Stress Analysis

Overview

Stress analysis is a general term used to describe analyses

where the results quantities include stresses and strains. It
is also known as structural analysis.

As described in Chapter 2, ANSYS allows several types of

stress analyses:

Module 4

Stress Analysis

Static

Transient Dynamic

Modal

Spectrum

Harmonic

Explicit Dynamics

In this chapter, we will use a linear static analysis to describe

the steps involved in an analysis. By mastering these steps,
you can quickly learn how to do other analyses.

Stress Analysis

Stress Analysis

...Overview

A. Analysis Steps

Every analysis involves three main steps:

Topics covered:
A. Analysis Steps

B. Geometry

Create or import the model geometry

C. Meshing
D. Loading
E. Solve

Preprocessing

Mesh the geometry

Solution
Apply loads

F. Reviewing Results

Solution

Solve

G. Checking Validity of Solution

H. Workshop

Preprocessing

Postprocessing
Review results
Check the validity of the solution

Postprocessing

Stress Analysis

Stress Analysis

...Analysis Steps

...Analysis Steps

The preprocessor (called PREP7 in ANSYS) is where you

provide the majority of the input to the program.

Its main purpose is to generate the finite element model,

which consists mainly of nodes, elements, and material
property definitions. You can also use PREP7 to apply loads.

Usually begins with definition of the model geometry.

A solid model model is typically used to represent model

geometry.

Notice that the ANSYS Main Menu is also organized in terms

of preprocessing, solution, and postprocessing.

A CAD-type mathematical representation that defines the

geometry of the structure.
May consist of solids or just surfaces, depending on what is
being modeled.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

B. Geometry

...Geometry

Volumes are bounded by areas. They represent solid objects.

Areas are bounded by lines. They represent faces of solid
objects, or planar or shell objects.
Lines are bounded by keypoints. They represent edges of
objects.
Keypoints are locations in 3-D space. They represent vertices of
objects.

There is a built -in hierarchy among solid model

entities. Keypoints are the foundation entities.
Lines are built from the keypoints, areas from
lines, and volumes from areas.

Lines & Keypoints

Lines
Keypoints

This hierarchy holds true regardless of how the

solid model is created.

ANSYS will not allow you to delete or modify a lower-order

entity if it is attached to a higher-order entity. (Certain types
of modifications are allowed discussed later.)
Volumes
Areas
Lines
Keypoints

OOPs!

Lines
Keypoints

Areas

Areas

Areas

Ill just
change
this line

Volumes

Volumes

es
lum
Vo

A typical solid model is defined by volumes, areas, lines, and

keypoints.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Geometry

...Geometry

You can either create a solid model in ANSYS or import it

from another software package.

Details of both methods will be presented later. For now, we

will briefly discuss how to import an IGES file and scale the
geometry if needed.

IGES (Initial Graphics Exchange Specification) is a way to

transfer solid model geometry from one software package to
another.

To import an IGES file into ANSYS:

Utility Menu > File > Import > IGES...
In the resulting dialog box, choose the
No defeaturing * (default) and press OK
(defaults for everything else).
In the second dialog box, choose the
desired file and press OK.
OR use the IGESIN command:
/aux15

An IGES file is ASCII, allowing it to be easily transported

between computer systems.

ioptn,iges,nodefeat
igesin,filename,extension,directory

Most packages, including ANSYS, allow you to write as well as

read an IGES file.

finish

* Details about the No Defeaturing vs. Defeaturing method and the other options will be presented later.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Geometry

...Geometry

When the import is completed, ANSYS will automatically plot

the geometry.

Scaling is typically needed when you want to convert the geometr y

to a different set of units, say from inches to millimeters.

You may then modify the

geometry as needed.

To scale a model in ANSYS:

ANSYS allows many

operations on the solid
model, which will be
describe later.
For now, we will discuss
how to scale the model to a
different set of units. (Note:
Scaling is NOT available for
a Defeature IGES import.)

First save the database --Toolbar >

SAVE_DB or SAVE command.
Then Main Menu > Preprocessor >
Operate > Scale > Volumes (choose the
highest-level entity available in the
model)
[Pick All] to pick all volumes
Then enter desired scale factors
for RX, RY, RZ and set IMOVE to
Moved instead of Copied
Or use the VLSCALE command:
vlscale,all,,,25.4,25.4,25.4,,,1

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Geometry

...Geometry

Demo:
Import pipe.igs using:
No Defeaturing method
All other defaults
Orient the model as shown

Preprocessing
3 Geometry
Meshing

Save as pipe.db

Solution
Loading
Solve

Postprocessing
Review results
Check validity of solution

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

C. Meshing

...Meshing

Meshing is the process used to fill the solid model with

nodes and elements, i.e, to create the FEA model.

There are three steps to meshing:

Define element attributes

Remember, you need nodes and elements for the finite element
solution, not just the solid model. The solid model does NOT
participate in the finite element solution.

Specify mesh controls

Generate the mesh

Element attributes are characteristics of the finite element

model that you must establish prior to meshing. They
include:
Element types

meshing
Solid model

Real constants
FEA model

Material properties

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Element Type

To define an element type:

Preprocessor > Element Type >
Add/Edit/Delete

The element type is an important choice that determines the

following element characteristics:

[Add] to add new element

type

Degree of Freedom (DOF) set. A thermal element type, for

example, has one dof: TEMP , whereas a structural element type
may have up to six dof: UX, UY, UZ, ROTX, ROTY, ROTZ.

Choose the desired type

(such as SOLID92) and
press OK

Element shape -- brick, tetrahedron, quadrilateral, triangle, etc.

Dimensionality -- 2-D (X -Y plane only), or 3 -D.

[Options] to specify
additional element options

Assumed displacement shape -- linear vs. quadratic.

Or use the ET command:

ANSYS has a library of over 150 element types from which

you can choose. Details on how to choose the correct
element type will be presented later. For now, lets see how
to define an element type.

et,1,solid92

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Real Constants

Notes:
Setting preferences to the desired discipline (Main Menu >
Preferences) will show only the element types valid for that
discipline.
You should define the element type early in the preprocessing
phase because many of the menu choices in the GUI are filtered
out based on the current DOF set. For example, if you choose a
structural element type, thermal load choices will be grayed
out or not shown at all.

Real constants are used for geometric properties that cannot

be completely defined by the elements geometry. For
example:
A beam element is defined by a line joining two nodes. This
defines only the length of the beam. To specify the beams
cross -sectional properties, such as the area and moment of
inertia, you need to use real constants.
A shell element is defined by a quadrilateral or triangular area.
This defines only the surface area of the shell. To specify the
shell thickness, you need to use real constants.
Most 3-D solid elements do not require a real constant since the
element geometry is fully defined by its nodes.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Material Properties

To define real constants:

Preprocessor > Real Constants

Every analysis requires some material property input:

Youngs modulus EX for structural elements, thermal
conductivity KXX for thermal elements, etc.

There are two ways to define material properties:

[Add] to add a new real constant set.

If multiple element types have been defined, choose the
element type for which you are specifying real constants.
Then enter the real constant values.
Or use the R family of commands.

Material library
Individual properties

Different element types require different real constants, and

some dont require any real constants. Check the Elements
Manual, available on-line, for details.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Using the Material Library

This method allows you to choose a predefined set of properties for

a given material.

ANSYS supplies typical structural and thermal properties (linear

only) for some common materials, but we strongly recommend that
you create your own material library.

To choose a material from the library:

First define the library path.
Preprocessor > Material Props >
Material Library > Library Path
Enter the location from which
to READ material data, e.g,
/ansys57/matlib.
Or use the /MPLIB command.

Then import a material from the

library.
Preprocessor > Material Library >
Import Library
Choose the units system.
This is used only to filter the
list of files shown in the
subsequent dialog. ANSYS
has no knowledge of units
and does NOT do unit
conversion.
Choose the desired material
file, such as steel AISI C1020.
Or use the MPREAD command
with the LIB option.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Specifying Individual Material Properties

Work through the tree

structure to the material
type to be defined.

Then enter the individual

property values.

Or use the M P command.

Instead of choosing a material name, this method involves directly

specifying the required properties through the Material Model GUI.

To specify individual
properties:
Preprocessor > Material
Props > Material Models

mp,ex,1,30e6
mp,prxy,1,.3

Double -click on the

appropriate
property to be
defined.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

Add temperature dependent

properties

Copy material models from

one table to another

Graph properties v.
temperature

Delete material models

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

A Note on Units

Specifying Mesh Controls is the second step in meshing.

You do not need to tell ANSYS the system of units you are
using. Simply decide what units you will use, then make sure
all of your input is consistent.

Many mesh controls are available in ANSYS. For now, we will

present a simple method of specifying mesh density, called
SmartSizing.

For example, if the model geometry is in inches, make sure that

all other input data material properties, real constants, loads,
etc. are in terms of inches.

SmartSizing is an algorithm that assigns element divisions to

all lines in the model based on line length, curvature, and
proximity to holes, etc.

You simply specify a size level ranging from 1 (very fine

mesh) to 10 (very coarse mesh), and ANSYS takes care of the
rest.

ANSYS does NOT do units conversion! It simply accepts all

numbers you input without questioning their validity.

The command /UNITS allows you to specify a units system,

but it is simply a recording device to let other users of your
model know what units you used.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

...Meshing

The MeshTool is the best way to specify mesh

controls:
Preprocessor > MeshTool.
Activate SmartSizing. Size level defaults to 6.

When the meshing is complete, ANSYS will automatically plot

the elements.
The default element plot shows all element edges as straight
lines even for a quadratic element type.
To show curved element edges, issue /EFACET,2 (or Utility Menu
> PlotCtrls > Size and Shape).

Generating the mesh is the final step in meshing.

First save the database.

Then press [Mesh] in the MeshTool.

This brings up a picker. Press [Pick All] in the picker to
indicate all entities.

Stress Analysis - Preprocessing

Stress Analysis - Preprocessing

...Meshing

Meshing

Demo:

3 Meshing

Define SHELL63 element type

Specify real constant thickness = 1/8 in

Preprocessing
3 Geometry

Resume pipe.db (if needed)

Use the Material Model GUI to define Material 1:

Solution
Loading

Structural, Linear, Elastic, Isotropic

Solve

Youngs modulus EX = 30e6

Poissons ratio PRXY = .3

Postprocessing

Save as pipe.db, then mesh the model using SMRT,4

Review results

Save as pipemesh.db

Check validity of solution

Stress Analysis - Solution

Stress Analysis - Solution

D. Loading

...Loading

The solution step is where we apply loads on the object and

let the solver calculate the finite element solution.

Loads are available both in the Solution and Preprocessor

menus.

There are five categories of loads:

DOF Constraints

Specified DOF values, such as

displacements in a stress analysis or
temperatures in a thermal analysis.

Concentrated Loads

Point loads, such as forces or heat flow

rates.

Surface Loads

Loads distributed over a surface, such as

pressures or convections.

Body Loads

Volumetric or field loads, such as

temperatures (causing thermal expansion)
or internal heat generation.

Inertia Loads

Loads due to structural mass or inertia,

such as gravity and rotational velocity.

Stress Analysis - Solution

Stress Analysis - Solution

...Loading

...Loading

Regardless of how you apply the loads, the solver expects all
loads to be in terms of the finite element model. Therefore,
solid model loads are automatically transferred to the
underlying nodes and elements during solution.

We will now discuss how to apply the following types of

structural loads:

You can apply loads either on the solid model or directly on

the FEA model (nodes and elements).
Solid model loads are easier to apply because there are fewer
entities to pick.
Moreover, solid model loads are independent of the mesh. You
dont need to reapply the loads if you change the mesh.
Pressure on line

Displacement constraints

Pressures on element faces

Pressures
Gravity
Constraint
on line
Solid model

Force at keypoint

Constraints
at nodes
FEA model

Force at node

Stress Analysis - Solution

Stress Analysis - Solution

...Loading

...Loading

Displacement Constraints

Used to specify where the model is fixed (zero displacement

locations).

Can also be non-zero, to simulate a known deflection.

To apply displacement constraints :

Solution > -Loads- Apply > Displacement
Choose where you want to apply
the constraint.
Pick the desired entities in the
graphics window.
Then choose the constraint
direction. Value defaults to zero.
Or use the D family of commands:
DK, DL, DA, D.

Displacement constraints are also used to enforce symmetry

or antisymmetry boundary conditions.
Symmetry BC: Out-of-plane displacements and in-plane
rotations are fixed.
Antisymmetry BC: In -plane displacements and out-of-plane
rotations are fixed.

