Casa lab manual

BB..LL..DD..EE..AA’’SS SSSSMM PPOOLLYYTTEECCHHNNIICC,, VVIIJJAAYYAAPPUURR..
DDEEPPAARRTTMMEENNTT OOFF MMEECCHHAANNIICCAALL EENNGGIINNEEEERRIINNGG
CCAASSAA LLAABB MMAANNUUAALL
BBYY--BBHHAARRAATT NNIIKKKKAAMM LLEECCTT..

Introduction to ANSYS
v
ANSYS is a complete FEA software package used by engineers worldwide in virtually all fields of
engineering:
o Structural
o Thermal
o Fluid, including CFD (Computational Fluid Dynamics)
o Electrical / Electrostatics
O Electromagnetics
v
A partial list of industries in which ANSYS is used:
o Aerospace
o Automotive
O Bio-medical
o Bridges & Buildings
v
ANSYS/Multiphysics is the flagship ANSYS product which includes all capabilities in all
engineering disciplines.

DEPARTMENT OF MECHANICAL ENGINEERING
v
There are three main component products derived from ANSYS/Multiphysics:
OANSYS/Mechanical - structural & thermal capabilities
OANSYS/Emag - electromagnetics
OANSYS/FLOTRAN - CFD capabilities
v
Other product lines:
OANSYS/LS-DYNA - for highly nonlinear structural problems
ODesign Space - an easy-to-use design and analysis tool meant for quick analysis within
the CAD environment
OANSYS/ProFEA - for ANSYS analysis & design optimization within Pro/ENGINEER
v
Structural analysis: is used to determine deformations, strains, stresses, and reaction forces.
OStatic analysis
ß
Used for static loading conditions.
ß
Nonlinear behavior such as large deflections, large strain, contact, plasticity, hyper
elasticity, and creep can be simulated
ODynamic analysis
ß
Includes mass and damping effects.
ß
Modal analysis calculates natural frequencies and mode shapes.
ß
Harmonic analysis determines a structure‘s response to sinusoidal loads
of known amplitude and frequency.
ß
Transient Dynamic analysis determines a structure‘s response to time-
varying loadsand can include nonlinear behavior.
OOther structural capabilities
ß
Spectrum analysis
ß
Random vibrations
ß
Eigen value buckling
ß
Substructuring, submodeling
OExplicit Dynamics with ANSYS/LS-DYNA
ß
Intended for very large deformation simulations where inertia forces are dominant.
ß
Used to simulate impact, crushing, rapid forming, etc.
v
Thermal analysis: is used to determine the temperature distribution in an object. Other
quantities of interest include amount of heat lost or gained, thermal gradients, and thermal flux.
All three primary heat transfer modes can be simulated: conduction, convection, radiation.
O Steady-State
ß
Time-dependent effects are ignored.
O Transient
ß
To determine temperatures, etc. as a function of time.
ß
Allows phase change (melting or freezing) to be simulated.

O Electromagnetic analysis is used to calculate magnetic fields in electromagnetic devices.
O Static and low-frequency electro magnetic
ß
To simulate devices operating with DC power sources, low-frequency
AC, or low- frequency transient signals.
v
Computational Fluid Dynamics (CFD)
oTo determine the flow distributions and temperatures in a fluid.
oANSYS/FLOTRAN can simulate laminar and turbulent flow, compressible andincompressible
flow, and multiple species.
o Applications: aerospace, electronic packaging, automotive design
o Typical quantities of interest are velocities, pressures, temperatures, and film coefficients.
The GUI Layout
Icon Toolbar Menu
Input Line Raise/Hidden Icon
Abbreviation Toolbar Menu
Graphics Area
Main Menu
Output
Window
User Prompt Info
Current Settings
Utility Menu
Contains functions which are available throughout the ANSYS session, such as file
controls, selecting, graphics controls, parameters, and exiting.
Toolbar Menu
Contains push buttons for executing commonly used ANSYS commands and functions.
Customized buttons can be created.
Graphics Area
Displays graphics created in ANSYS or imported into ANSYS.
Input Line Displays program prompt messages and a text field for typing commands. All
previously typed commands appear for easy reference and access.

Main Menu
Contains the primary ANSYS functions, organized by processors (preprocessor, solution,
general postprocessor, etc.)
Output
Displays text output from the program. It is usually positioned behind the other windows
and can be raised to the front when necessary.
Resume:
This is opening a previously saved database. It is important to know that if you simply
resume a database, it doesn‘t change the job name. For example: You start ANSYS with a job
name of ―fileǁ. Then you resume my model.db, do some work, then save. That save is done to
file.db! Avoid this issue by always resuming using the icon on the toolbar. If you open
mymodel.db using this method, it resumes the model and automatically changes the job name to
my model.
Plotting:
Contrary to the name, this has nothing to do with sending an image to a plotter or printer.
Plotting in ANSYS refers to drawing something in the graphics window. Generally you plot one
type of entity (lines, elements, etc.) to the screen at a time. If you want to plot more than one
kind of entity use, ―Plot → Multiplotǁ, which by default will plot everything in your model at
once.
Plot Controls:
This refers to how you want your ―plotǁ to look on the screen (shaded, wire frame, entity
numbers on or off, etc). Other plot control functions include sending an image to a graphics file
or printer.
Creating Geometry:
Geometry in ANSYS is created from
―Main Menu → Preprocessor → Modeling → Createǁ and has the following terminology,
KEYPOINTS: These are points, locations in 3D space.
LINES: This includes straight lines, curves, circles, spline curves, etc. Lines are typically
defined using existing key points.
AREAS: This is a surface. When you create an area, it‘s associated lines and key points are
automatically created to border it.
VOLUMES: This is a solid. When you create a volume, it‘s associated areas, lines and key
points are automatically created.
SOLID MODEL: In most packages this would refer to the volumes only, but in ANSYS this
refers to your geometry. Any geometry. A line is considered a ―solid modelǁ.
You can‘t delete a child entity without deleting its parent, in other words you can‘t delete a line
if it‘s part of an area, can‘t delete a key point if it‘s the end point of a line, etc.
Boolean Operations:
Top Down style modeling can be a very convenient way to work. Instead of first creating
key points, then lines from those key points, then areas from the lines and so on (bottom up
modeling), start with volumes of basic shapes and use Boolean operations to add them, subtract
them, divide them etc. Even if you are creating a shell model, for example a box, you could
create the box as a volume (a single command) and then delete the volume keeping the existing
areas, lines and key points.
These kinds of operations are found under ―Main Menu → Preprocessor → Modeling →
Operate → Booleansǁ with some common ones being:
Add: Take two entities that overlap (or are at least touching) and make them one.

