Element Practical Aspects of Finite Book

2

Contents

Foreword .......................................................................................................................................... 7

About This Book ............................................................................................................................... 9

HyperWorks For Teaching .............................................................................................................. 13

1. CAE-Driven Design Process ......................................................................................................... 17

2 Introduction to Finite Element .................................................................................................... 21

2.1 A Brief Summary ..................................................................................................... 21

2.2 Element Types ......................................................................................................... 54

2.3 Open Source FEM Courses ...................................................................................... 76

3 What is Needed to Run a Finite Element Analysis?..................................................................... 79

3.1 Three Main Stages of a Finite Element Analysis ..................................................... 79

3.2 Modeling / Pre-Processing ...................................................................................... 80

3.3 Solution ................................................................................................................... 83

3.4 Visualization / Post-Processing ............................................................................... 84

4 Analysis Types ............................................................................................................................. 87

5 Getting Started with HyperWorks ............................................................................................. 109

5.1 The HyperWorks Desktop Graphical User Interface ............................................. 109

5.2 Tutorials and Videos .............................................................................................. 119

6 Geometry in HyperMesh ........................................................................................................... 121

6.1 HyperMesh Geometry Terminology ..................................................................... 121

6.2 Geometry Cleanup ................................................................................................ 124

6.3 Geometry Creation and Editing ............................................................................ 133

6.4 Importing CAD Geometry ...................................................................................... 138

6.5 Geometry FAQ’s .................................................................................................... 140

6.6 Recommended Tutorials and Videos .................................................................... 145

6.7 Student Racing Car Project - Introduction and CAD Related Aspects ................... 147

7 Introduction to Meshing ........................................................................................................... 152

7.1 How to Start Meshing ........................................................................................... 152

7.2 Meshing Techniques ............................................................................................. 161

3

7.3 Meshing in Critical Areas ....................................................................................... 163

7.4 Mesh Display Options ........................................................................................... 165

7.5 Mesh density Solution Convergence ..................................................................... 167

8 1D Meshing with HyperMesh ................................................................................................... 170

8.1 When to Use 1D Elements .................................................................................... 170

8.2 Special Features of Beam/Bar Elements ............................................................... 171

8.3 Rigid Elements ....................................................................................................... 175

8.4 Fasteners ............................................................................................................... 177

8.5 1D Element Creation ............................................................................................. 181

8.6 Connectors in HyperMesh..................................................................................... 208

8.7 Learn More About 1D Meshing and Connectors .................................................. 212

8.8 1D Meshing Tutorials and Videos......................................................................... 228

8.9 Student Racing Car Project - 1D Meshing ............................................................. 230

9 2D Meshing with HyperMesh ................................................................................................... 233

9.1 Effect of Biasing in the Critical Region .................................................................. 235

9.2 Symmetric Boundary Conditions........................................................................... 236

9.3 Geometry Associative Mesh ................................................................................. 242

9.4 How Not to Mesh .................................................................................................. 244

9.5 Creating 2D Elements in HyperMesh .................................................................... 251

9.6 Automeshing ......................................................................................................... 252

9.7 Shrink Wrap Meshing ............................................................................................ 256

9.8 Meshing FAQ’s ...................................................................................................... 257

9.9 2D Meshing Tutorials and Videos ......................................................................... 265

10 3D Meshing with HyperMesh ................................................................................................. 267

10.1 3D Element Types ............................................................................................... 267

10.2 Tetra Meshing Techniques .................................................................................. 267

10.3 Brick Meshing ...................................................................................................... 271

10.4 Tips for Brick Meshing ......................................................................................... 274

10.5 How Not to Mesh ................................................................................................ 275

4

10.6 Creating 3D Elements Using HyperMesh ............................................................ 279

10.7 Tutorials and Videos ............................................................................................ 285

11 Element Quality and Checks .................................................................................................... 288

11.1 Compatibility and Mechanisms ........................................................................... 288

11.2 General Element Quality Checks ......................................................................... 292

11.3 2D Quality Checks ............................................................................................... 296