Y
X

Symmetry Boundary
UX=0
ROTY=ROTZ=0

Antisymmetry Boundary
UY=UZ=0
ROTX=0

Stress Analysis - Solution

Stress Analysis - Solution

...Loading

...Loading

Pressures

To apply a pressure:
Solution > -Loads- Apply > Pressure
Choose where you want to apply the
pressure -- usually on lines for 2 -D
models, on areas for 3-D models.
Pick the desired entities in the
graphics window.

Then enter the pressure value.

A positive value indicates a
compressive pressure (acting
towards the centroid of the
element).

For a 2-D model, where

pressures are usually applied
on a line, you can specify a
tapered pressure by entering a
value for both the I and J ends
of the line.
I and J are determined by the
line direction. If you see the
taper going in the wrong
direction, simply reapply the
pressure with the values
reversed.

500

VALI = 500
1000
500
L3
VALI = 500
VALJ = 1000
1000

VALI = 1000
VALJ = 500

Stress Analysis - Solution

Stress Analysis - Solution

...Loading

...Loading

Gravity

Verifying applied loads

Solution > -Loads- Apply > Gravity

Notes:
A positive acceleration value causes deflection in the negative
direction. If Y is pointing upwards, for example, a positive
ACELY value will cause the structure to move downwards.
Density (or mass in some form) must be defined for gravity and
other inertia loads.

Plot them by activating load symbols:

Utility Menu > PlotCtrls > Symbols

Or use the ACEL command.

500
L3

Or use the S F family of commands:

SFL, SFA, SFE, SF.

To apply gravitational acceleration:

500
L3

Commands -- /PBC, /PSF, /PBF

Or list them:
Utility Menu > List > Loads >

Stress Analysis - Solution

Stress Analysis - Solution

...Loading

...Loading

Modifying and Deleting Loads

To modify a load value, simply reapply the load

with the new value.

To delete loads:

3 Geometry
3 Meshing

Solution
3 Loading

Solution > -Loads- Delete >

When you delete solid model loads, ANSYS also
automatically deletes all corresponding finite
element loads.

Preprocessing

Solve

Postprocessing
Review results
Check validity of solution

Stress Analysis - Solution

Stress Analysis - Solution

E. Solve

Solve

The solve step is where you let the solver calculate the finite
element solution.

First, it is a good idea to review and check your analysis data,

e.g:

First save the database!

Then:
Solution > -Solve - Current LS

Consistent units
Element types, options, and real constants
Material properties
Density if inertia loading
Coefficient of thermal expansion for thermal stress
Mesh density, especially in stress concentration regions
Load values and directions
Reference temperature for thermal expansions

To initiate the solve:

Or issue the SOLVE command.

The solver writes results data to the in-memory

database and to the results file, jobname.rst (or
.rth, .rmg, .rfl).
Input
Data
Database

Solver

Results
Data

Results

Results
File

Stress Analysis - Solution

Stress Analysis - Solution

Solve

Solve

During solution, ANSYS provides a lot of useful information in t he

Output Window, such as:

Demo:
Resume ribmesh.db (2-D plane stress model, thickness = 1/8 in)

Mass properties of the model

The mass calculation is quite accurate; centroid and mass moment
calculations are rough approximations

Fix left line in UX and bottom line in UY

Pressure of 100 psi on top line
List line constraints and pressures

Range of element matrix coefficients

May indicate a problem with material properties or real constants if
maximum/minimum ratio > 1.0E8

Save as ribload.db
Solve. Show output window during solution.

Model size and solver statistics

Summary of files written and their sizes:
jobname.emat - element matrix file
jobname.esav - element saved data file
jobname.tri - triangularized matrix file
jobname.rst -results file

Stress Analysis - Solution

Stress Analysis - Postprocessing

Solve

F. Reviewing Results

Postprocessing is the final step in the finite element analysis

process.

It is imperative that you interpret your results relative to the

assumptions made during model creation and solution.

You may be required to make design decisions based on the

results, so it is a good idea not only to review the results
carefully, but also to check the validity of the solution.

ANSYS has two postprocessors:

Preprocessing
3 Geometry
3 Meshing

Solution
3 Loading
3 Solve

Postprocessing
Review results
Check validity of solution

POST1, the General Postprocessor, to review a single set of

results over the entire model.
POST26, the Time-History Postprocessor, to review results at
selected points in the model over time. Mainly used for transie nt
and nonlinear analyses. (Not discussed in this course.)

Stress Analysis - Postprocessing

Stress Analysis - Postprocessing

...Reviewing Results

...Reviewing Results

Reviewing results of a stress analysis generally involves:

Deformed shape

General Postproc > Plot

Results > Deformed Shape

Stresses
Reaction forces

Deformed Shape

To plot the deformed

shape:

Or use the PLDISP

command.

For animation:

Gives a quick indication of whether the loads were applied in

the correct direction.

Utility Menu > PlotCtrls >

Animate > Deformed Shape

Legend column shows the maximum displacement, DMX.

Or use the ANDISP

command.

You can also animate the deformation.

Stress Analysis - Postprocessing

Stress Analysis - Postprocessing

...Reviewing Results

...Reviewing Results

Stresses

Component stresses SX, SY, SZ, SXY, SYZ, SXZ (global

Cartesian directions by default)
Principal stresses S1, S2, S3, SEQV (von Mises), SINT (stress
intensity)

Best viewed as contour plots, which allow you to quickly

locate hot spots or trouble regions.
Nodal solution: Stresses are averaged at the nodes, showing
smooth, continuous contours.
Element solution: No averaging, resulting in discontinuous
contours.

To plot stress contours:

General Postproc > Plot Results > Nodal Solu or PLNSOL command

The following stresses are typically available for a 3-D solid

model:

General Postproc > Plot Results > Element Solu or PLESOL command

You can also animate stress contours:

Utility Menu > PlotCtrls > Animate > Deformed Results... or ANCNTR
command

Stress Analysis - Postprocessing

Stress Analysis - Postprocessing

...Reviewing Results

...Reviewing Results

A Note on PowerGraphics

Reaction Forces

It is the default graphics setting (/GRAPH,POWER).

Plots only the visible surfaces and ignores

everything underneath.

The sum of the reaction forces in each direction must equal

the sum of applied loads in that direction.

Best viewed as a listing:

Advantages:

General Postprocessor > List Results > Reaction Solution or

PRRSOL command

Faster REPLOT, crisp graphics.

Smooth, almost photo-realistic displays.
Prevents stress averaging across material and
real constant boundaries.

To deactivate PowerGraphics (or activate full

graphics):
Toolbar > POWERGRPH
Or issue /GRAPH,FULL

Stress Analysis - Postprocessing

Stress Analysis - Postprocessing

...Reviewing Results

G. Checking Validity of Solution

It is always a good idea to do a sanity check and make sure

that the solution is acceptable.

What you need to check depends on the type of problem you

are solving, but here are some typical questions to ask:

3 Loading

Do the reaction forces balance the applied loads?

3 Solve

Where is the maximum stress located?

Preprocessing
3 Geometry
3 Meshing

Solution

If it is at a singularity, such as a point load or a re-entrant corner,

the value is generally meaningless. (We will discuss more about
this in Chapter 5.)

Postprocessing
3 Review results
Check validity of solution

Are the stress values beyond the elastic limit?

If so, the load magnitudes may be wrong, or you may need to do
a nonlinear analysis.

Stress Analysis - Postprocessing

Stress Analysis - Postprocessing

...Checking Validity of Solution

Solve

Is the mesh adequate?

This is always debatable, but you can gain confidence in the
mesh by using error estimation data (discussed in Chapter 14).

Demo:
Continue rib problem...
Plot deformed shape and animate it

Other ways to check mesh adequacy:

Plot SX and SEQV contours. Animate one of them.

Plot the element solution (unaveraged stresses) and look for

elements with high stress gradients. These regions are
candidates for mesh refinement.

List reaction forces. Total FY reaction should be 100*2*1/8 = 2 5.

Plot unaveraged SX and compare with averaged SX

If there is a significant difference between the nodal

(averaged) and element ( unaveraged ) stress contours, the
mesh may be too coarse.
Similarly, if there is a significant difference between
PowerGraphics and full graphics stresses, the mesh may be
too coarse.
Re-mesh with twice as many elements, re-solve, and compare
the results. (But this may not always be practical.)

Stress Analysis

Preprocessing
3 Geometry
3 Meshing

Solution
3 Loading
3 Solve

Postprocessing
3 Review results
3 Check validity of solution

Stress Analysis

H. Workshop

This workshop consists of two problems:

2A. Lathe Cutter
2B. 2 -D Corner Bracket Tutorial

Refer to your Workshop Supplement for instructions.

Preliminary Decisions

Overview

Before starting an analysis in ANSYS, you need to make a

few decisions, such as the analysis type needed and the type
of model you want to build.

In this chapter, we will discuss some of the decision making

process. The purpose is to give you an idea of the amount of
planning generally needed before jumping in to do the
analysis.

Topics covered:

Module 5

Preliminary Decisions

A. Which analysis type?

B. What to model?
C. Which element type?

Preliminary Decisions

Preliminary Decisions

A. Which analysis type?

...Which analysis type?

The analysis type usually belongs to one of the following

disciplines:

Once you choose a structural analysis, the next questions

are:

Structural

Motion of solid bodies, pressure on solid bodies,

or contact of solid bodies

Thermal

Applied heat, high temperatures, or changes in

temperature

Electromagnetic

Devices subjected to electric currents (AC or

DC), electromagnetic waves, and voltage or
charge excitation

Fluid

Motion of gases/fluids, or contained gases/fluids

inertia forces (due to mass)

Coupled-Field

Combinations of any of the above

damping forces

We will focus on structural analyses in this discussion.

Static or dynamic analysis?

Linear or nonlinear analysis?

To answer these, remember that whenever a body is

subjected to some excitation (loading), it responds with three
types of forces:
static forces (due to stiffness)

Preliminary Decisions

Preliminary Decisions

...Which analysis type?

...Which analysis type?

Static vs. Dynamic Analysis

Inertia and damping forces are usually significant if the

applied loads vary rapidly with time.

Therefore you can use time-dependency of loads as a way to

choose between static and dynamic analysis.

A static analysis assumes that only the stiffness forces are

significant.

A dynamic analysis takes into account all three types of

forces.

For example, consider the analysis of a diving

board.

If the loading is constant over a relatively long period of time,

choose a static analysis.
Otherwise, choose a dynamic analysis.

If the diver is standing still, it might be sufficient to

do a static analysis.
But if the diver is jumping up and down, you will
need to do a dynamic analysis.

In general, if the excitation frequency is less than 1/3 of the

structures lowest natural frequency, a static analysis may be
acceptable.

Preliminary Decisions

Preliminary Decisions

...Which analysis type?

...Which analysis type?

Linear vs. Nonlinear Analysis

A linear analysis assumes that the loading causes negligible

changes to the stiffness of the structure. Typical
characteristics are:

A nonlinear analysis is needed if the loading causes

significant changes in the structures stiffness. Typical
reasons for stiffness to change significantly are:
Strains beyond the elastic limit (plasticity)

Small deflections

Large deflections, such as with a loaded fishing rod

Strains and stresses within the elastic limit

Contact between two bodies

No abrupt changes in stiffness such as two bodies coming into

and out of contact
Stress
Stress
Elastic modulus
(EX)

Strain
Strain

Preliminary Decisions

Preliminary Decisions

B. What to Model?

...What to Model?

Details

Many modeling decisions must be made before building an

analysis model:

Small details that are unimportant to the analysis should not

be included in the analysis model. You can suppress such
features before sending a model to ANSYS from a CAD
system.

For some structures, however, "small" details such as fillets

or holes can be locations of maximum stress and might be
quite important, depending on your analysis objectives.

How much detail should be included?

Does symmetry apply?
Will the model contain stress singularities?

Preliminary Decisions

Preliminary Decisions

...What to Model?

...What to Model?

Symmetry

Many structures are symmetric in some form and allow only a

representative portion or cross-section to be modeled.

The main advantages of using a symmetric model are:

Geometry
Material properties
Loading conditions

It is generally easier to create the model.

It allows you to make a finer, more detailed model and thereby
obtain better results than would have been possible with the full
model.

To take advantage of symmetry, all of the following must be

symmetric:

There are different types of symmetry:

Axisymmetry
Rotational
Planar or reflective
Repetitive or translational

Preliminary Decisions

Preliminary Decisions

...What to Model?

...What to Model?

Axisymmetry

Rotational symmetry

Symmetry about a central axis, such as in light bulbs, straight

pipes, cones, circular plates, and domes.