Subtract: Subtract one entity from another. To make a hole in a plate, create the plate (area of
volume) then create a circular area or cylinder and subtract it from the plate.
Glue: Take two entities that are touching and make them contiguous or congruent so that when
meshed they will share common nodes. For example, using default mesh parameters,
Note: In case of Meshing after gluing areas. The coincident nodes on the common line between the two
areas will be automatically merged. You don‘t have to manually equivalence them like in some other
codes.
The Working Plane:
All geometry is created with respect to the working plane, which by
default is aligned with the global Cartesian coordinate system. The
―Working Planeǁ is actually the XY plane of the working coordinate
system. The working coordinate system ID is coordinate system 4 in
ANSYS. Global Cartesian is ID 0, Global Cylindrical is ID 1, and Global
Spherical is ID 2.
Working Plane Hints:
Turn on the working plane so you can see it with, ―Utility Menu
→ Work Plane → Display Working Planeǁ.
Change the way the working plane looks or adjust the snap settings under
―Utility Menu → Work Plane → WP Settings…ǁ.
Move the working plane around using
―Utility Menu → Work Plane → Offset WP to…ǁ.
Align the working plane with various parts of the model using
―Utility Menu → Work Plane → Align WP with…ǁ.
If you select more than one node or keypoint to offset the working plane to, it will go to the
average location of the selected entities. VERY handy!
Use the working plane to slice and dice your model. For example to cut an area in pieces use
―Main Menu → Modeling → Operate → Booleans → Divide → Area by WrkPlaneǁ. Do this for
lines and volumes as well.

Select Logic:
Selecting is an important and fundamental concept in ANSYS. Selected entities are your active
entities. All operations (including Solving) are performed on the selected set. In many
operations you select items ―on the flyǁ; ANSYS prompts for what volumes to mesh for
example, you pick them with the mouse, and ANSYS does the meshing.
However there are many times when you need to select things in more sophisticated ways. Also,
in an ANSYS input file or batch file you can‘t select things with the
mouse!
Examples where this would be useful:
• You have many different areas at Z = 0 you want to constrain. You could
select them all one by one when applying the constraint, or select ―By
Locationǁ beforehand, then say ―Pick Allǁ in the picking dialog.
• You have a structure with many fastener holes that you want to constrain.
Again, you could select them all one by one when applying the constraint,
or select lines ―By Length/Radiusǁ, type in the radius of the
holes to select all of them in one shot, then ―Pick Allǁ in the picking
dialog when applying the constraint.
After working with the selected set,
―Utility Menu → Select → Everythingǁ to make the whole model active
again.
Select Entities Dialog Box Terminology:
From Full: Select from the entire set of entities in the model.
Reselect: Select a subset from the currently selected entities.
Also Select: Select in addition to (from the whole model) the set you have currently selected.
Unselect: Remove items from the selection set.
Select All: This is not the same as ―Utility Menu → Select → Everythingǁ. This selects all of
whatever entity you have specified at the top of the dialog.
Invert: Reverses the selected and unselected entities (just the entities specified at the top of the
dialog).
OK: This does the select operation (or brings up a picker dialog so that you can pick with the
mouse) and then dismisses the dialog.
Apply: This does the operation but keeps the dialog box. Typically use this so the dialog stays
active.
Replot: Replots whatever is active in the graphics window.
Plot: Plots only the entity specified at the top of the dialog.
Organizing Your Model Using Components:
If you select a group of entities and think that you might want to use that selection set again,
create a component out of it. Components are groups of entities but hold only one kind of entity
at a time. Components can themselves be grouped into Assemblies, so this is how you group
different types of entities together. Use ―Utility Menu → Select → Comp/Assembly → Create

