to depth ratios
and also for different elements (2D & 3D).
The variation of the transverse displacements to the different span to depth ratios (1, 2, 3) are
shown below for a 4 noded 2D element

.
4 noded 2D element 8 noded 2D element
450 450
400 400
Displacement

350 350
Displacement

300 300
250 250
200 200
150 150
imm

100 100
50 50
0 0
0 10 20 30 40 50 0 10 20 30 40 50
Angle in degrees Angle in degrees

L/R = 1 L/R = 2 L/R = 3 L/R = 1 L/R = 2 L/R = 3

Figure 8-Displacements for various L/R ratios . Figure 9-Displacements for various L/R ratios

The graphs above shows that the transverse displacements increase by smaller value by increasing
the L/R ratio from 1 -2 and it drastically increases for the L/R ratio 3. It indicates that longer shells
are more prone to failures as the self-weight deflection is very large.
The variation of transverse displacements for different elements shows similar behaviour for all the
four elements used For centre nodes, 8 noded 3D element shows maximum deflection and for the edge
nodes, the 20 noded 3D elements shows the maximum deflection.

. Displacements for L/R =1

16

14

12

10

0
0 5 10 15 20 25 30 35 40 45
Angle in degrees

4 noded 2D 8 noded 2D 8 noded 3D 20 noded 3D

Figure 10-Displacements for various elements

RESULT

Thus the analysis of shells structure with is done by using the ANSYS Software.
 EX. NO : 14 ANALYSIS OF SCAFFOLDING STRUCTURE USING ANSYS
DATE :

PRE-PROCESSOR STAGE IMPORTING THE MODEL INTO ANSYS:

 File  Import  IGES (selecting the scaffolding „structure. iges‟ file that has been exported
from PRO/E)

TYPE OF ANALYSIS

 Preferences  Structural
 Pre-processing of the model:
 Preprocessor  Element type  Add (select „solid 10node187‟)
 Preprocessor Material Properties Material Models
 Structural LinearElastic  Isotropic EX=70000 and PRXY=0.33
 Preprocessor  Modeling  OperateBooleans Overlap  Volumes  Pick all
 Dividing the surface area of the holes into equal quarters:
 Preprocessor  Modeling  Create  Key points Line w/Ratio
Now selecting the semicircular line attached to one surface area of the circular plate and the ratio of
„0.5‟ is given.
Thus a new key point is created exactly at center of the circumference of the hole.
 Preprocessor  modeling  Create  Lines
Currently picking the above created key points a line is formed.
 Preprocessor modeling Operate Booleans Divide  Area by Line

Now the inner half surface area of the hole is divided into two equal areas. This process of area
division is carried out all over the model.

Division of surface area.

Thus the surface areas are divided into equal quarters. This procedure is repeated for all the
circular holes present in the model
Meshing of the Model

 Preprocessor  Meshing  Mesh Tools

 Global Set  Solid 10node187  Ok
 Check Box  Smart size „on‟ to size 6
 Size Controls  Global Set  Element Edge Length= 5
 Mesh  Volumes  tet, free  Mesh  Pick all.

Now the meshing of the complete model will be done. In the model that has been imported has
finally produced about 1106223elements and 1823667

Element plot of the model. Nodes

COUPLING

Preprocessor  Coupling/ Ceqn  couple DOFs

Picking the nodes at the starting and ending plates and coupling to the respective
nodes on Central Support Tube as these solid plates that should be attached to CST.
Coupling is done due to the minor errors in the assembly of the final model so as to avoid
incorrect results.

Couplings and Constrains

 APPLICATION OF LOADS AND CONSTRAINS

 Solution  Define Loads  Apply  Structural 

Displacement  On Nodes
Selecting the nodes present near the circular hole on the starting plate using a circle and the
rectangular extrusion on the final or ending plate using a polygon. The displacement of these
nodes is arrested in all Degrees Of Freedom (All DOF).

 Solution  Define Loads  Structural  Apply 

Pressure  On Areas
Now calculating the pressure that is applied on the surface areas of the holes at an acceleration of
„3G‟ using the below equations.

Where,
Wt of each munitions = 27kgs. Acceleration due to gravity,
Area can be measured directly from the assembly model.

Element Load Plot

PRESSURE ON 3RD PLATE:

Area = 1125.98 mm2 for each quarter.
= 2502.25 mm2 for each half section on the circumference.
Pressure = 0.3528N/ mm2
= 0.1588N/ mm2
PRESSURE ON 4TH PLATE:
Area = 1129.28 mm2 Pressure = 0.3518N/ mm2

Deflection of Scaffolding Structure:

 General postproc  Plot Results  Deformed Shape.
 Max Deflection (DMX) = 0.225mm
 Pressure on 1St plate: Area =2269.77mm2 Pressure = 0.175N/ mm2
Pressure on 2nd plate:for each quarter.

= 2374.32 mm2 for each half section on the circumference. Pressure =

0.3538N/ mm2 for each quarter.
= 0.167N/ mm2 for half sections on the circumference.

Deflection Plot.

General Postproc  Plot Results  Countr Plot  Nodal Sol‟n  stress 

von mises stress solution.
o Minimum Stress (SMN) = 0.179e-05
o Maximum Stress (SMX) = 193.198

Deflection Plot.

RESULT
Thus the analysis of Scaffolding Structure with is done by using the ANSYS
Software.