Repeated segments arranged about a central axis, such as in

turbine rotors.

Plane of symmetry is the cross-section anywhere around the

structure. Thus you are using a single 2-D slice to
represent 360 a real savings in model size!

Only one segment of the structure needs to be modeled.

Loading is also assumed to be symmetric about the axis.

Loading is also assumed to be

axisymmetric in most cases.
However, if it is not, and if the
analysis is linear, the loads can be
separated into harmonic
components for independent
solutions that can be superimposed.

Preliminary Decisions

Preliminary Decisions

...What to Model?

...What to Model?

Planar or reflective symmetry

Repetitive or translational symmetry

One half of the structure is a mirror image of the other half.

The mirror is the plane of symmetry.

Repeated segments arranged along a straight line, such as a

long pipe with evenly spaced cooling fins.

Loading may be symmetric or anti-symmetric about the plane

of symmetry.

Loading is also assumed to be repeated along the length of

the model.

This model illustrates

both reflective and
rotational symmetry

This model illustrates both repetitive and reflective symmetry.

Preliminary Decisions

Preliminary Decisions

...What to Model?

...What to Model?

Stress singularities

In some cases, only a few minor details will disrupt a

structure's symmetry. You may be able to ignore such
details (or treat them as being symmetric) in order to gain the
benefits of using a smaller model. How much accuracy is
lost as the result of such a compromise might be difficult to
estimate.

A stress singularity is a location in a finite element model

where the stress value is unbounded (infinite). Examples:
A point load, such as an applied force or moment
An isolated constraint point, where the reaction force behaves
like a point load
A sharp re -entrant corner (with zero fillet radius)

As the mesh density is refined at

a stress singularity, the stress value
increases and never converges.

= P/A
As A 0,

Preliminary Decisions

Preliminary Decisions

...What to Model?

C. Which Element Type?

Real structures do not contain stress singularities. They are

a fiction created by the simplifying assumptions of the model.

This is an important decision you usually need to make

before beginning the analysis.

So how do you deal with stress singularities?

Typical issues are:

If they are located far away from the region of interest, you ca n
simply ignore them by deactivating the affected zone while
reviewing results.
If they are located in the region of interest, you will need to take
corrective action, such as:
adding a fillet at re -entrant corners and reruning the analysis.
replacing a point force with an equivalent pressure load.
spreading out displacement constraints over a set of
nodes.

Which element category? Solid, shell, beam, etc.

Element order. Linear or quadratic.
Mesh density. Usually determined by the objectives of the
analysis.

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Element category

Line elements:
Beam elements are used to model bolts, tubular members, Csections, angle irons, or any long, slender members where only
membrane and bending stresses are needed.

ANSYS offers many different categories of elements. Some

of the commonly used ones are:
Line elements

Spar elements are used to model springs, bolts, preloaded bolts,

and truss members.

Shells
2-D solids

Spring elements are used to model springs, bolts, or long

slender parts, or to replace complex parts by an equivalent
stiffness.

3-D solids

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Shell elements:

2-D Solid elements:

Used to model thin panels or curved surfaces.

Used to model a cross -section of solid objects.

The definition of thin depends on the application, but as a

general guideline, the major dimensions of the shell structure
(panel) should be at least 10 times its thickness.

Must be modeled in the global Cartesian X-Y plane.

All loads are in the X-Y plane, and the response (displacements)
are also in the X-Y plane.
Element behavior may be one of the following:
plane stress
plane strain
axisymmetric
axisymmetric harmonic

Y
Z

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Plane stress assumes zero stress

in the Z direction.
Valid for components in which the
Z dimension is smaller than the X
and Y dimensions.
Z-strain is non-zero.

Valid for components in which the Z

dimension is much larger than the X and Y
dimensions.

Y
Z

Plane strain assumes zero strain in the Z

direction.

Z-stress is non-zero.

Used for long, constant cross-section

structures such as structural beams.

Optional thickness (Z direction)

allowed.

Z
Y

Used for structures such as flat

plates subjected to in-plane
loading, or thin disks under
pressure or centrifugal loading.

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Axisymmetry assumes that the 3-D model

and its loading can be generated by revolving
a 2-D section 360 about the Y axis.
Axis of symmetry must coincide with the
global Y axis.
Negative X coordinates are not permitted.
Y direction is axial, X direction is radial, and Z
direction is circumferential (hoop) direction.
Hoop displacement is zero; hoop strains and
stresses are usually very significant.
Used for pressure vessels, straight pipes,
shafts, etc.

Axisymmetric harmonic is a special case of axisymmetry

where the loads can be non- axisymmetric.
The non -axisymmetric loading is decomposed into Fourier
series components, applied and solved separately, and then
combined later. No approximation is introduced by this
simplification!
Used for non -axisymmetric loads such as torque on a shaft.

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Element Order

3-D Solid elements:

Used for structures which, because of geometry, materials,
loading, or detail of required results, cannot be modeled with
simpler elements.

Element order refers to the polynomial order of the elements

shape functions.

Also used when the model geometry is transferred from a 3-D

CAD system, and a large amount of time and effort is required to
convert it to a 2 -D or shell form.

What is a shape function?

It is a mathematical function that gives the shape of the results
within the element. Since FEA solves for DOF values only at
nodes, we need the shape function to map the nodal DOF values
to points within the element.
The shape function represents assumed behavior for a given
element.
How well each assumed element shape function matches the
true behavior directly affects the accuracy of the solution, as
shown on the next slide.

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Quadratic distribution of
DOF values

Linear approximation
(Poor Results )

When you choose an element type, you are implicitly

choosing and accepting the element shape function assumed
for that element type. Therefore, check the shape function
information before you choose an element type.

Typically, a linear element has only corner nodes, whereas a

quadratic element also has midside nodes.

Actual quadratic
curve

Linear approximation
with multiple elements
(Better Results )

Quadratic approximation
(Best Results)

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Linear elements

Quadratic elements

Can support only a linear variation

of displacement and therefore
(mostly) only a constant state of
stress within a single element.

Can support a quadratic variation

of displacement and therefore a
linear variation of stress within a
single element.

Highly sensitive to element

distortion.

Acceptable if you are only

interested in nominal stress
results.

Can represent curved edges and

surfaces more accurately than
linear elements. Not as sensitive
to element distortion.

Need to use a large number of

elements to resolve high stress
gradients.

Recommended if you are

interested in highly accurate
stresses.

Give better results than linear

elements, in many cases with
fewer number of elements and
total DOF.

Notes:
For shell models, the difference between linear and quadratic
elements is not as dramatic as for solid models. Linear shells
are therefore usually preferred.
Besides linear and quadratic elements, a third kind is available,
known as p-elements. P -elements can support anywhere from a
quadratic to an 8th -order variation of displacement within a
single element and include automatic solution convergence
controls.

Preliminary Decisions

Preliminary Decisions

...Which Element Type?

...Which Element Type?

Mesh Density

The fundamental premise of FEA is that as the number of

elements (mesh density) is increased, the solution gets
closer and closer to the true solution.

However, solution time and computer resources required

also increase dramatically as you increase the number of
elements.

The objectives of the analysis usually decide which way the

slider bar below should be moved.

If you are interested in highly accurate stresses:

A fine mesh will be needed, omitting no geometric details at any
location in the structure where such accuracy is needed.
Stress convergence should be demonstrated.
Any simplification anywhere in the model might introduce
significant error.

If you are interested in deflections or nominal stresses:

A relatively coarse mesh is sufficient.
Small geometry details may be omitted.

Preliminary Decisions

...Which Element Type?

If you are interested in mode shapes (modal analysis):

Small details can usually be omitted.
Simple mode shapes can be captured using a relatively coarse
mesh.
Complex mode shapes may require a uniform, moderately fine
mesh.

Thermal Analyses:
Small details can usually be omitted, but since many thermal
analyses are followed by a stress analysis, stress
considerations generally dictate the detail of the model.
Mesh density is usually determined by expected thermal
gradients. A fine mesh is required for high thermal gradients,
whereas a coarse mesh may be sufficient for low gradients.

Thermal Analysis

In this chapter, we will briefly describe the procedure to do a

steady- state thermal analysis.

The purpose is two -fold:

To reiterate the typical analysis steps that were introduced in
Chapter 4.

Module 6

To introduce you to thermal loads and boundary conditions.

Thermal Analysis

Topics covered:
A. Overview
B. Procedure
C. Workshop

Thermal Analysis

Thermal Analysis

A. Overview

...Overview

Thermal analyses are used to determine the temperature

distribution, thermal gradient, heat flow, and other such
thermal quantities in a structure.

Thermal loading conditions can be:

Temperatures
Convections

A thermal analysis can be steady-state or transient.

Steady-state implies that the loading conditions have settled
down to a steady level, with little or no time dependency.
Example: An iron that has already reached the desired
temperature setting.
Transient* implies conditions that are changing with time.
Example: A casting in the process of cooling down from molten
metal to solid.

Heat flux*
Heat flow*
Heat generation*
Radiation*

Adiabatic surfaces
* Not covered in this course

Regions of the model where temperatures are known.

Surfaces where heat is transferred to (or from)
surroundings by means of convection. Input consists
of film coefficient h and bulk temperature of the
surrounding fluid Tb.
Surfaces where the heat flow rate per unit area is
known.
Points where the heat flow rate is known.
Regions where the volumetric heat generation rate is
known.
Surfaces where heat transfer occurs by means of
radiation. Input consists of emissivity, StefanBoltzmann constant, and optionally, temperature at a
space node.
Perfectly insulated surfaces where no heat transfer
takes place.
* Not covered in this course

Thermal Analysis

Thermal Analysis - Procedure

B. Procedure

Preprocessing

Geometry

The procedure to do a steady- state thermal analysis is similar

to that for a static stress analysis:

Can either be created within ANSYS or imported .

Details of both methods will be covered later.

Preprocessing
Geometry
Meshing
Solution
Loading
Solve
Postprocessing
Review results
Validate the solution

Setting GUI preferences ( Main Menu > Preferences) to Thermal

may be helpful.

Thermal Analysis - Procedure

Thermal Analysis - Procedure

...Preprocessing

...Preprocessing

Meshing

Material properties

First define element attributes: element type, real constants,

and material properties.
Element type
The table below shows commonly used thermal element
types.
There is only one DOF per node: TEMP

Commonly used thermal element types

Linear
Quadratic

2-D Solid

3-D Solid

3-D Shell

Line Elements

PLANE55 n
PLANE77 n

SOLID70 n
SOLID90 n

SHELL57 n

LINK31,32,33,34

PLANE35 s

SOLID87 s

Minimum requirement is thermal conductivity, KXX.

Specific heat (C) will be needed if internal heat generation is to
be applied.
ANSYS-supplied material library (/ansys57/matlib) contains both
structural and thermal properties for a few common materials,
but we recommend that you create and use your own material
library.
Setting preferences to Thermal limits the Material Model GUI t o
display only thermal properties.

Real constants
Primarily needed for shell and line elements.

Thermal Analysis - Procedure

Thermal Analysis - Procedure

...Preprocessing

Solution

Loading

Then mesh the geometry.

Save the database.

Use the MeshTool to create the mesh. The default smart-size

level of 6 produces a good initial mesh.

Prescribed Temperatures
DOF constraints for a thermal
analysis
Solution > -Loads-Apply >
Temperature

This completes the preprocessing step. Solution is next.

Or the D family of commands

(DA, DL, D )

Convections
These are surface loads
Solution > -Loads-Apply >
Convection
Or the S F family of commands
(SFA, SFL, SF, SFE )

Thermal Analysis - Procedure

Thermal Analysis - Procedure

...Solution

...Solution

Solve

Adiabatic Surfaces
Perfectly insulated surfaces where no heat transfer takes
place.

First save the database.

This is the default condition, i.e, any surface with no boundary

conditions specified is automatically treated as an adiabatic
surface.

Then issue SOLVE or click on Solution > - Solve- Current LS .

Other possible thermal loads:

heat flux
heat flow

(BTU / (hr-in2)
(BTU / hr)

heat generation
radiation

(BTU / hr)

(BTU / (hr-in3)

Results are written to the results file, jobname.rth, as well as to

the in-memory database.

This completes the solution step. Postprocessing is next.

Thermal Analysis - Procedure

Thermal Analysis - Procedure

Postprocessing

...Postprocessing

Review Results

Typically consists of contour plots of temperature, thermal

gradient, and thermal flux.