11.4 Other Checks for 2D Meshing ............................................................................. 301

11.5 Quality Checks for Tetra Meshes ........................................................................ 306

11.6 Other Checks for Tetra Meshes .......................................................................... 307

11.7 Brick Mesh Quality Checks .................................................................................. 310

11.8 Other Checks for Brick Meshes ........................................................................... 311

11.9 Mesh Check Tools in HyperMesh ........................................................................ 313

11.10 Mesh Check Tools Tutorials and Videos............................................................ 321

11.11 Student Racing Car Project - Mesh Quality ....................................................... 322

12 Linear Elastic Material ............................................................................................................. 326

12.1 Hooke’s Law and Two Constants ........................................................................ 326

12.2 Generalized Hooke’s Law and 36 Total Constants in the Equation .................... 328

12.3 Material Classification ......................................................................................... 328

12.4 Material Properties ............................................................................................. 329

12.5 Linear Elastic Material and Property Tutorials and Videos ................................. 330

12.6 Student Racing Car Project - Material Definition ................................................ 332

13 Boundary Conditions and Loads.............................................................................................. 342

13.1 Boundary Conditions ........................................................................................... 342

13.2 How to Apply Constraints ................................................................................... 361

13.3 Symmetry ............................................................................................................ 375

13.4 Creating Loadsteps In HyperMesh ...................................................................... 381

13.5 Discussion On AUTOSPC In OptiStruct ................................................................ 382

13.6 Recommended Tutorials and Videos .................................................................. 390

13.7 Student Racing Car Project - Boundary Conditions ............................................. 392

5

14 Linear Static Analysis ............................................................................................................... 396

14.1 Linear Static Analysis ........................................................................................... 396

14.2 Linear Static Analysis Example Using HyperMesh............................................... 397

14.3 Linear Static Analysis Setup Using HyperMesh ................................................... 401

14.4 Linear Static Analysis Tutorials and Videos ......................................................... 413

14.5 Example: Analysis of A Rotating Disc .................................................................. 415

14.6 Student Racing Car Project: Linear Static Analysis .............................................. 424

15 Modal Analysis ........................................................................................................................ 426

15.1 Introduction ........................................................................................................ 426

15.2 Example: Modal Analysis .................................................................................... 430

15.3 Example: Modal Analysis with Constraint Model ............................................... 437

15.4 Tips & Tricks Regarding Post-Processing ............................................................. 440

16 Linear Buckling Analysis ........................................................................................................... 444

16.1 Introduction ........................................................................................................ 444

16.2 Elastic Buckling .................................................................................................... 446

16.3 Linear Buckling Analysis with OptiStruct ............................................................. 448

16.4 Example: Linear Buckling Analysis of a Beam Structure ..................................... 451

16.5 Example: Wing Linear Buckling Analysis ............................................................. 458

16.6 Example: Buckling with Gravitational Load ......................................................... 463

16.7 Linear Buckling Analysis Tutorials and Videos .................................................... 468

17 Post-Processing........................................................................................................................ 470

17.1 How to Validate and Check Accuracy of The Result ........................................... 470

17.2 How to View and Interpret Results ..................................................................... 471

17.3 Post-Processing in HyperView............................................................................. 478

17.4 Stress Calculation and Output in OptiStruct ....................................................... 491

17.5 Special Tricks for Post-Processing ....................................................................... 508

17.6 Interpretation of Results and Design Modifications ........................................... 520

17.7 CAE Reports ......................................................................................................... 527

17.8 Post-Processing Tutorials and Videos ................................................................. 529

6

17.9 Student Racing Car Project: Post-Processing ...................................................... 532

Appendix A ................................................................................................................................... 537

Strategic Planning ......................................................................................................................... 537

Planning the Solution .................................................................................................. 537

Creating a Solution Checklist ...................................................................................... 549

Boundary Conditions and Load Cases ......................................................................... 550

Linear Assumption ...................................................................................................... 557

Appendix B ................................................................................................................................... 561

Common Mistakes and Errors ...................................................................................................... 561

Modeling and Visualization ......................................................................................... 561

Errors Within Organizations ........................................................................................ 566

Appendix C ................................................................................................................................... 575

Consistent Units ........................................................................................................................... 575

Equations Used to Help Determine Consistent Units ................................................. 576

7

Foreword

Simulation has come a long way since it was generally adopted in Aerospace and

Automotive industries in the 1970’s. On the other hand, we still see archaic

terminology such as “card image” when today’s users may have never seen or used

a “card” punch.