Component…ǁ to create a component. The new Component Manager in Release 8.0 makes it
very easy to manage and manipulate groups and select/plot what you want to see to the screen.
This is found under ―Utility Menu → Select → Component Managerǁ
Creating a Material:
Create the material properties for your model in
―Main Menu → Preprocessor → Material Props → Material Modelsǁ. This gives you this
dialog box where all materials can be created,
Double click on items in the right hand pane of this window to get to the type of material model
you want to create. All properties can be temperature dependant. Click OK to create the material
and it will appear in the left hand pane. Create as many different materials as you need for your
analysis.
Selecting an Element Type:
ANSYS has a large library of element types. Why so many? Elements are organized into groups
of similar characteristics. These group names make up the first part of the element name
(BEAM, SOLID, SHELL, etc). The second part of the element name is a number that is more or
less (but not exactly) chronological. As elements have been created over the past 30 years the
element numbers have simply been incremented. The earliest and simplest elements have the
lowest numbers (LINK1, BEAM3, etc), the more recently developed ones have higher numbers.
The ―18xǁ series of elements (SHELL181, SOLID187, etc) are the newest and most modern in
the ANSYS element library.
Tell ANSYS what elements you are going to use in your model using ―Main Menu → Element
Type → Add/Edit/Deleteǁ
Later, when meshing or creating elements manually you will need to tell ANSYS what type
of elements you want to create.

Creating Properties A solid element (brick or tet) knows its thickness, length, volume, etc by
virtue of its geometry, since it is defined in 3D space. Shell, beam and link (truss) elements do
not know this information since they are a geometric idealization or engineering abstraction.
Properties in ANSYS are called Real Constants. Define real constants using ―Main Menu →
Real Constants → Add/Edit/Deleteǁ.
Creating the Finite Elements Model - Meshing:
If you are just starting out in FEA, it is important to realize that your geometry (called the solid
model in ANSYS) is not your finite element model. In the finite element method we take an
arbitrarily complex domain, impossible to describe fully with a classical equation, and break it
down into small pieces that we can describe with an equation. These small pieces are called
finite elements. We essentially sum up the response of all these little pieces into the response of
our entire structure The solver works with the elements. The geometry we create is simply a
vehicle used to tell ANSYS where we want our nodes and elements to go. While you can create
nodes and elements one by one in a manual fashion (called direct generation in ANSYS) most
people mesh geometry because it is much another very good reason we mesh geometry is that
we assign materials and properties to that geometry.
Then any element created on or in that geometric entity gets those attributes. If we don‘t like the
mesh we can clear it and re-mesh, without having to re-assign the attributes.
Steps for Creating the Finite Elements:
∑ Assign Attributes to Geometry (materials, real constants, etc).
∑ Specify Mesh Controls on the Geometry (element sizes you wa
∑ Mesh.
Most of the meshing operations can be done within the MeshTool, so that will be examined in
some detail now. Start it from ―Main Menu → Preprocessor → Meshing → MeshToolǁ.

Smart Size is used to automatically pick
the element edge length depending on the
sizes of features in the geometry. It
makes a finer mesh around smaller
Features in order to capture
them adequately.
For example in the mesh below
no sizes were specified at all
except a Smart Size level of 4.
A mapped mesh generates a very regular
grid of elements. This can only be used
on rectangular shaped areas or volumes.
A free mesh will mesh any entity
regardless of shape.
Applying Loads and Boundary Conditions:
Loads and boundary condition can be applied in both the Preprocessor
(―Main Menu → Preprocessor → Loads → Define Loads → Applyǁ), and the Solution
processor
(―Main Menu → Solution → Define Loads → Applyǁ).
1. Select the kind of constraint you want to apply.
2. Select the geometric entity where you want it applied.
3. Enter the value and direction for it.
There is no ―modifyǁ command for loads and B.C.‘s. If you make a mistake simply apply it
again with a new value (the old one will be replaced if it‘s on the same entity), or delete it and
reapply it.
Loads: Forces, pressures, moments, heat flows, heat fluxes, etc.
Constraints: Fixities, enforced displacements, symmetry and anti-symmetry
conditions, temperatures, convections, etc.
Although you can apply loads and boundary conditions to nodes or elements, it‘s generally better
to apply all B.C.‘s to your geometry. When the solve command is issued, they will be
automatically transferred to the underlying nodes and elements. If B.C.‘s are put on the
geometry, you can re-mesh that geometry without having to reapply them

Solving:
Solution is the term given to the actual simultaneous equation solving of the mathematical
model. The details of how this is done internally is beyond the scope of this guideline but is
addressed in a separate ―ANSYS Tipsǁ white paper. For the moment, it is sufficient to say that
the basic equation of the finite element method that we are solving is, [K]{u}={F}
where [K] is the assembled stiffness matrix of the
structure, {u} is the vector of displacements at each
node, and {F} is the applied load vector.
This is analogous to a simple spring and is the essence of small deflection theory.
To submit your model to ANSYS for solving, go to “Main Menu → Solution → Solve →
Current LS”. LS stands for load step. A load step is a loading ―conditionǁ.
This is a single set of defined loads and boundary conditions (And their associated solution
results. More on this in the next section). Within an interactive session the first solve you do is
load step 1, the next solution is load step 2, etc.
If you leave the solution processor after solving to do post-processing for example, the load step
counter gets set back to one. You can also define and solve multiple load steps all at once.
There are several solvers in ANSYS that differ in the way that the system of equations is solved
for the unknown displacements. The two main solvers are the sparse solver and the PCG solver.
If the choice of solvers is left to ―program chosenǁ then generally ANSYS will use the sparse
solver. The PCG (preconditioned conjugate gradient) solver works well for models using all
solid elements. From a practical perspective one thing to consider is that the sparse solver
doesn‘t require a lot of RAM but swaps out to the disk a lot. Disk I/O is very slow. If you have a
solid model and lots of RAM the PCG solver could be significantly faster since the solution runs
mostly in core memory
Postprocessing:
The General Postprocessor is used to look at the results over the whole model at one point in
time. This is the final objective of everything we have discussed so far; finding the stresses,
deflections, temperature distributions, pressures, etc. These results can then be compared to
some criteria to make an objective evaluation of the performance of your design.
The solution results will be stored in the results file as result ―setsǁ. For a linear static
analysis like we are talking about, the correlation between Load Step numbers and Results Set
numbers will be one to one as shown below. Only one set of results can be stored in the
database at a time, so when you want to look at a particular set, you have to read it in from the
results file. Reading it in clears the previous results set from active memory.