A useful option for contour plots in 3-D solid models is

isosurfaces surfaces of constant value. Use the /CTYPE
command or Utility Menu > PlotCtrls > Style > Contours >
Contour Style.

General Postproc > Plot Results > Nodal Solu (or Element Solu)
Or use PLNSOL (or PLESOL )

Thermal Analysis - Procedure

Thermal Analysis - Procedure

...Postprocessing

C. Workshop

Validate the Solution

Are temperatures within the expected range?

You can generally guess the expected range based on
prescribed temperatures and convection boundaries.

Is the mesh adequate?

Just as in the case of stresses, you can plot the unaveraged
thermal gradients (element solution) and look for elements with
high gradients. These regions are candidates for mesh
refinement.
If there is a significant difference between the nodal (averaged )
and element ( unaveraged ) thermal gradients, the mesh may be
too coarse.

Refer to your Workshop Supplement for instructions on:

W3. Axisymmetric Pipe with Fins

Thermal-Stress Analysis

In this chapter, we will briefly describe how to do a thermalstress analysis.

The purpose is two -fold:

Module 7

To show you how to apply thermal loads in a stress analysis.

To introduce you to a coupled -field analysis.

Topics covered:
A. Overview

Thermal-Stress Analysis

B. Sequential
C. Direct
D. Workshop

Thermal -Stress Analysis

Thermal -Stress Analysis

A. Overview

Overview

Thermally Induced Stress

When a structure is heated or cooled, it

deforms by expanding or contracting.

If the deformation is somehow restricted

by displacement constraints or an
opposing pressure, for example
thermal stresses are induced in the
structure.

Another cause of thermal stresses is

non-uniform deformation, due to different
materials (i.e, different coefficients of
thermal expansion).

Thermal stresses
due to constraints

Thermal stresses
due to different
materials

There are two methods of solving thermal-stress

problems using ANSYS. Both methods have their
advantages.
Sequential coupled field
- Older method, uses two element types mapping
thermal results as structural temperature loads
+ Efficient when running many thermal transient time
points but few structural time points
+ Can easily be automated with input files
Direct coupled field
+ Newer method uses one element type to solve both
physics problems
+ Allows true coupling between thermal and structural
phenomena
- May carry unnecessary overhead for some analyses

Thermal -Stress Analysis

Thermal -Stress Analysis

B. Sequential Method

Sequential Method

1. Thermal Analysis

The Sequential method involves two analyses:

1. First do a steady-state (or transient) thermal
analysis.
Model with thermal elements.
Apply thermal loading.

The procedure for this is described in Chapter 6.

Thermal
Analysis
jobname.rth

Solve and review results.

2. Then do a static structural analysis.
Switch element types to structural.
Define structural material properties,
including thermal expansion coefficient.
Apply structural loading, including
temperatures from thermal analysis.
Solve and review results.

2. Structural Analysis
a) Move to PREP7 and switch element types from thermal to
structural.
Preprocessor > Element Type > Switch Elem Type

Temperatures
Structural
Analysis
jobname.rst

Or ETCHG command
Caution: Switching element types will reset all element options
back to their default settings. For example, if you used 2-D
axisymmetric elements in the thermal analysis, you may need to
respecify the axisymmetric option after the switch. Therefore,
be sure to verify and set the proper element options:
Preprocessor > Element Type > Add/Edit/Delete > [Options]
Or use ETLIST and KEYOPT commands

Thermal -Stress Analysis

Thermal -Stress Analysis

Sequential Method

Sequential Method

b) Define structural material properties (EX, etc.), including the

coefficient of thermal expansion (ALPX). (If you use the ANSYS supplied material library, both thermal and structural properties
will be defined, so this step may not be needed.)
Note: If ALPX is not defined or set to zero, no thermal strains
will be calculated. You can use this technique to turn off
temperature effects!
c) Specify static analysis type. This step is needed only if the
thermal analysis was a transient.
Solution > -Analysis Type- New Analysis
Or ANTYPE command

d) Apply structural loads and include temperatures as part of the

loading.
Solution > -Loads- Apply > -Structural - Temperature > From
Therm Analy
Or use the LDREAD command.
e) Solve.
f) Review stress results.

Thermal -Stress Analysis

Thermal -Stress Analysis

C. Direct Method

Sequential vs. Direct

The Direct Method usually involves just one analysis that uses a coupledfield element type containing all necessary degrees of freedom.
1. First prepare the model and mesh using one
of the following coupled field element types.
PLANE13 (plane solid).
SOLID5 (hexahedron).
SOLID98 (tetrahedron).
2. Apply both the structural and thermal loads
and constraints to the model.
3. Solve and review both thermal and
structural results.

Thermal
Analysis
Combined

Structural
Analysis

jobname .rst

Thermal -Stress Analysis

D. Workshop

Refer to your Workshop Supplement for instructions on:

W4a. Axisymmetric Pipe with Fins (Sequential Coupled Fileld)
W4b. Axisymmetric Pipe with Fins (Direct Coupled Field)

Sequential
For coupling situations which
do not exhibit a high degree of
nonlinear interaction, the
sequential method is more
efficient and flexible because
you can perform the two
analyses independently of
each other.
In a sequential thermal-stress
analysis, for example, you can
perform a nonlinear transient
thermal analysis followed by a
linear static stress analysis.
You can then use nodal
temperatures from ANY load
step or time-point in the
thermal analysis as loads for
the stress analysis.

Direct
Direct coupling is
advantageous when the
coupled-field interaction is
highly nonlinear and is best
solved in a single solution
using a coupled formulation.
Examples of direct coupling
include piezoelectric analysis,
conjugate heat transfer with
fluid flow, and circuitelectromagnetic analysis.

Importing Geometry

Overview

If the geometry of the part you want to analyze has already

been created in a CAD package, it is generally more efficient
to import it into ANSYS than to re- create it.

In this chapter, we will discuss the various import options

available in ANSYS:

Module 8

A. IGES Imports expands on IGES importing, which was covered

briefly in Chapter 4.
B. Connection Products shows how to import parts directly from
certain CAD packages.

Importing Geometry

C. F.E. Model Imports briefly explains how to import nodes and

elements.
D. Workshop a hands -on exercise on importing.

Importing Geometry

Importing Geometry

A. IGES Imports

...IGES Imports

The general procedure to import an IGES file has already

been discussed in Chapter 4. In this section, we will explore
some of the options available:

No Defeaturing Method Imports and stores geometry in the

standard ANSYS database. [ ioptn,iges,nodefeat]
+ Faster and more reliable than the Defeaturing method.

the two methods, No Defeaturing and Defeaturing

+ Allows the full set of solid model operations.

the Merge , Solid, and Small options

No defeaturing tools are available.

+ This is the DEFAULT and recommended method.

Importing Geometry

Importing Geometry

...IGES Imports

...IGES Imports

Defeaturing Method Imports and stores geometry

in a special database that allows you to repair and
defeature the model. [ ioptn,iges,defeat]

Merge Option
YES by default, to merge coincident entities so that adjacent
areas meet at a common line, and adjacent lines meet at a
common keypoint.

+ Ability to defeature, i.e, to remove minor details such

as protrusions, cavities, and small holes.

Switch it to NO only if you are using the Defeaturing method and

your initial attempt runs out of memory.

Because of the special database used to store

geometry, only a limited number of solid model
operations are available.

ioptn,merge,yes/no

Generally requires more memory and is somewhat

slower than the No defeaturing method.
+ This method is efficient for single solid models that
will be imported, loaded, meshed and solved.

merge

In general, it is NOT recommended when advanced

geometry capabilities are required.

Importing Geometry

Importing Geometry

...IGES Imports

...IGES Imports

Solid Option

Small Option

YES default, to automatically create a volume (solid) after

importing and merging.

YES by default, to automatically delete small, sliver-like areas

that might be troublesome for meshing.

Switch it to NO if you want to import surfaces only and create a

shell or 2-D plane model.

Available only for the Defeature method.

ioptn,solid,yes/no

ioptn,small,yes/no

Switch it to NO if you find gaps or holes in the model.

Importing Geometry

Importing Geometry

B. Connection Products

...Connection Products

IGES importing works quite well, but because of the dual

translation process CAD IGES ANSYS there are
many cases when a 100% translation is not achieved.

Connection for Pro/E

Reads .prt file produced by Pro/ENGINEER (from Parametric Technology
Corp.).

ANSYS Connection products help overcome this problem by

directly reading the native part files produced by the CAD
package:

Can also read a Pro/Engineer assembly file (.asm)

Requires Pro/ENGINEER software.
Utility Menu > File > Import > Pro/E...
Or ~proein

Connection for Pro/ENGINEER (Pro/E for short)

Connection for Unigraphics (UG for short)
Connection for SAT
Defeaturing option available

Connection for Parasolid

No Defeaturing is default

To use a connection product, you need to purchase the

appropriate license.

Command that launches your Pro/E

Importing Geometry

Importing Geometry

...Connection Products

...Connection Products

Connection for UG

Connection for SAT

Reads .p r t file produced by Unigraphics (from Electronic Data

Systems Corp.).

Reads .sat file produced by CAD packages that use the ACIS
modeler.

Requires Unigraphics software.

Does not require ACIS software.

Utility Menu > File > Import > UG...

Utility Menu > File > Import > SAT...

Or ~ugin

Or ~satin

Option to read only

selected layers and
geometry types

Option to read only

selected geometry types

Defeaturing option available

Defeaturing option available

No Defeaturing is default

No Defeaturing is default

Importing Geometry

Importing Geometry

...Connection Products

C. F.E. Model Imports

In addition to solid model geometry, ANSYS can also import

finite element model data (nodes and elements) from certain
packages.

The most common approach is for the software vendor to

write out the nodes and elements in a format that ANSYS
can read (using NREAD and EREAD ). This format is
published in the ANSYS Programmers Manual.

Some software packages provide an interface that allows you

to transfer more than just nodes and elements from another
finite element package into ANSYS.

Connection for Parasolid

Reads .x_t or .xmt_txt file produced by CAD packages that use
the Parasolid modeler.
Does not require Parasolid software.
Utility Menu > File > Import > PARA...
Or ~parain
Option to read only
selected geometry types
Defeaturing option available
No Defeaturing is default
Option to scale geometry

Importing Geometry

D. Workshop

Refer to your Workshop Supplement for instructions on:

W5. Importing Geometry

Meshing

Overview

Recall that meshing is a three- step procedure:

Define element attributes
Specify mesh controls
Generate the mesh

Module 10

In this chapter, we will expand on each of these steps and

also discuss additional meshing options.

Meshing

Topics covered:
A. Multiple Element Attributes

E. Hex -to-Tet Meshing

B. Controlling Mesh Density

F. Mesh Extrusion

C. Changing a Mesh

G. Sweep Meshing

D. Mapped Meshing

H. Workshop

Meshing

Meshing

A. Multiple Element Attributes

...Multiple Element Attributes

As we discussed earlier, every element has the following attributes

associated with it:
Element type (TYPE)

Whenever you have multiple TYPEs, REALs and MATs, you

need to make sure that each element is assigned the proper
attributes. There are three ways to do this:

Real constants (REAL)

Assign attributes to the solid model entities before meshing

Material properties (MAT)

Activate a global setting of MAT, TYPE, and REAL before

meshing

Most FEA models have multiple attributes. For example, the silo
shown here has two element types, three real constant sets, and two
materials.

Modify element attributes after meshing

TYPE 1 = shell
TYPE 2 = beam

MAT 1 = concrete
MAT 2 = steel

REAL 1 = 3/8 thickness

REAL 2 = beam properties
REAL 3 = 1/8 thickness

If no assignments are made, ANSYS uses default settings of

MAT=1, TYPE=1, and REAL=1 for all elements in the model.
Note, the current activeTYPE, REAL, and MAT dictates mesh
operation.

Meshing

Meshing

...Multiple Element Attributes

...Multiple Element Attributes

Assigning Attributes to the Solid Model

Using Global Attribute Settings

1. Define all necessary element types, materials,

and real constant sets.

1. Define all necessary element types,

materials, and real constant sets.

2. Then use the Element Attributes section of

the MeshTool (Preprocessor > MeshTool):

2. Then use the Element Attributes

section of the MeshTool (Preprocessor >
MeshTool):

Choose entity type and press the SET button.

Choose Global and press the SET button.

Pick the entities to which you want to assign

attributes.

Activate the desired combination of

attributes in the Meshing Attributes
dialog box. We refer to these as the
active TYPE, REAL, and MAT settings.

Set the appropriate attributes in the subsequent

dialog box.
Or select the desired entities and use the
VATT, AATT, LATT, or KATT command.
3. When you mesh an entity, its attributes are
automatically transferred to the elements.