Engineers are normally conservative and somewhat slow to change which is a good

thing for the safety aspects of the products they design. But we live in an ever

changing and accelerating technological era. Today, simulation is used in every

industry that designs and manufactures products from toothpaste tubes to rocket

engines. The demand for engineers in the simulation field has never been higher.

The advance of computing is relentless. Today’s mobile devices are more powerful

and can store more information than the supercomputers of the early days of

simulation. The pace of computing continues to grow at an exponential rate even

though a receding growth rate has been predicted many times. The only thing that

is not changing is the basic physics behind the simulation computations. So where

are we going with all of this advance in capability and demand?

The level of detail in the simulation models continues to increase with fewer and

fewer assumptions required to get answers in a reasonable time. As the models

become more complex the requirements for assembling models, analysis of the

results, and storing the volumes of input and output are increasing. Altair is

working to bring the future of simulation to engineers in both an evolutionary and

revolutionary way. We continue to modernize our tradition tools for ease of use,

large model handling, and efficiency and at the same invent new ways of working

for the future generations of engineers.

8

The challenge for the future is to make the complex simple by reducing the

requirements put on the user to get into the details unless necessary or desired.

The simulation process can be more systematic and guided versus more of an art

as it is sometimes today. Two engineers solving the same problem should be able

to get similar results by establishing processes that are repeatable. More realistic

representation of reality can be achieved by stochastic analysis where the variation

of real products is a standard part of the simulation process. Data and processes

can be shared within teams and across teams. Finally, with advance in technology

we will see a return to remote computation or as it is called today cloud computing

which will include high speed 3D graphics. Altair is working in all of the directions

described above to bring the best value and experience to the engineering

community worldwide.

In the document that follows, you will see elements of where we are going. But the

reality is there is a lot to learn and the knowledge you need to successfully apply

simulation is quite vast. Good luck in your endeavours and we hope we can be of

value to you now and throughout your career.

James E. Brancheau, Altair

Altair Engineering

9

About This Book

Over the years Altair has matured into a solver company with OptiStruct (linear and

nonlinear implicit, structural optimization), RADIOSS (non-linear explicit Finite Element

Analysis), solidThinking Inspire (structural optimization), MotionSolve (multibody

simulation), AcuSolve (Computational Fluid Dynamics or CFD), and FEKO (electro-

magnetic field simulation).

Altair has always extended its hands to academia – in the past mainly with regards to

modeling (pre-processing) and visualization (post-processing). Today, Altair’s CAE

offering is more complete and suitable to universities. Thus, we are very grateful that

many universities adopted HyperWorks& solidThinking in their engineering programs in

order to train students in the Simulation-Driven Design and Optimization Process.

The Altair Student Edition 2017 in combination with our learning and teaching program

target the needs of teachers and students.

“It is exciting news that the student version of HyperWorks is now available,”

said Dr. Wei Chen, Wilson-Cook Professor in Engineering Design at

Northwestern University. “This program truly demonstrates Altair’s

commitment to enhancing students’ learning experience outside the

classroom so that they can reinforce their engineering knowledge and

classroom instruction.”

Still, we realized that a dedicated CAE book including some best practice tips were

missing. This was the moment when we decided to publish our CAE expertise in a book

addressing questions typical raised by students.

10

At that time, it so happened that we learned about the book by Nitin S. Gokhale and his

team with the title

Practical Finite Element Analysis (from Finite to Infinite)

An amazing book with the focus on what we were targeting at. Nitin S. Gokhale and his

team immediately agreed to merge their CAE book and Altair’s simulation training

material into this Study Guide.

Even though it is the 5th Edition of this collaborative work, it is by far not complete. The

book still is “Work in Progress”.

This book intends to provide basic information to help the beginner Finite Element

Analysis (FEA) modeler as well as the novice HyperWorks user to get started.

And we know that becoming familiar with a (new) CAE system such as HyperWorks is

somewhat comparable to learning, for instance, a new language. At the same time, we

all face a major challenge: not having enough time. This challenge is universal. This is

because we are educated to constantly increase the pace of our lives and work.

Hence, learning new technologies must be as easy (and as comfortable) as possible.

Otherwise, as practice shows, making the first step is very difficult.

At the beginning there are many questions, such as:

• Where to start?

• Which “rules” are important?

• Where to learn?