To read in a results set from the results file (not needed if you have run only a single load step)
use ―Main Menu → General Postprocessor → Read Results → First Set, or By Pickǁ. Most
results are displayed as a contour plot as shown below. To generate a plot of stresses use ―Main
Menu → General Postproc → Plot Results → Contour Plot → Nodal Solutionǁ, then pick the
stresses you want to see
There are many, many other ways to look at your results data including:
• Listing them to a file.
• Querying with the mouse to find a result at a particular node.
• Graphing results along a path.
• Combining different load cases.
• Summing forces at a point.
• Extracting data and storing it an APDL array that you can do further operations.
Animate any result on the deformed shape with ―Utility Menu → Plot Ctrls → Animateǁ. This
is very helpful for understanding if your model is behaving in a reasonable way.

Experiment No: 1 Date:
Stress Analysis of Bars of Constant Cross Section Area
AIM:
To perform displacement and stress analysis for the given bar using Ansys simulation and
analytical expressions.
Problem Description:
A steel rod subjected to tension is modeled by one bar element, as shown in figure. Determine
the nodal displacements and the axial stress in each Element and reaction forces. E=2.1x 105
N/
mm2
, 0.3 (Poisson‘s Ratio).
Software Required: Ansys 14.5.
Procedure:
Step 1: Ansys Utility Menu
File - Change Job name
File - Change Title
Step 2: Ansys Main Menu –Preferences
Select –STRUCTURAL - ok
Step 3: Preprocessor
Element type –Add/Edit/Delete –Add –Link –3D finit stn 180 –ok – close.
Real constants –Add –ok –Real constant set no –1 –c/s area –22/7*50**2/4 –ok.
Material Properties –Material Models –Structural –Linear –Elastic –Isotropic –EX –
2.1e5 –ok –close.
Modeling –Create –Nodes –In Active CS –Apply (first node is Created) –x, y, z
location in CS –300, 0, 0 –ok (second node is Created).
Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –ok
(elements are Created through nodes).
Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes- pick node 1 –Apply – DOFs
to be constrained –All DOF –ok.
Define loads –Apply –Structural –Force/Moment –on Nodes - pick node 2 –Apply –

direction of For/Mom –FX –Force/Moment value –1500 (+ve value) –
ok. Solve –Current LS –ok (Solution is done is displayed) –close.
Step 5: General Post Processor
Element table –Define table –Add –‗Results–By data Sequence item‘num–LS–LS1
–ok.
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).
List Results –Elem table Data –Items to be listed –LS1 –ok. (Stress will be
displayed with the element numbers)
List Results –Reaction Solution –items to be listed –All items –ok (reaction forces
will be displayed with the node numbers).
List Results –Nodal Solution –DOF solution –Displacement Vector Sum –ok. (Nodal
solution will be displayed with the node numbers).
List Results –Nodal loads –items to be listed –All items –ok (Nodal loads will be
displayed with the node numbers).
Step 6: PlotCtrls –Animate –Deformed shape –def+ undeformed-ok
PlotCtrls – Animate – Deformed results – DOF solution – Displacement Vector sum
– ok.
Comparison between theoretical and Ansys values:
Ansys Theoretical
Particulars
Node 1 Node 2 Node 1 Node2
Results:
The analysis of the bar was carried out using the Ansys simulation and the
software results were compared with theoretical or analytical results.
Verification/Validation: Verify the Ansys results by increasing number of nodes and
elements to match the theoretical or analytical results.
Conclusions: Ansys simulation and the software results are near to theoretical or
analytical results.

AIM:
A steel rod subjected to tension is modeled by one bar element, as shown in figure. Determine
the nodal displacements and the axial stress in each Element and reaction forces. E=2.1x 10
5
N/
mm
2
,0.3 (Poisson‘s Ratio).
Procedure:
File - Change Title
Real Constants –Add –ok –Real constant set no –1 –c/s area –22/7*60**2/4 –ok.
2.1e5 –PRXY –0.3 –ok –close.
location in CS –450, 0, 0 –ok (second node is Created).
(elements are Created through nodes).
Step 4: Solution

Define loads –Apply –Structural –Force/Moment –on Nodes- pick node 2 –Apply
– direction of For/Mom –FX –Force/Moment value –2500 (+ve value) –ok.
Solve –Current LS –ok (Solution is done is displayed) –close.
Element table –Define table –Add –‗Results–BydataSequence item‘num–LS–LS1-ok.
List Results –Elem table Data –Items to be listed –LS1 –ok. (Stress will be
displayed with the element numbers)
Step 6: PlotCtrls –Animate –Deformed shape –def+undeformed-ok
PlotCtrls – Animate – Deformed results – DOF solution – Displacement Vector sum
– ok.
Ansys Theoretical
Particulars
Node 1 Node 2 Node 1 Node2
Results:

Conclusion: Ansys simulation and the software results are near to theoretical or
analytical results.
AIM:
A steel rod subjected to compression is modeled by two bar elements, as shown in figure.
Determine the nodal displacements and the axial stress in each Element. E=207 GPa,
A = 500 mm
2
Procedure:
File - Change Title
Real constants –Add –ok –Real constant set no –1 –c/s area –500 –ok.
Material Properties –Material models –Structural –Linear –Elastic –Isotropic –EX
– 207e3 –ok –close.
location in CS –500, 0, 0 –Apply (second node is Created) - x, y, z location in CS –
1000, 0, 0 (third node is Created).
Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –Apply -
pick 2 & 3 (elements are Created through nodes).
Step 4: Solution

– direction of For/Mom –FX –Force/Moment value –- 12000 (-ve value) –ok.
Element table –Define table –Add –‗Results–BydataSequence item‘num–LS–LS1–ok.
Step 6: PlotCtrls –Animate –Deformed shape –def+undeformed-ok.
Theoretical
Ansys
Particulars
Node 1 Node 2 Node 3 Node 1 Node2
Deformation
Stress
Reaction
Results:
Verification/Validation: Verify the Ansys results by increaing number of nodes and
analytical results.

AIM:
A load of P = 60 x 10
3
N is applied as shown. Determine the following, a) Nodal
Displacement, b) Stress in each member, c) Reaction Forces.
Given Data: E=20 x10
3
N/mm
2
.0.3 (Poisson‘sRatio)
Procedure:
File - Change Title
Real Constants –Add –ok –Real constant set no –1 –c/s area –250 –ok.
20e3 –ok –close.
location in CS –150, 0, 0 –Apply (second node is Created) - x, y, z location in CS –300,
0, 0 (third node is Created).
Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –Apply - pick
2 & 3 (elements are Created through nodes).
Step 4: Solution
– DOFs to be constrained –UX –VALUE - Displacement Value –1.2 - ok.

DEPARTMENT OF MECHANICAL ENGINEERING GCEM
– direction of For/Mom –FX –Force/Moment value –60e3 (+ve value) –ok.
Element table –Define table –Add –‗Results–BydataSequence item‘num–LS–LS1
–ok.
Particulars
Ansys Theoretical
Node1 Node2 Node3 Node1 Node2 Node3
Deformation
Stress
Reaction
Results:
analytical results.

Stress Analysis of Bars of Tapered Cross Section Area
AIM:
To perform displacement and stress analysis for the given Taper bar using Ansys
simulation and analytical expressions.
For the tapered bar shown in the figure determine the displacement, stress and reaction in
the bar. Given A1 = 1000 mm
2
and A2 = 500 mm
2
, E = 2x10
5
N/mm
2
The Tapered bar is modified into 2 elements as shown below with modified area of cross
section (1000+500)/2 = 750 mm
2
Areas of modified two elements:
A`1= (1000+750)/2 = 875 mm
2
A`2= (750+500)/2 = 625 mm
2
Procedure:
File - Change Title
Real constants –Add –ok –Real constant set no –1 –c/s area –875 –ok. Add –ok –
Real constant set no –2 –c/s area 625– ok.
– 2e5 –ok –close.
Modeling –Create –Nodes –In Active CS –Apply (first node is Created) –x, y, z location in
CS –187.5, 0, 0 –Apply (second node is Created) - x, y, z location in CS – 375, 0, 0

(third node is Created).
Step 4: Solution
Particulars
Ansys Theoretical
Node1 Node2 Node3 Node1 Node3
Deformation
Stress
Reaction
Results:
analytical results.

Stress Analysis of Bars Varying In Cross Section or Stepped Bars
AIM:
To perform displacement and stress analysis for the given stepped bar using Ansys
Consider the stepped bar shown in figure below. Determine the nodal displacement stress in
each element, reaction forces.
Procedure:
File - Change Title
Element type –Add/Edit/Delete –Add –Link –3D finit stn 180 –ok –close.
Real constants –Add –ok –Real constant set no –1 –c/s area –900 –ok. Add –ok –
Real constant set no –2 –c/s area 600–ok.
2e5 –ok,
Material –New model –Define material ID –2 –ok –Structural –Linear –Elastic
– Isotropic –EX –0.7e5 –ok –close.
Step 4: Solution

Define loads –Apply –Structural –Displacement –on Nodes- pick node 1 –Apply –
DOFs to be constrained –All DOF –ok.
Define loads –Apply –Structural –Force/Moment –on Nodes - pick node 3 –Apply
Particulars
Ansys Theoretical
Deformation
Stress
Reaction
Results:
analytical results.

AIM:
Find nodal displacement, stress in the element & reaction forces for the following
problem. Given Data: E = 2x 10
5
N /mm
2
, g= 0.3 (Poisson‘s Ratio).A1 = 40 mm
2
, A2
= 20 mm
2
Procedure:
File - Change Title
Real constants –Add –ok –Real constant set no –1 –c/s area –40 –
ok. Add –ok –Real constant set no –2 –c/s area
– 20 –ok.
Material Properties –Material models –Structural –Linear –Elastic –Isotropic –EX –
2e5 –ok - close
Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –Apply
- pick 2 & 3 (elements are Created through nodes).
Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes - pick node 1 –Apply –

DOFs to be constrained –All DOF –ok.
– direction of For/Mom –FX –Force/Moment value –1000 (-ve value) –ok.
Element table –Define table –Add –‗Results–BydataSequence item‘num–LS–LS1
–ok.
Particulars
Ansys Theoretical
Deformation
Stress
Reaction
Results:
analytical results.