Or use the TYPE, REAL, and MAT

commands.
3. Mesh only those entities to which the
above settings apply.

Meshing

Meshing

...Multiple Element Attributes

...Multiple Element Attributes

Modifying Element Attributes

Some points to keep in mind:

1. Define all necessary element types, materials, and real constant

sets.

You can verify element attributes by

activating attribute numbering:
Utility Menu > PlotCtrls > Numbering

2. Activate the desired combination of TYPE, REAL, and MAT settings:

Or /PNUM,attr,ON, where attr may be TYPE,

MAT, or REAL

Preprocessor > -Attributes- Define > Default Attribs...

Or use the TYPE, REAL, and MAT commands
3. Modify the attributes of only those elements to which the above
settings apply:
Issue EMODIF,PICK or choose Preprocessor > Move/Modify > -ElementsModify Attrib

Element attributes assigned directly to solid model entities will

override the default attribute pointers.

By assigning attributes to solid model entities, you can avoid having

to reset attributes in the middle of meshing operations. This is
advantageous because ANSYS meshing algorithms are most
efficient when meshing all entities at once.

Clearing a solid model entity of its mesh will not delete attrib ute
assignments.

Then pick the desired elements

4. In the subsequent dialog box,
set attributes to All to current.

Meshing

Meshing

...Multiple Element Attributes

B. Controlling Mesh Density

Demo:
Resume ribgeom.db

ANSYS provides many tools to control mesh density, both on

a global and local level:
Global controls

List element types, real constants, and materials. One of each

has been defined.

SmartSizing
Global element sizing

Bring up MeshTool, choose area attributes, and press Set

Default sizing

Pick the single area, show the Area Attributes dialog box, and
press OK. (There is only one set of attributes, but this illustrates
the general procedure.)

Local controls
Keypoint sizing
Line sizing
Area sizing

Meshing

Meshing

...Controlling Mesh Density

...Controlling Mesh Density

SmartSizing

Determines element sizes by assigning divisions on all lines,

taking into account curvature of the line, its proximity to
holes and other features, and element order.
SmartSizing is off by default, but is recommended for free
meshing. It does not affect mapped meshing. (Free meshing
vs. mapped meshing will be discussed later.)

To use SmartSizing:
Bring up the MeshTool (Preprocessor > MeshTool),
turn on SmartSizing, and set the desired size level.
Or use SMRT,level
Size level ranges from 1 (very fine) to 10 (very
coarse). Defaults to 6.
Then mesh all volumes (or all areas) at once, rather
than one -b y-one.

Meshing

Meshing

...Controlling Mesh Density

...Controlling Mesh Density

Examples of different SmartSize

levels are shown here for a
tetrahedron mesh.

Global Element Sizing

Advanced SmartSize controls,

such as mesh expansion and
transition factors, are available
on the SMRT command (or
Preprocessor > -Meshing- Size
Cntrls > -SmartSize - Adv Opts...)

ESIZE,SIZE

Allows you to specify a maximum element edge length

for the entire model (or number of divisions per line):
or Preprocessor > MeshTool > Size Controls - Global [Set]
or Preprocessor > -Meshing- Size Cntrls > -Global-Size

You can turn off SmartSizing

using the MeshTool or by
issuing smrt,off.

Can be used by itself or in conjunction

with SmartSizing.
Using ESIZE by itself (SmartSizing off) will
result in a uniform element size throughout
the volume (or area) being meshed.
With SmartSizing on, ESIZE acts as a
guide, but the specified size may be
overridden to accommodate line curvature
or proximity to features.

Meshing

Meshing

...Controlling Mesh Density

...Controlling Mesh Density

Default Sizing

Keypoint Sizing

If you dont specify any controls, ANSYS uses default sizing,

which assigns minimum and maximum line divisions, aspect
ratio, etc. based on element order.

Controls element size at keypoints:

Preprocessor > MeshTool > Size Controls: Keypt [Set]
or KESIZE command

Meant for mapped meshing, but is also used for free meshing
if SmartSizing is off.

or Preprocessor > -Meshing- Size Cntrls > -Keypoints-

Different keypoints can have different KESIZEs,

giving you more control over the mesh.

You can adjust default size specifications using DESIZE or

Preprocessor > -Meshing - Size Cntrls > -Global - Other .

Useful for stress concentration regions.

Specified sizes may be overridden by SmartSizing

to accommodate line curvature or proximity to
features.

Meshing

Meshing

...Controlling Mesh Density

...Controlling Mesh Density

Line Sizing

Area Sizing

Controls element size at lines:

Preprocessor > MeshTool > Size Controls: Lines
[Set]
or LESIZE command
or Preprocessor > -Meshing- Size Cntrls > -Lines-

Controls element size in the interior of areas:

Preprocessor > MeshTool > Size Controls: Areas [Set]
or AESIZE command

Yes for soft

No for hard

or Preprocessor > -Meshing- Size Cntrls > -Areas -

Different lines can have different LESIZEs.

Size specifications may be hard or soft.

Hard sizes are always honored by the mesher,
even if SmartSizing is on. They take
precedence over all other size controls.
Soft sizes may be overridden by SmartSizing.

Different areas can have different AESIZEs.

You can also specify a spacing ratio ratio

of last division to first. Used to bias the
divisions towards one end or towards the
middle.

Bounding lines will use the specified size only if they

have no LESIZE or KESIZE specified and if no
adjacent area has a smaller size.

Specified sizes may be overridden by SmartSizing to

accommodate line curvature or proximity to features.

Meshing

Meshing

...Controlling Mesh Density

C. Changing a Mesh

Demo:
Resume ribgeom.db
Mesh with SMRT,6. (Not a very good mesh)
Re-mesh with SMRT,3 (good mesh)
Set ESIZE to 0.2 and re-mesh. The mesh becomes coarse even
though SMRT is set to 3, because the smart-mesher takes ESIZE
into account. Also note that the element sizes are not uniform
(because SMRT is on).
Turn off SMRT and re -mesh. Element sizes are now uniform.

If a mesh is not acceptable, you can always

re-mesh the model by following these steps:
1. Clear the mesh.
The clear operation is the opposite of mesh:
it removes nodes and elements.
Use the [Clear] button on the MeshTool, or
use VCLEAR, ACLEAR, etc.
(If you are using the MeshTool, you may skip
this step since the program will prompt you
whether to clear or not when you execute
step 3.)
2. Specify new or different mesh controls.
3. Mesh again.

Meshing

Meshing

...Changing a Mesh

...Changing a Mesh

Another meshing option is to refine

the mesh in specific regions.

Demo:
Continuing the last demo (ribgeom has been meshed with
ESIZE = 0.2)

Available for all area elements and

only tetrahedral volume elements.

Choose refinement at Lines and press Refine

Easiest way is to use the MeshTool:

First save the database.
Then choose how you want to
specify the region of refinement
at nodes, elements, keypoints,
lines, or areas and press the
Refine button.
Pick the entities at which you
want the mesh to be refined. (Not
required if you choose All
Elems .)
Finally, choose the level of
refinement. Level 1 (minimal
refinement) is a good starting
point.

Pick the top line, then choose the default minimal refinement

Meshing

Meshing

D. Mapped Meshing

...Mapped Meshing

There are two main meshing methods: free and

mapped .
Free Mesh

Free Mesh
+ Easy to create; no need to
divide complex shapes into
regular shapes.

Has no element shape restrictions.

The mesh does not follow any pattern.

Volume meshes can contain

only tetrahedra, resulting in a
large number of elements.

Only higher-order (10 -node)

tetrahedral elements are
acceptable, so the number of
DOF can be very high.

Suitable for complex shaped areas and volumes.

Mapped Mesh
Restricts element shapes to quadrilaterals for
areas and hexahedra (bricks) for volumes.
Typically has a regular pattern with obvious rows
of elements.
Suitable only for regular areas and volumes
such as rectangles and bricks.

Mapped Mesh
+ Generally contains a lower
number of elements.
+ Lower -order elements may be
acceptable, so the number of
DOF is lower.

Areas and volumes must be

regular in shape, and mesh
divisions must meet certain
criteria.

Very difficult to achieve,

especially for complex shaped
volumes.

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

Creating a Free Mesh

Creating a Mapped Mesh

Free meshing is the default setting for both

area and volume meshes.

Create a free mesh is easy:

Bring up the MeshTool and verify that free
meshing is set.
SmartSizing is generally recommended for free
meshing, so activate it and specify a size level.
Save the database.
Then initiate the mesh by pressing the Mesh
button.
Press [Pick All] in the picker to choose all
entities (recommended).

This is not as easy as free meshing because the areas and

volumes have to meet certain requirements:
Area must contain either 3 or 4 lines (triangle or quadrilateral).
Volume must contain either 4, 5, or 6 areas (tetrahedron,
triangular prism, or hexahedron).
Element divisions on opposite sides must match.
For triangular areas or tetrahedral volumes, the number of
element divisions must be even.

Or use the commands VMESH,ALL or

AMESH,ALL .

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

For quadrilateral areas or hexahedral volumes, unequal

divisions are allowed, as shown in these examples, but the
number of divisions must satisfy a formula (shown on the
next page).

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

Ensure regular shapes

Thus mapped meshing involves a three-step procedure:

Ensure regular shapes, i.e, areas with 3 or 4 sides, or volumes
with 4, 5, or 6 sides.

Specify size and shape controls

Generate the mesh

In most cases, the model geometry is such that the areas

have more than 4 sides, and volumes have more that 6 sides.
To convert these to regular shapes, you may need to do one
or both of these operations:
Slice the areas (or volumes) into smaller, simpler shapes.
Concatenate two or more lines (or areas) to reduce the total
number of sides.

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

Slicing can be accomplished with the Boolean divide

operation.
Remember that you can use the working plane, an area, or a line
as the slicing tool.
Sometimes, it may be easier to create a new line or a new area
than to move and orient the working plane in the correct
direction.

Concatenation creates a new line (for meshing purposes) that

is a combination of two or more lines, thereby reducing the
number of lines making up the area.
Use the LCCAT command or Preprocessor > -MeshingConcatenate > Lines, then pick the lines to be concatenated.
For area concatenation, use ACCAT command or Preprocessor >
-Meshing- Concatenate > Areas

Concatenating
these two lines
makes this a
4-sided area

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

You can also i m p l y a concatenation by simply

identifying the three or four corners of the area. In
this case, ANSYS internally generates the
concatenation.

Notes on concatenation:
It is purely a meshing operation and therefore should be the las t step
before meshing, after all solid modeling operations. This is because the
output entity obtained from a concatenation cannot be used in any
subsequent solid modeling operation.

To do this, choose Quad shape and Map mesh in the

MeshTool.

You can "undo" a concatenation by deleting the line or area it produced.

Then change 3/4 sided to Pick corners .

Concatenating areas (for mapped volume meshing) is generally much

more complicated because you may also need to concatenate some
lines. Lines are automatically concatenated only when two adjac ent, 4sided areas are concatenated.

Press the Mesh button, pick the area, and then pick
the 3 or 4 corners that form the regular shape.

Consider the add (Boolean) operation if the lines or areas meet at a

tangent.

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

Specify size and shape controls

This is the second step of the three-step mapped

meshing procedure.

Choosing the shape is simple. In the MeshTool,

choose Quad for area meshing, and H e x for volume
meshing, then click on Map.

Commonly used size controls and the order in which

they are applied:
Line sizing [LESIZE ] is always honored.
Global element size , if specified, will be applied to
unsized lines.
Default element sizing [DESIZE ] will be applied to
unsized lines only if ESIZE is not specified.
(SmartSizing is not valid.)

If you specify line divisions, remember that:

divisions on opposite sides must match, but you only need to
specify one side. The map mesher automatically transfers
divisions to the opposite side.
if you have concatenated lines, divisions can only be applied to
the original (input) lines, not the composite line.
6 divisions specified on
each original line.
12 divisions will be
automatically applied to
this line (opposite to
composite line).
How many divisions are
used for the other two
lines? (Upcoming demo
will answer it.)

Meshing

Meshing

...Mapped Meshing

...Mapped Meshing

Generate the mapped mesh

Question: How would

you slice this model for
mapped meshing?

Answer: It may not be worth

the effort!

Once you have ensured regular shapes and assigned the

appropriate divisions, generating the mesh is easy. Just
press the Mesh button in the MeshTool, then press [ Pick All]
in the picker or choose the desired entities.