• When to learn?

• etc.

11

So how does one become familiar with FEA and become a proficient HyperWorks user?

To support your endeavours in learning more about FEA and HyperWorks, we offer (in

addition to this book):

• The Learning & Certification Program with more than 28 eLearning courses

https://certification.altairuniversity.com/

• Additional free study guides about Nonlinear Finite Element Analysis,

Introduction to Explicit Finite Element Analysis, Introduction to Dynamic Analysis

with OptiStruct, Introduction to Composite Analysis and Optimization, etc…

• Highly discounted seminars at colleges or at Altair facilities,

• Best practice Tips and Tricks,

• Academic User Meetings,

• Academic Blog (altairuniversity.com/academic) to stay up to date with news

about Altair and our technology,

• Moderated Support Forum. If you need help cracking any technical queries

pertaining to Altair’s software suite HyperWorks, please feel free to post your

questions on the moderated Support Forum https://forum.altair.com/

• and more ....

An ideal supplement to this book is the free Altair Student Edition which allows you to

study and practice the various topics addressed in this book.

More information about the Student Edition is available on Altair University

https://altairuniversity.com/academic/.

We are confident that this “ecosystem” will help you get up to speed quickly.

12

And now - enjoy the latest edition of this book and keep on learning and exploring.

Best regards

Dr. Matthias Goelke

On behalf of “The Altair University Team” in cooperation with Finite to Infinite

P.S.: We would appreciate your feedback about your learning experience

(eMail to [e-mail])

13

HyperWorks For Teaching

Leading universities across the globe are using HyperWorks computer aided engineering

(CAE) simulation software for teaching and research in the fields of:

• Structural Analysis

• Computational Fluid Dynamics (CFD)

• Optimization

• Multi-Body Simulation (MBS)

• Electro-Magnetic Simulation (EM)

• Model Based Development and much more!

Altair has commercial expertise to share with the academic community. By including

real life scenarios in your teaching material, Altair can help you add value to your

engineering design courses.

Moreover, we provide teachers and professors curriculum material (PPT’s, reading

material, exercises with model files). This free offer hopefully makes your life easier …

https://altairuniversity.com/teaching-simulation-driven-innovation/

14

Our unique licensing system allows universities to use the entire HyperWorks suite in a

very flexible and cost-efficient way:

*Results may be used for marketing, training and demo purposes

Please let us know your requirements by sending an eMail notification to

[e-mail]

We are more than happy helping and assisting you with your teaching activities.

Non-

commercial

research*

Complimentary

Student Edition

No
limitation on

model size

Entire Suite

Professor 2

Professor 3

Professor 4

Freely accessible
by

other teachers
(same campus)

Support

On-site

seminars/

demos

Teaching

License

15

Acknowledgement

A very special THANK YOU goes to:

Rahul Ponginan (Altair India) who thoroughly reviewed this Study Guide. Rahul’s feedback

significantly improved its quality.

• Premanand Suryavanshi for reformatting and updating the book to the latest version,

• Sanjay Nainani for updating the images in the book, Prajay Solanki for creating and

designing new images.

• Rajneesh Shinde, Nelson Dias, Srirangam R. Srirangarajan, Prakash Pagadala (Altair

India)

• Elizabeth White, Sean Putman, David Schmueser, John Brink, James Brancheau, Lena

Hanna, Ralph Krawczyk, Chad Zamler, Jeff Brennan, and the entire HyperWorks

Documentation Team (Altair USA)

• Tony Gray (Altair Australia)

• Hossein Shakourzadeh (Altair France)

• Baljesh Mehmi, Gareth Lee, Nicola Turner (Altair UK)

• Jan Grasmannsdorf, Thomas Lehmann, Sascha Beuermann, Debdatta Sen, Kristian

Holm, Christian Steenbook, Patrick Zerbe, Marian Bulla, Juergen Kranzeder, Bernhard

Wiedemann, Carolina Penteado, Jacob Tremmel and Moritz Günther (Altair

Germany)

• Markus Kriesch and Andre Wehr (Universität der Bundeswehr München / Germany)

16

Disclaimer

Every effort has been made to keep the book free from technical as well as other

mistakes. However, publishers and authors will not be responsible for loss, damage in any

form and consequences arising directly or indirectly from the use of this book.