AIM:
Find nodal displacement, stress in each element & reaction forces for the following problem Given
Data: 1) E1 =70x103
N/mm2
, A1 = 2400 mm2
. 2) E2= 200 x 103
N / mm2
, A2 = 600 mm2
,g= 0.3 (Poisson‘s Ratio)
Procedure:
File - Change Title
Real constants –Add –ok –Real constant set no –1 –c/s area –
2400 –ok. Add –ok –Real constant set no –2 –
c/s area –600 –ok.
Material Properties –Material Models –Structural –Linear –Elastic –Isotropic
–EX – 70e3 –PRXY –0.3 - ok
Material –New model –Define material ID –2 –ok –Structural –Linear –Elastic
– Isotropic –EX –200e3 –PRXY –0.3 - ok –close.
Modeling –Create –Nodes –In Active CS –Apply (first node is Created) –x,
y, z location in CS –300, 0, 0 –Apply (second node is Created) - x, y, z
location in CS –700, 0, 0 (third node is Created).
Elements Attributes- Change Real Constant Set No 2 & Material No 2- Ok- Elements –
Auto Numbered - Thru Nodes - Pick 2 & 3 Node-Apply-0k.
COMPUTER AIDED MODELING 45 VI SEMESTER
AND ANALYSIS LAB (10MEL68)

Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes- pick node 1 & 3 –Apply
–DOFs to be constrained –All DOF –ok.
Element table –Define table –Add –‗Resultem‘s–BydataSequence inum –LS –LS1
–ok.
Particulars
Ansys Theoretical
Deformation
Stress
Reaction
Results:
analytical results.

AIM:
Consider the bar loaded as shown. Determine the following
1)Nodal displacement, 2)Stress in the element, 3)Reaction forces. Given Data: P = 300 KN, E =
200x10
9
N/m
2
. g= 0.3 (Poisson‘s Ratio) ,A1 = 250 mm
2
, A2 = 400 mm
2
Procedure:
File - Change Title
Real Constants –Add –ok –Real constant set no –1 –c/s area
–250 –ok Add –ok –Real constant set no –
2 –c/s area –400 –ok
Material Properties –Material Models –Structural –Linear –Elastic –
Isotropic –EX – 200e3 –PRXY –0.3 - ok
Modeling –Create –Nodes –In Active CS –Apply (first node is Created) –
x, y, z location in CS –150, 0, 0 –Apply (second node is Created) - x, y, z
location in CS –300, 0, 0 –Apply (third node is Created), x, y, z location in
CS –600, 0, 0 –ok (fourth node is Created).
Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –
Apply - pick 2 & 3 –ok.
Modeling –Create –Elements –Element Attributes –Change Real Constant Set No 2 –
ok - pick 3 & 4 (elements are Created through nodes).

Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes - pick node 1 & 4 –Apply
–DOFs to be constrained –All DOF –ok.
– direction of For/Mom –FX –Force/Moment value –300e3 (+ve value) –ok.
List Results –Reaction solution –items to be listed –All items –ok (reaction forces
List Results –Nodal solution –DOF solution –Displacement Vector Sum –ok. (Nodal
Particulars
Ansys Theoretical
Node1 Node2 Node3 Node4 Node1 Node2 Node3 Node4
Deformation
Stress
Reaction
Results:
analytical results.

AIM:
An axial load P = 300 x 10
3
N is applied at 20 °C to the rod as shown. The temperature is
raised to 60
0
c. Determine the nodal displacement, stress in the element, reaction forces.
Given Data:
1: Aluminum: 2: Steel:
E = 70 x 10
9
N / m
2
. E = 200x10
9
N/m
2
g= 0.3 (Poisson‘sRatio)
A = 900 mm
2
A = 1200 mm
2
a = 23 x10
-6
°C a = 11.7 x10
-6
°c
Procedure:
File - Change Title
Real constants –Add –ok –Real constant set no –1 –c/s area –900 –ok
Add –ok –Real constant set no –2 –c/s area –1200 –ok –close.
Material Properties –Material models –Structural –Linear –Elastic –Isotropic –EX –
70e3 –PRXY –0.3 –ok
Thermal Expansion - Secant Coefficient - lsotropic - ALPX-23E-6 –ok.
Material - Define material ID –2 –ok ––Structural –Linear –Elastic –Isotropic –EX
– 200e3 –PRXY –0.3 –ok
Thermal Expansion-Secant Coefficient - lsotropic –ALPX -11.7E-6-Ok
location in CS –200, 0, 0 –Apply (second node is Created) - x, y, z location in CS –500,
0, 0 –Apply (third node is Created)

Modeling –Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –ok -
Elements Attributes- Change Real Constant Set No 2 & Material No 2- Ok- Elements –
Auto Numbered - Thru Nodes - Pick 2 & 3 Node -Apply- 0k.
Step 4: Solution
Define loads –Settings –Reference Temperature –20 - Ok.
Define Loads - Apply-Structural –Temperature - On Elements - Select Both Elements -
Apply - VAL 1 Temperature at Location N = 60 –ok.
Define Loads - Apply - Structural - Displacement –On Nodes - Pick Node No 1 & 3 -
Apply -All DOF -Apply - OK.
Define Loads –Apply –Structural - Force / Moments –On Nodes - Pick 2
nd
Node
- Apply - Select FX = 300e3 - Apply - Ok.
Element Table - List Element Table - Select Stress - Ok.
Particulars
Ansys Theoretical
Node1 Node2 Node3 Node4 Node1 Node2 Node3 Node4
Deformation
Stress
Reaction
Results:
The analysis of the stepped bar was carried out using the Ansys simulation and the

analytical results.