Meshing

Meshing

...Mapped Meshing

E. Hex-to-Tet Meshing

Demo:
Resume ribfull.db

For volume meshing, we have only seen two

options so far:
Free meshing, which creates an all-tet mesh.
This is easy to achieve but may not be
desirable in some cases because of the large
number of elements and total DOF created.

Bring up MeshTool and apply 6 divisions to top and right lines

Map -mesh the area using Pick corners. Notice that the left and
bottom lines get only two divisions each (from DESIZE).
Now specify ESIZE,,4 (4 divisions per line) and re -mesh

Mapped meshing, which creates an all -hex

mesh. This is desirable but usually very
difficult to achieve.

Finally, clear line divisions, specify ESIZE,0.1 (size), and re -mesh

Hex-to-tet meshing provides a third option

that is the best of both worlds. It allows
you to have a combination of hex and tet
meshes without compromising the integrity
of the mesh.

Meshing

Meshing

...Hex-to-Tet Meshing

...Hex-to-Tet Meshing

This option works by creating pyramid-shaped elements in the

transition region between hex and tet regions.
Requires the hex mesh to be available (or at least a quad mesh at the
shared area).

Hex-to-tet meshing is valid for both quadratic-to-quadratic and linear-toquadratic transitions. Element type must support a 9-node pyramid for
the latter.
Hex Mesh

Transition Layer

Tet Mesh

The mesher first creates all tets, then combines and rearranges the tet
elements in the transition region to form pyramids.
Available only for element types that support both pyramid and tet
shapes, e.g:
Structural SOLID95, 186, VISCO89
Thermal SOLID90
Multiphysics SOLID62, 117, 122
Results are good even in the transition
region. Element faces are compatible
even when transitioning from a linear
hex element to a quadratic tet element.

Quadratic
to
Quadratic
20-Node Hex

13-Node Pyramid

10-Node Tet

8-Node Hex

9-Node Pyramid

10-Node Tet

Linear
to
Quadratic
SOLID95

Meshing

Meshing

...Hex-to-Tet Meshing

...Hex-to-Tet Meshing

Procedure involves four steps:

2. Activate an element type that supports both pyramids and

tets.

1. Create the hex mesh.

Start by map -meshing the regular-shaped volumes. (Or mesh
the shared areas with quads.)

These are usually brick elements that can degenerate into

pyramids and tets. Check the Elements Manual, available online, to find out which element types are valid.

For stress analysis, use either an 8-node brick (SOLID45 or

SOLID185) or a 20 -node brick (SOLID95 or SOLID186).

Examples:
Structural SOLID95, 186, VISCO89
Thermal SOLID90
Multiphysics SOLID62, 117, 122

Meshing

Meshing

...Hex-to-Tet Meshing

...Hex-to-Tet Meshing

3. Generate the tet mesh.

4. Convert degenerate tets to true 10-node tets.

First activate free meshing.

The tet mesh created by the transition mesher consists of

degenerate elements 1 0-node tetrahedra derived from 20node bricks, for example.

Then mesh the volumes that are to be tet-meshed.

Pyramids are automatically generated at the interface.

These elements are not as efficient as true 10-node tets such as

SOLID92, which use less memory and write smaller files during
solution.
To convert the degenerate tets into true tets:
Preprocessor > -Meshing- Modify Mesh > Change Tets...
Or use the TCHG command.

Meshing

Meshing

...Hex-to-Tet Meshing

F. Mesh Extrusion

When you extrude an area into a volume, you can extrude the
area elements along with it, resulting in a meshed volume.
This is called mesh extrusion.

Advantage: Easy to create a volume mesh with all bricks

(hexahedra) or a combination of bricks and prisms.

Obvious requirement: Shape of the volume must lend itself

to extrusion.

Demo:
Resume hextet.db
Show element type list using Element Type > Add/Edit/Delete.
There are two element types: SOLID45 & 95
Bring up MeshTool and set ESIZE,1 (size)
Map -mesh the regular shaped volume
Set element type to 2, and activate tet-meshing
Free-mesh the other volume
Convert degenerate tets to SOLID92
Show element type list. There are now three element types.
Select elements of type 2 (SOLID95 pyramids) and plot elements

Extrude

Meshing

Meshing

...Mesh Extrusion

...Mesh Extrusion

Procedure

2. Mesh the area to be extruded with MESH200 elements.

Use mapped or free meshing with desired mesh density.

1. Define two element types an area

element and a volume element.
Area element: Choose MESH200
quadrilaterals. MESH200 is a meshonly (Not Solved) element and has n o
DOFs or material properties
associated with it.

Preprocessor > MeshTool

3. Choose element extrusion options.
EXTOPT command or Preprocessor >
Operate > Extrude > Elem Ext Opts
Typical options are:

Volume element: Should be

compatible with the MESH200
element type. For example, if you
choose midside nodes for MESH200,
the 3-D solid element should also
have midside nodes.

Active TYPE attribute (should be 3-D

solid).
Number of element divisions in the
extrusion direction (i.e, number of
elements through the thickness).
Must be greater than zero; otherwise,
only the area will be extruded, without
elements.

ET command or Preprocessor >

Element Type > Add/Edit/Delete

Meshing

Meshing

...Mesh Extrusion

...Mesh Extrusion

4. Extrude the area.

First delete concatenated lines, if any. If concatenations are

present, ANSYS will not allow the extrusion operation.
Preprocessor > -Meshing- Concatenate > -Del Concats- Lines
Then extrude the area using any of the extrusion methods.

Demo:
Resume ribgeom.db
Bring up the Element Types dialog, delete PLANE82 element
type, and replace it with MESH200 4-node quad
Also add SOLID45 as element type 2
Bring up MeshTool and set ESIZE,0.1
Choose free quad -meshing and mesh the area
Set extrusion options: TYPE=2, number of element divisions = 4
Rotate view to ISO
Extrude area along normal with offset = 0.4
Save the database to ribvol.db

Meshing

Meshing

G. Sweep Meshing

...Sweep Meshing

Sweep meshing is yet another option available for volume

meshing. It is the process of meshing an existing volume by
sweeping an area mesh.

Advantages:
Target surface
(1 area)

Easy to create a volume mesh with all

bricks (hexahedra) or a combination of
bricks and prisms.

Similar to mesh extrusion, except that the volume already

exists in this case (from a geometry import, for example).

Option to tet-mesh volumes that are

not sweepable . Transition pyramids
are automatically generated.

Requirements:

Source surface
(1 area)

Valid for sweep meshing

Topology of the volume must be

consistent in the sweep direction.
Example: a block with a through hole
(ok even if the hole is tapered).
Source and target surfaces must be
single areas. Concatenated areas are
not allowed for either the source or the
target.
Not valid for sweep meshing

Meshing

Meshing

...Sweep Meshing

...Sweep Meshing

Procedure

Tet -Mesh Option

Define and activate a 3-D hexahedral solid element

type, such as structural SOLID45 or SOLID95.

A useful sweep option is to generate a

tet -mesh in non-sweepable volumes.

Bring up MeshTool and choose Hex/Wedge and

Sweep.

To use this option:

Choose how the source and target surfaces are

identified:
Auto Source/Target means that ANSYS will
automatically choose them based on the volumes
topology.
Pick Source/Target means that you will be
choosing them.

Press the SWEEP button and follow prompt

instructions from the picker. (Or use VSWEEP
command.)

Make sure that the element type supports

degenerate pyramid and tetrahedron
shapes. Examples:
Structural SOLID95, 186, VISCO89
Thermal SOLID90
Multiphysics SOLID62, 117, 122
Choose Preprocessor > -Meshing- Mesh > Volume Sweep-Sweep Opts and activate
the tet-mesh option. (Or use the
EXTOPT,VSWE command.)

Meshing

Meshing

...Sweep Meshing

...Sweep Meshing

Notes

To map -mesh a complex volume, you may need to slice it

several times and also do some area and line concatenations.
For sweep meshing, you typically need only a few slicing
operations, and n o concatenations are needed!
You can control the source area mesh using standard mesh
controls. SmartSizing is generally not recommended since it
is meant for free meshing.

Meshing

H. Workshop

This workshop consists of four exercises:

W8A. Pillow Block
W8B. Connecting Rod
W8C. Cotter Pin
W8D. Wheel

Demo:
Resume ribvol.db
Clear all volumes and all areas, then plot volumes
Bring up MeshTool and activate sweep meshing
Sweep mesh the volume

Loading & Solution

Overview

So far, we have seen how to apply the following types of

loads:
Displacement (DOF constraints)
Pressure and convection (surface loads)
Gravity (inertia loads)

Module 13

Structural temperatures (body loads)

These loads account for four of the five main categories. In

this chapter, we will account for the remaining category
concentrated loads, such as nodal forces in a stress analysis.

Loading & Solution

Loading & Solution

Loading & Solution

...Overview

A. Force Loads

A force is a concentrated load (or

point load) that you can apply at a
node or keypoint.

Point loads such as forces are

appropriate for line element models
such as beams, spars, and springs.

We will cover the following topics in this chapter:

A. Force Loads
B. Nodal Coordinate System
C. Solvers
D. Multiple Load Steps
E. Workshop

In solid and shell models, point loads

usually cause a stress singularity,
but are acceptable if you ignore
stresses in the vicinity. Remember,
you can use select logic to ignore
the elements in the vicinity of the
point load.

Loading & Solution

Loading & Solution

...Force Loads

...Force Loads

In the 2-D solid model shown at bottom left, notice that

maximum stress SMAX (23,854) is reported at the location of
the force.

By unselecting nodes and elements near the bottom corner,

you get the expected stress distribution with SMAX (8,098)
near the top hole.

When the nodes and elements in the vicinity of the force are
unselected, SMAX (12,755) moves to the bottom corner,
which is another singularity due to the displacement
constraint at the corner.

Loading & Solution

Loading & Solution

...Force Loads

...Force Loads

Note that for axisymmetric models:

To apply a force, the following information is needed:

Input values of forces are based on the full 360.

node or keypoint number (which you can identify by picking)

Output values (reaction forces) are also based on the full 360.

force magnitude (which should be consistent with the system of

units you are using)

For example, suppose a cylindrical shell of radius r has an edge

load of P lb/in. To apply this load on a 2-D axisymmetric shell model
(SHELL51 elements, for example), you would specify a force of 2rP.

direction of the force FX, FY, or FZ

Use:

2rP lb

P lb/in

Solution > -Loads- Apply > Force/Moment

Or the commands FK or F

Question: In which coordinate system are FX, FY, and FZ

interpreted?

Loading & Solution

Loading & Solution

B. Nodal Coordinate System

...Nodal Coordinate System

A nodal coordinate system is attached to every node in the

model.

By default, the nodal CS is parallel to global Cartesian, i.e, all

applied forces and displacement constraints are interpreted
in global Cartesian by default.

All forces, displacements, and other direction-dependent

nodal quantities are interpreted in the nodal coordinate
system.
Input quantities:
Forces and moments FX, FY, FZ, MX, MY, MZ
Displacement constraints UX, UY, UZ, ROTX, ROTY, ROTZ
Coupling and constraint equations

Yn

Etc.
Output quantities:

Xn

Yn

Xn

Calculated displacements UX, UY, UZ, ROTX, ROTY, ROTZ

Yn

Reaction forces FX, FY, FZ, MX, MY, MZ

Xn

Etc.
Y
X

Loading & Solution

Loading & Solution

...Nodal Coordinate System

...Nodal Coordinate System

If necessary, you can rotate

the nodal CS to a different
orientation.

Xn

To rotate nodes, use this four- step procedure:

1. Select the desired nodes.
2. Activate the coordinate system (or create a local
CS) into which you want to rotate the nodes, e.g,
CSYS,1.

For example:
To simulate an inclined
roller support.

3. Choose Preprocessor > Move/Modify > -Rotate Node

CS- To Active CS, then press [Pick All] in the picker.

To apply radial forces.

To apply radial constraints
(perhaps to simulate a
rigid, press -fitted pin).

Yn

Or issue NROTAT,ALL.
4. Reactivate all nodes.

Note: When you apply symmetry on antisymmetry boundary conditions, ANSYS

automatically rotates all nodes on that boundary.

Loading & Solution

Loading & Solution

...Nodal Coordinate System

C. Solvers

The function of the solver is to solve the system of linear

simultaneous equations representing the structures degrees
of freedom.

The solution could take anywhere from a few seconds to

several hours depending primarily on the size of the model
and the speed of your computer.

A linear static analysis with one load step requires only one
such solution, but a nonlinear or transient analysis may
require tens, hundreds, or even thousands of solutions.

Demo:
Resume rib.db.
Offset working plane to center of bottom circle (using average keypoint
location).
Create local cylindrical CS at working plane origin.
Select nodes at radius = 0.35 and plot them.
Rotate all selected nodes into active system.
Apply a UX displacement constraint (or an FX force) at all selected
nodes. Note the radial direction.
Now activate global Cartesian (CSYS,0).
Rotate all selected nodes into active system.

Therefore, the type of solver you choose for solution could

be important.

Replot, and note the new direction of the loads.

Loading & Solution

Loading & Solution

...Solvers

...Solvers

The solvers available in ANSYS can be categorized into three

types:
Direct elimination solvers
Frontal
Sparse (default)
Iterative solvers
PCG (Pre-conditioned Conjugate Gradient)
ICCG (Incomplete Cholesky Conjugate Gradient)
JCG (Jacobi Conjugate Gradient)
Parallel Performance solvers (special license required)
AMG (Algebraic Multigrid)
DDS (Distributed Domain Solver)

Direct elimination solvers calculate the

solution as follows:
1. Formulate individual element matrices.

Formulate element
matrices

.emat
file

Assemble
and triangularize
global matrix

.tri
file

Back-substitute
for solution

results
file

2. Read in degrees of freedom (DOF) for the

first element.
3. Eliminate any DOF that has a known
value or can be expressed in terms of
other DOFs, then write an equation to the
.tri file. The remaining DOFs constitute
the wavefront.
4. Repeat steps 2 & 3 for all elements until
all DOFs have been eliminated. The .tri
file now contains a triangularized matrix.
5. Calculate the DOF solution by back
substitution, then use element matrices
to calculate the element solution.

Loading & Solution

Loading & Solution

...Solvers

...Solvers

The wavefront is the number of DOF retained by the solver

during triangularization because they cannot yet be
eliminated. It swells and shrinks as the solution progresses,
and finally becomes zero when all DOF have been eliminated.

Iterative solvers calculate the solution

as follows:
1. Formulate individual element matrices.

The value of wavefront directly affects solution time: the

higher the wavefront, the longer the solution time.

3. Start with an assumed zero value for all

DOF and iterate to convergence (based
on an input tolerance on residual force).

Reordering the elements choosing a proper order in which

elements are processed by the solver can reduce the
wavefront. ANSYS does automatic reordering at the
beginning of a solution.

4. Use element matrices to calculate the

element solution.

The main difference between the

iterative solvers in ANSYS PCG,
JCG, ICCG is the type of pre conditioner used.

Loading & Solution

Loading & Solution

...Solvers

...Solvers

Frontal

When to Use
When robustness is required (nonlinear analysis) or
when memory is limited.

Model Size Memory Disk

(DOFs)
Use
Use
< 50k

Low

High

10k - 500k
When robustness and solution speed are required
(more for
(nonlinear analysis); for linear analysis where iterative
Sparse
shell &
Medium High
solvers are slow to converge (especially for illbeam
conditioned matrices, such as poorly shaped elements). models)
When solution speed is crucial (linear analysis of large
PCG models, especially those with solid elements).

50k 1000k+

High

Low

When solution speed is crucial in multiphysics

ICCG applications. Handles models that have convergence
difficulties with other iterative solvers (nearly indefinite
matrices).

50k 1000k+

High

Low

JCG

When solution speed is crucial in "single-field" problems

(thermal, magnetics, acoustics, and multiphysics).

50k 1000k+

Medium Low

.emat
file

Assemble
global matrix

.full
file

Iterate
to solution

results
file

2. Assemble the global stiffness matrix.

Solver

Formulate element
matrices

Parallel Performance solvers (special license required)

AMG (Algebraic Multigrid)
Iterative solver that can be used in single and
multiprocessor environments
DDS (Distributed Domain Solver)
Decomposes large models into smaller domains, and then
sends those domains to multiple processors for solving.

Loading & Solution

Loading & Solution

...Solvers

D. Multiple Load Steps

To choose a solver:
Solution > -Analysis Type- Soln Control, then choose Soln Options
tab

So far, we have seen how to solve for one set of loading

conditions, i.e, one load step .
Import or create the model

Or use EQSLV command

Mesh it
Apply loads

The default is to use a program chosen solver [ eqslv, -1],

which is usually the sparse direct solver.

Solve (one load step)

Review results

Loading & Solution

Loading & Solution

...Multiple Load Steps

...Multiple Load Steps

A load step can be defined as one set of loading conditions

for which you obtain a solution.

By using multiple load steps, you can:

If you have multiple loading conditions,

you can choose one of two ways:
Solve for all loads together in a single
load step

isolate the structures response to each loading condition.

Or apply each loading condition

separately and solve multiple load steps.

combine these responses in any desired fashion during

postprocessing, allowing you to study different what-if
scenarios. (This is called load case combination and is valid for
linear analyses only. It is covered in Chapter 14.)

There are two ways to define and solve multiple load steps:
Multiple solve method
Load step file method

Loading & Solution

Loading & Solution

...Multiple Load Steps

...Multiple Load Steps

Multiple Solve Method

An extension of the single -load step solution, where you solve

each load step sequentially without
leaving the Solution processor .

Best suited for batch mode.

When used in interactive mode,

this method is useful only for
models that solve quickly.

Load Step File Method

Import or create the model

Mesh it
Apply loads
Solve (load step 1)

In this case, instead of solving each

load step, you write the load step
information to a file, called the load
step file :

Mesh it
Apply loads
Write to LS file (.s01)

Apply different loads

Solution > -Load Step Opts - Write LS

File

Solve (load step 2)

Or use LSWRITE command.

Write to LS file (.s02)

Apply different loads

Etc.

The load step file is named

jobname.s01, .s02, .s03, etc.

Apply different loads

After all load steps have been written

out, you can use one command
LSSOLVE or Solution > -Solve - From
LS Files to read in each file
sequentially and solve it.

Etc.

Review results

Loading & Solution

Loading & Solution

...Multiple Load Steps

...Multiple Load Steps

The advantage of the load step file method is that you can
interactively set up all load steps even for a large model and
then solve them while you are away from the computer.
Note: The loading commands on the load step file are always
in terms of nodes and elements, even if you apply loads on
the solid model.

Apply different loads

Solve (load step 3)

Import or create the model

Write to LS file (.s03)

Solve from LS files
Review results

For both methods:

Loads applied in a previous load step will s t a y in
the database unless they are deleted. So be sure
to delete any loads that are not part of the current
load step.
Results for each load step are appended to the
results file and identified as load step 1, load step
2, etc.
In postprocessing, you first read in the desired
set of results and then review them.
The database contains the loads and results for the
last load step that was solved.

Loading & Solution

Loading & Solution

...Multiple Load Steps

E. Workshop

Demo:

This workshop consists of three exercises:

Resume rib.db

W11A. 3 -D Bracket

Fix left line in UX and bottom line in UY

W11B. Connecting Rod

Apply pressure = 100 on top line

W11C. Wheel

Write LS file 1, then list it and show F.E. load commands

Apply pressure = 50 to 100 (tapered) on right line
Delete the top pressure load
Write LS file 2
LSSOLVE,1,2
Review results for each load step separately

Refer to your Workshop Supplement for instructions.

Postprocessing

Overview

There are many ways to review results in the general postprocessor

(POST1), some of which have already been covered.

In this chapter, we will explore two additional methods query

picking and path operations and also introduce you to the
concepts of results transformation, error estimation, and load case
combination.

We will also introduce two productivity enhancement tools:

Module 14

Postprocessing

Results Viewer

Report Generator

Topics covered:
A. Query Picking

E. Load Case Combinations

B. Results Coordinate System

F. Results Viewer

C. Path Operations

G. Report Generator

D. Error Estimation

H. Workshop

Postprocessing

Postprocessing

A. Query Picking

...Query Picking

Query picking allows you to probe the model for stresses,

displacements, or other results quantities at any picked
location.

You can also quickly locate the maximum and minimum

values of the item being queried.

Available only through the GUI (no commands):

Then pick any point in the model to see the results value at that
point.
Min and Max will show the value at the minimum and
maximum points.
Use Reset to clear all values and start over.
Notice that the entity number, its location, and the results
value are also shown in the Picker.

General Postproc > Query Results > Nodal or Element or Subgrid

Solu...
Choose a results quantity and press OK
PowerGraphics
ON

PowerGraphics
OFF

Automatically
generate text
annotation

Postprocessing

Postprocessing

...Query Picking

B. Results Coordinate System

All direction-dependent quantities that you view in POST1,

such as component stresses, displacements, and reaction
forces, are reported in the results coordinate system (RSYS).

RSYS defaults to 0 (global Cartesian). That is, POST1

transforms all results to global Cartesian by default, including
results at rotated nodes.

But there are many situations such as pressure vessels

and spherical structures where you need to check the
results in a cylindrical, spherical, or other local coordinate
system.

Demo:
Continue from the last multi-load-step solution of rib.db
Plot SEQV for load step 1
Query Nodal Solu SEQV at several locations, including MIN & MAX.
(Switch to full graphics if needed.)
Switch to PowerGraphics and query Subgrid Solu.

Postprocessing

Postprocessing

...Results Coordinate System

...Results Coordinate System

To change the results CS to a

different system, use:

RSYS,SOLU
Sets the results CS to as-calculated.

General Postproc > Options for Outp

or the RSYS command

All subsequent contour plots, listings, query picks, etc. will

report the values in that system.
All subsequent contour plots, listings, query picks, etc. will
report the values in the nodal and element coordinate systems.
DOF results and reaction forces will be in the nodal CS.

Default orientation
RSYS,0

Local cylindrical
system RSYS,11

Global cylindrical
system RSYS,1

Stresses, strains, etc. will be in the element CS. (The

orientation of the element CS depends on the element type
and the ESYS attribute of the element. Most solid elements,
for example, default to global Cartesian.)
Not supported by PowerGraphics.

Postprocessing

Postprocessing

C. Path Operations

...Path Operations

Another way to review results is via path operations, which

allow you to:

Three steps to produce a path plot:

Define a path

map results data onto an arbitrary path through the model

Map data onto the path

perform mathematical operations along the path, including

integration and differentiation

Plot the data

display a path plot see how a result item varies along the
path

1. Define a Path

Available only for models containing 2-D or 3-D solid

elements or shell elements.

Requires the following information:

Points defining the path (2 to 1000). You can use existing
nodes or locations on the working plane.
Path curvature, determined by the active coordinate system
(CSYS).
A name for the path.

Postprocessing

Postprocessing

...Path Operations

...Path Operations

1. Define a Path (contd)

2. Map Data onto Path

First activate the desired coordinate system (CSYS).

General Postproc > Path Operations > Map onto Path (or PDEF
command)

General Postproc > Path Operations > Define Path > By Nodes or On
Working Plane
Pick the nodes or WP locations that form the desired path,
and press OK
Choose a path name. The nSets and nDiv fields are best left
to default in most cases.

Choose desired quantity, such as SX.

Enter a label for the quantity, to be used on plots and listings.
You can now display the path if needed.
General Postproc > Path Operations > Plot Paths
(or issue /PBC,PATH,1 followed by NPLOT or EPLOT )

Postprocessing

Postprocessing

...Path Operations

...Path Operations

3. Plot the Data

ANSYS allows you to define multiple paths, each with

a unique name that you assign. Only one path can be
active at a time.

Besides plots and listings, there are many other path

capabilities, including:

You can plot path items either on a graph:

PLPATH or General Postproc > Path Operations > On Graph...
or along path geometry:
PLPAGM or General Postproc > Path Operations > On
Geometry...

Stress linearization used in the pressure vessel

industry to decompose stress along a path into its
membrane and bending components.
Calculus functions used in fracture mechanics to
calculate J -integrals and stress concentration factors.
Also useful in thermal analyses to calculate the heat lost
or gained across a path.
Dot products and cross products used widely in
electromagnetics analyses to operate on vector
quantities.

Postprocessing

Postprocessing

...Path Operations

D. Error Estimation

The finite element solution calculates stresses on a perelement basis, i.e, stresses are individually calculated in each
element.

When you plot nodal stress contours in POST1, however, you

will see smooth contours because the stresses are averaged
at the nodes.

Demo:
Continue with rib postprocessing
Plot nodes, then switch to CSYS,1 if desired
Define a path using nodes
Map SX or SEQV or other data onto path
Plot the path itself
Plot the path item on graph and on geometry

If you plot the element solution, you will see unaveraged data,
which shows the discontinuity between elements.

Define a second path elsewhere in the model and show how to toggle
between the two.