EXPT;11 Stress analysis of Beams
AIM:
Draw the shear force and bending moment diagrams for the given beam due to applied
load .
Compute the Shear force and bending moment diagrams for the beam shown. Assume
rectangular c/s area of 0.2 m * 0.3 m, Young‘s modulus of 210 GPa, Poisson‘s ratio 0.27.
Procedure:
File - Change Title
Element type –Add/Edit/Delete –Add –BEAM –2 noded 188 –ok- close.
Isotropic –EX – 210e3 –PRXY –0.27 –ok –close.
Sections –Beam –Common Section –B = 200, H = 300 –ok.
Modeling –Create –Nodes –In Active CS –Apply (first node is created) –
x, y, z location in CS –5000, 0, 0 –ok (second node is Created).
Create –Elements –Auto numbered –Thru Nodes –pick 1 & 2 –ok
(elements are created through nodes).
Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes - pick node 1 –
Apply – DOFs to be constrained –ALL DOF –ok.
Define loads –Apply –Structural –Force/Moment –on Nodes - pick node 2
–Apply – direction of For/Mom –FY –Force/Moment value - -10000 (-ve
value) –ok.

Plot Results –Contour plot –Nodal solu –DOF solution –displacement vector sum –
ok.
Element table –Define table –Add –‗Results–BydataSequence item‘num–SMISC
–SMISC, 6 –Apply, By Sequence num –SMISC –SMISC, 19 –Apply, By Sequence num –
SMISC –SMISC, 2 –Apply, By Sequence num –SMISC –SMISC, 15 –ok – close.
NOTE: For Shear Force Diagram use the combination SMISC 6 & SMISC 19,
for Bending Moment Diagram use the combination SMISC 3 & SMISC 16.
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).
–Elem table item at node J –SMIS15 –ok (bending moment diagram will be displayed).
List Results –reaction solution –items to be listed –All items –ok (reaction forces
Step 6: PlotCtrls –Animate –Deformed results –DOF solution –USUM –ok.
Comparison b/w Theoretical & Ansys Results
Theoretical
Particulars Maximum Minimum Maximum Minimum
Shear force
Bending Moment
Results:
The analysis of the cantilever Beam was carried out using the Ansys simulation
and the software results were compared with theoretical or analytical results.
analytical results.

Stress analysis of Beams
AIM:
load.
Compute the shear force and bending moment diagrams for the beam shown Assume
rectangular c/s area of 0.2 m * 0.3 m, Young‘s modulus of 210 GPa, Poisson‘s ratio 0.27.
Procedure:
File - Change Title
Select –STRUCTURAL –ok
Modeling –Create –Keypoints –In Active CS –Apply (first node is
Created) –x, y, z location in CS –2000, 0, 0 - Apply (second node is
Created) –4000, 0, 0 –ok - (third node is Created).
Modeling –Create –Lines –Straight lines–In Active Coord –pick
keypoints 1 & 2, pick keypoints 2 & 3 –ok.
Meshing –Size cntrls –Manual size –Global –Size –Element edge length –5 –ok.
Meshing –Mesh –Lines –Pick all –ok.
Step 4: Solution
Define loads –Apply –Structural –Displacement –on keypoint - pick keypoint 1 – Apply
–DOFs to be constrained –UX, UY, UZ, ROTX, ROTY –Apply –pick keypoint 3 –Apply

–DOFs to be constrained –UY–ok.
Define loads –Apply –Structural –Force/Moment –on keypoint - pick keypoint 2 –
Apply –direction of For/Mom –FY –Force/Moment value –-20e3 (-ve value) –ok.
Plot Results –Contour plot –Nodal solu –DOF solution –displacement vector sum -ok.
–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.
Plot Results –Contour plot –Line Element Results –Elem table item at node I –SMIS3–
Elem table item at node J –SMIS16 –ok (Bending moment diagram will be displayed). List
Results –reaction solution –items to be listed –All items –ok (Reaction forces will
be displayed with the node numbers).
Ansys Theoretical
Particulars
Maximum Minimum Maximum Minimum
Shear force
Bending Moment
Results:
The analysis of the cantilever Beam was carried out using the Ansys simulation
and the software results were compared with theoretical or analytical results.
analytical results.

Experiment No: 13
AIM:
load.
Draw the shearforce and bending moment diagram for the beam loaded as shown in figure.
Assume rectangular c/s area of 0.2 m * 0.3 m, E = 200GPa, Poisson‘s ratio = 0.3, Length (L) =
2m, q = 10kN/m.
Procedure:
File - Change Title
Material Properties –Material models –Structural –Linear –Elastic –
Modeling –Create –Keypoints –In Active CS –Apply (first node is Created)
–x, y, z location in CS –2000, 0, 0 –ok (second node is Created).
Modeling –Create –Lines –Straight lines–in Active Coord –pick keypoints 1 & 2, pick
ok.
Meshing –Size Cntrls –Manual size –Global –Size –No of element divisions –100 –ok.
Step 4: Solution
Define loads –Apply –Structural –Displacement –on keypoint - pick keypoint
1 – Apply –DOFs to be constrained –UX, UY, UZ, ROTX, ROTY –Apply –
pick keypoint 2 –Apply –DOFs to be constrained –UY–ok.