The difference between averaged and

unaveraged stresses gives an
indication of how good or how bad
the mesh is. This is the basis for error
estimation.

avg = 1100
= 1000 = 1200
Elem 1

Elem 2

= 1100 = 1300
avg = 1200

Postprocessing

Postprocessing

...Error Estimation

...Error Estimation

Error estimation is available only in POST1 and is valid only

for:

Stress analysis:

linear static structural and linear steady-state thermal analyses

percentage error in energy norm (SEPC)

solid elements (2-D and 3 -D) and shell elements

element stress deviations (SDSG)

Full Graphics (not PowerGraphics )

element energy error (SERR)

maximum and minimum stress bounds (SMXB, SMNB)

If these conditions are not met, ANSYS automatically turns

off error estimation calculations.

POST1 calculates the following error measures.

Thermal analysis:
percentage error in energy norm (TEPC)

To manually activate or deactivate error estimation, use

element thermal gradient deviations (TDSG)

ERNORM,ON/OFF

element energy error (TERR)

or General Postproc > Options for Outp ...

Postprocessing

Postprocessing

...Error Estimation

...Error Estimation

Percentage error in energy norm (SEPC)

SEPC is a rough estimate of the stress error (or

displacement, temperature, or thermal flux) over the entire set
of selected elements.

Can be used to compare similar models of similar structures

subjected to similar loadings.

SEPC is shown in the legend column of deformed shape

displays. You can list it manually using PRERR or General
Postproc > List Results > Percent Error .

As a general rule of thumb,

look for SEPC to be 10% or
less. If it is higher, then:

SEPC = 34.5

Check for point loads or

other stress singularities
and unselect elements in
the vicinity.
If it is still higher, plot the
element energy error. The
elements with high values
of energy error are
candidates for mesh
refinement.

SEPC = 10.2

Postprocessing

Postprocessing

...Error Estimation

...Error Estimation

Element stress deviations (SDSG)

Element energy error (SERR)

SDSG is a measure of the amount by

which an elements stress disagrees
with the stress averages at its nodes.

You can plot SDSG contours using

PLESOL,SDSGor General Postproc >
Plot Results > Element Solu...

SERR is the energy associated with the stress mismatches at

the nodes of the element. This is the basic error measure
from which the other error quantities are derived. SERR has
units of energy.

A high value of SDSG is not

necessarily bad, especially if it is a
small percentage of the nominal
stresses in the structure.

To plot SERR contours, issue PLESOL,SERR or General

Postproc > Plot Results > Element Solu...

Generally, the elements with the highest SERR are

candidates for mesh refinement. However, since SERR will
always be highest at stress singularities, be sure to unselect
those elements first.

For example, this plate -with-a -hole

model shows only a 1.5% stress
deviation in the region of interest.

SDSG at location of interest

= ~450 psi, which is ~1.5% of
~30,000 psi nominal stress

Postprocessing

Postprocessing

...Error Estimation

...Error Estimation

Stress bounds (SMXB and SMNB)

The stress bounds can help you determine the potential

effect of mesh discretization error on the maximum stress.

They are displayed on stress contour plots in the legend

column as SMXB (upper bound) and SMNB (lower bound).

The bounds are not estimates of the actual maximum and

minimum, but they do define a confidence band. Without
other supporting verification, you have no basis for believing
that the true maximum stress is below SMXB.

Caution: If you dont unselect elements near stress

singularities, the stress bounds are meaningless, as shown
below.

SMXB = 18,102
SMXB = 4,773

Postprocessing

Postprocessing

E. Load Case Combinations

...Load Case Combinations

Typical procedure:

Whenever you solve multiple load steps, the results of each

load step are stored as separate sets on the results file
(identified by load step number).
A load case combination is an operation between two sets of
results, which are called load cases.

1. Create the load cases

2. Read one load case into the database
3. Perform the desired operation

The operation occurs between one load case in the database

and the second load case on the results file.
The result of the operation the combined load case is
stored back in the database.

Load case in database

(computer memory)

Load case
on results file

Combined load case in database

overwrites previous contents

Postprocessing

Postprocessing

...Load Case Combinations

...Load Case Combinations

Create Load Cases

Read One Load Case into the Database (memory)

Simply identify the results set by its load case

number using LCASE or General Postproc >
Load Case > Read Load Case .

Or use one of the standard Read Results

choices in the postprocessor ( SET command).

A load case simply acts as a pointer to a set of

results. It requires two pieces of information:
a unique ID number
the results set it represents (load step and substep
number)

Use the LCDEF command or General Postproc >

Load Case > Create Load Case

Postprocessing

Postprocessing

...Load Case Combinations

...Load Case Combinations

Perform the Desired Operation

There are two useful options to save the

combined load case:

Many operations are available as shown in the

menu here.

Use the LCOPER command or General Postproc

> Load Case > Add, Subtract , etc.

Writing a load case file (LCWRITE or General

Postproc > Write Results) creates a file that is
similar to, but much smaller than the results file.

Remember that the results of the operation are

stored in the database (memory). The combined
load case is identified on plots and listings as
number 9999 .

The Append option (RAPPND or General

Postproc > Load Case > Write Load Case) allows
you to add the combined load case to the
results file and identify it with a given load step
number and time value.

Write a load case file

Append the load case to the results file

Postprocessing

Postprocessing

F. Results Viewer

The Results Viewer is a

specialized postprocessing
menu and graphic system.
Fast graphics for large models
or models that have many time
steps

Results Viewer

Can be created two different ways

Use the POUTRES command before
solving to write a jobname.pgr file
during solution.
Solution > Output Cntrls > PGR file

Easy to use menu system for

quick results viewing

Hold CTRL key for

multiple selection

Postprocessing

Postprocessing

Results Viewer

Results Viewer

Use the PGWRITE command after

solution to write a jobname.pgr file.
General Postproc > Write PGR File

Open the Results Viewer from the General Post Processor.

Postprocessing

Postprocessing

... Results Viewer

... Results Viewer

Nodal/element/vector/trace
results plots

Query Results

Element
Plot

Animate using
PNG files

The graphics window becomes Context Sensitive.

Context-sensitive graphics window

Right Click on Model

Results Set
Locator

List
Results

Capture/print
image

Postprocessing

Postprocessing

... Results Viewer

... Results Viewer

Context-sensitive graphics window

Context-sensitive graphics window

Right Click on Contour Legend

Right Click on Contour Bar

Postprocessing

Postprocessing

G. Report Generator

Report Generator

Launching the Report Generator will

shrink the graphics window and set
the background to white.

The Capture Tool will be opened

allowing the user to grab plots,
listings, and tables.

A time consuming part of

any analysis is documenting
the model and results. This
procedure has been partially
automated through the
implementation of the
ANSYS Report Generator.
The Report Generator allows
the user to quickly capture
pictures, listings, tables, and
other pertinent information.

Utility Menu> File> Report Generator

or

~eui,euidl::report::toolbar::create

It also facilitates the creation

of an HTML formatted file
ready to be distributed to
colleagues or posted to a
web site.
Capture Tool

Postprocessing

Postprocessing

Report Generator

Report Generator

HTML Assembler . . .

Capture Tool
Animation Capture

Table
Capture

A tool that allows quick

organization of ANSYS graphics,
tables, listings .

Log file can be used as an HTML

template.

The generated HTML file can be

used with Netscape Composer,
Microsoft FrontPage, or any
other HTML editor to finalize the
report.

(multiple PNG files)

Image Capture

utilize parameter substitution

(single PNG file)

Settings

HTML Report
Assembler

The Log File records

all captures!
Listing
Capture

Postprocessing

Postprocessing

Report Generator

Report Generator

Insert TEXT

Insert any HTML FILE

Insert information grabbed using

the Capture Tool

Report Images

Insert an IMAGE

possibly created outside ANSYS

possibly one from an external

source like a digital photo

Insert a Report Heading

Including your name, analysis
title, date, and company name

Report Tables
Material properties, reaction
forces, etc.

Insert DYNAMIC DATA

information specific to your
current ANSYS run like version,
run time, etc.

Contour plots, element plots,

volume plots, graphs

Report Lists
Stress along a path, constraints,
etc.

Postprocessing

Postprocessing

Report Generator

Report Generator

Preview the report

Delete sections of the report

Move sections of the report up

or down

Dynamic Data

Postprocessing

H. Workshop

This workshop consists of five exercises:

W12A. Connecting Rod
W12B. Spherical Shell
W12C. Axisymmetric Fin with Multiple Load Steps
W12D. Results Viewer
W12E. Report Generator

Refer to your Workshop Supplement for instructions.

Mechanical Toolbar

Overview

The Mechanical Toolbar (MTB) is a streamlined GUI designed

to do mechanical analyses quickly and easily:
Linear static analysis
Modal analysis
Steady-state thermal analysis

Module 16

Main advantages of using MTB:

Easy to use. Tabs in the toolbar lead you through the analysis
steps in sequence.

Mechanical Toolbar

Provides more ways to apply loads, such as total force on an

area or line.
Handles multiple loading environments well, with user -assigned
names and automatic book -keeping of files.
Allows you to automatically generate an HTML report of the
analysis.

Mechanical Toolbar

Mechanical Toolbar

...Overview

A Quick Tour

The MTB does have a few limitations, mainly in view of

keeping it simple and easy to use:
No solid modeling capabilities. All geometry is imported via
IGES as well as Connection products. You can also import
geometry from an ANSYS .db file.
Contains only commonly used graphics controls and
postprocessing functions. However, the Utility Menu is available
and provides access to all graphics functions.
No nonlinearities or Multiphysics capabilities.

In this chapter, we will give you a quick guided tour of the

Mechanical Toolbar, followed by a workshop.

To start the MTB, click on Utility Menu > MenuCtrls >

Mechanical Toolbar
The Mechanical Toolbar window will appear, replacing the
Main Menu, Toolbar, and Input window. (If you want to use the
Toolbar or Input window, use Utiliy Menu > MenuCtrls to activate
them.)
If you already have a model in the database, ANSYS will save it
to preMT.db, which you can use later to import the geometry
portion.

Mechanical Toolbar

Mechanical Toolbar

...A Quick Tour

...A Quick Tour

New model,
Resume
model,
Save model

Analysis
sequence tabs

Using the MTB to do your analysis is quite simple

simply use the tabs in sequence from left to right.

And help is available in many forms:

To full
ANSYS

All buttons and menus provide tool tips as well as

prompts.
Most dialog boxes have a Help button that provides
context-sensitive help.
Prompt
area

Hard
copy

The [Tour] button next to [?] provides detailed

explanations of each analysis step.

Status
area

Plot controls

System
utilities:
calculator,
editor

View
fly-out
Plot
fly-out

Also, click the right mouse button on any button or

menu, then click on [Whats This?] to get a brief
description of that item.

Help &
Tour

Mechanical Toolbar - A Quick Tour

Mechanical Toolbar - A Quick Tour

Setup Tab

Model Tab

Use the Setup tab to specify:

The Model tab is used to:

analysis discipline

import geometry

analysis type

assign attributes to geometry

units system

create the mesh. If no mesh is created, MTB will automatically

mesh it during solution.

title
MTB properties

Import
Analysis Title

Assign material

Assign shape
(real constants)

SmartSize
slider

MeshTool

Mesh

Mechanical Toolbar - A Quick Tour

Mechanical Toolbar - A Quick Tour

Load Tab

Solve Tab

The Load tab allows you to:

The Solve tab allows you to solve now or at a specified later time.

specify environment name(s)

apply or delete loads

Symmetry BC

Apply or
Delete

Solve
button

Load
buttons
with fly-outs

Mechanical Toolbar - A Quick Tour

Mechanical Toolbar

Results Tab

A Quick Tour

Use the Results tab to:

review displaced shape and contour plots for the desired environment
query, animate, or list results
generate an HTML report, which can be e-mailed or posted on the web.

Contour, Query, Animate, List

Demo:
Clear the database and start MTB
Setup
change units to inch -lbm-s
type in a title, Plane stress
analysis of a rib
bring up Properties and enter a
user name
Model
import ribgeom.db
change Axisymmetric to Plane
Stress, then enter
Name=1/8thick, Thickness=1/8
set smart-size slider to 4
(notice change in element size
in Mesh button), but do not
mesh

Load
constrain left-side line in UX,
bottom line in UY
100-lb pressure on top line
Solve now
notice that MTB generates the
mesh
Results
animate SEQV
generate report
Click the To ANSYS button. The
model comes up in full ANSYS,
where you can now extend it to
nonlinearities and other complex
analyses.

Workshop

Refer to your Workshop Supplement for instructions on:

W14. Pipe Shell