Define loads –Apply –Structural –on beams –select full line –Load key –2 - Pressure
value at node I –10e3 - ok.
Plot Results –Contour plot –Nodal solu –DOF solution –displacement vector sum –ok.
–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.
Ansys Theoretical
Minimum Maximum Minimum
Shear force
Bending Moment
Results:
The analysis of the Simply Supported Beam was carried out using the Ansys
simulation and the software results were compared with theoretical or analytical
results.
analytical results

Experiment No: 14
AIM:
load.
Draw the shear force and bending moment diagram for the beam loaded as shown in figure.
Assume rectangular c/s area of 0.2 m * 0.3 m, E = 200GPa, Poisson‘s ratio = 0.3.
Procedure:
File - Change Title
Material Properties –Material models –Structural –Linear –Elastic –
Modeling –Create –Keypoints –In Active CS –Apply (first node is Created)
–x, y, z location in CS –4000, 0, 0 - Apply (second node is Created) –6000,
0, 0 –ok - (third node is Created) - 8000, 0, 0 –ok - (fourth node is Created).
Modeling –Create –Lines –Straight lines–in Active Coord –pick keypoints 1
& 2, pick keypoints 2 & 3, pick keypoints 3 & 4 –ok.
Meshing –Size cntrls –Manual size –Global –Size –Element edge length –5 –ok.
Step 4: Solution

Define loads –Apply –Structural –on beams –select box option –select from
1
st
keypoint to 2
nd
–Load key –2 - Pressure value at node I –20e3 - ok.
List Results –Reaction solution –items to be listed –All items –ok (reaction forces
Comparison b/w Theoretical & Ansys
Ansys Theoretical
Shear force
Bending Moment
Results: The analysis of the Simply Supported Beam was carried out using the
Ansys simulation and the software results were compared with theoretical or
analytical results.
analytical results

AIM:
load.
Draw the shear force and bending moment diagram for the beam loaded as shown in figure.
Assume rectangular c/s area of 0.2 m * 0.3 m, E = 200GPa,
Poisson‘s ratio = 0.3.
Procedure:
File –clear and start new –do not read file –ok –yes.
– 200e3 –PRXY –0.3 –ok –close.
Modeling –Create –Keypoints –In Active CS –Apply (first node is Created) –x, y, z
location in CS –2000, 0, 0 - Apply (second node is Created) –4000, 0, 0 –ok - (third
node is Created) - 10000, 0, 0 –ok - (fourth node is Created).
Modeling –Create –Lines –Straight lines–in Active Coord –pick keypoints 1 & 2, pick
keypoints 2 & 3, pick keypoints 3 & 4 –ok.
Meshing –Size cntrls –Manual size –Global –Size –No of element divisions –100 –ok.
Step 4: Solution

Define loads –Apply –Structural –on beams –select box option –select from 1
st
keypoint to
2
nd
–Load key –2 - Pressure value at node I –0 - Pressure value at node J –5e3 - ok.
Ansys Theoretical
Shear force
Bending Moment
Results:
The analysis of the Simply Supported Beam was carried out using the Ansys
simulation and the software results were compared with theoretical or analytical
results.
analytical results

Stress Analysis of a Rectangular Plate with a circular Hole
AIM:
To determine the stress acting on a rectangular plate with a circular hole due to
the applied external load.
In the plate with a hole under plane stress, find deformed shape of the hole and determine
the maximum stress distribution along A-B. E = 210GPa, t = 1 mm, Poisson‘s0.3,
Diameter of the circle =10 mm.
2000 N
40 mm
60 mm
Procedure:
File - Change Title
Select –STRUCTURAL –ok
Element type –Add/Edit/Delete –Add –Solid –Quad 4 node 182 –ok –Option – element
behavior K3 –Plane stress with thickness –ok –close.
Real constants –Add –ok –Real constant set no –1 –Thickness –1 –ok.
Material Properties –material models –Structural –Linear –Elastic –Isotropic –EX –
210e3 –PRXY –0.3 –ok –close.

Modeling –Create –Area –Rectangle –by dimensions –X1, X2, Y1, Y2 –0, 60, 0, 40
–ok.
Modeling –Create –Area –Circle –solid circle –X, Y, radius –30, 20, 5 –ok.
Modeling –Operate –Booleans –Subtract –Areas –pick area which is not to be
deleted (rectangle) –Apply –pick area which is to be deleted (circle) –ok.
Meshing –Mesh Tool –Mesh Areas –Quad –Free –Mesh –pick all –ok.
Meshing –Mesh Tool –Refine–pick all –Level of refinement –3 –ok.
Step 4: Solution
Define loads –Apply –Structural –Displacement –on Nodes –select box –drag the
left side of the area –Apply –DOFs to be constrained –ALL DOF
Define loads –Apply –Structural –Force/Moment –on Nodes –select box –drag the
right side of the area –Apply –direction of For/Mom –FX –Force/Moment value –
2000 (+ve value) –ok.
Plot results –Contour plot –Element solu –Stress –Von Mises Stress –ok (the
stress distribution diagram will be displayed).
Step 6: PlotCtrls –Animate –Deformed shape –def+undeformed-ok
Result: Thus the performance of the stress analysis of a Rectangular Plate with a circular
hole was analyzed and animated.
analytical results

Casa lab manual

More Related Content

What's hot (20)

Similar to Casa lab manual (20)

Recently uploaded (20)

Casa lab manual