© 2019 Altair Engineering, Inc. All rights reserved. No part of this publication may be

reproduced, transmitted, transcribed, or translated to another language without the

written permission of Altair Engineering, Inc. To obtain this permission, write to the

attention Altair Engineering legal department at: 1820 E. Big Beaver, Troy, Michigan, USA,

or call [phone].

17

1. CAE-Driven Design Process

*This chapter includes material from the book “Practical Finite Element Analysis (From Finite to

Infinite)” as well as information from the HyperWorks Help Documentation. Additional material

was added by Matthias Goelke and Jan Grasmannsdorf.

The “CAE-Driven Design Process” has gained significant attraction in most industries such

as aerospace, automotive, biomedical, consumer goods, defense, energy, electronics,

heavy industry, and marine throughout the last years. There are many reasons for the

overall acceptance of CAE as simulation has proven to help with:

• New and inspiring designs

• Products with better quality (e.g. increased material efficiency where less

material = lighter designs)

• Designing faster (i.e. due to shortened development cycles and a reduction in

the number of prototypes by minimizing “Trial and Error” attempts

In other words, simulation saves time, reduces costs, and essentially strengthens the

competitiveness of companies, thus strengthening their market position.

When doing an analysis, we always target optimum designs, but the methods and tools

we use in achieving the optimum design makes a difference. Still, in many “places” the

design process is a trial-and-error process which depends on the selection of the initial

design. This is not a well-established process in terms of how the design evolves and

depends on the engineer’s prior experience. Due to these challenges reaching the best

design is not guaranteed.

To overcome these hurdles, numerical optimization is used to search for and determine

the optimum design.

18

With the Altair Design Approach, a “concept” optimization step is employed early in the

design process which delivers a conceived design proposal.

Starting the CAE process with an optimized concept design sounds contradictory. How

does one start with something being optimized while not really knowing how to start?

19

Without getting lost in detail – the principal working scheme (depicted in the figure

above) is as follows:

1. Define the maximum package/design space. If needed exclude areas/regions

(i.e. non-design space)

2. Finite element mesh the structure (design and non-design area)

3. Assign material properties

4. Apply loads and constraints

5. Specify the objective of the optimization problem (e.g. use minimum

weight/volume only but make sure that certain responses such as

displacements, do not exceed specified threshold values)

This optimization delivers a design concept which answers questions such as where to

remove material, where to place (stiffening) ribs, etc. After the optimization results have

been interpreted and smoothed (in the CAD system) an analysis is carried out to verify

the optimized components performance. Based on these results, another optimization

step may follow, addressing questions such as how to change local geometry in order to

reduce stress peaks or how thick do the stiffening ribs really need to be.

By following this design process, unnecessary redesign loops are eliminated leading not

only to shortened design cycles but also to more competitive products.

“Optimization of a structural part is all about efficient material use. Using OptiStruct takes

the question of material distribution in a design out of the equation and tells you exactly

what you need to do and where the material needs to be. If you use OptiStruct, you can

skip all that messing around with different options, because it gives you the best options

straight away.” (Mark Stroud, Monash Motorsport Team)

20

21

2 Introduction to Finite Element

Analysis

This chapter includes material from the book “Practical Finite Element Analysis (From Finite to

Infinite)” as well as information from the HyperWorks Help Documentation. Additional material

was added by Matthias Goelke and Jan Grasmannsdorf.

2.1 A Brief Summary

As mentioned in the introduction to this guide we deliberately refrained from inlcuding a

chapter about the theory of the Finite Element Method. The reason is rather simple - the

book shelves in the libraries are filled up with thousands of books about FEM already. In

addition, in the web you will find a countless number of online learning material like

reports, FEM lecture notes, videos and so on.

Hence, the table below is meant to give FEM beginners a “feeling” on what is happening

in the background.

22

Methods to Solve Any Engineering Problem

Analytical Method

Numerical Method

Experimental Method

• Classical approach

• 100% accurate results

• Closed form solution

• Applicable only for simple

problems like cantilever and
simply supported beams, etc.

• Complete in itself

• Mathematical representation

• Approximate, assumptions

made

• Applicable even if a physical

prototype is not available
(initial design phase)

• Real life complex problems

• Results cannot be believed

blindly. Certain results must be

validated by experiments
and/or analytical method.

• Actual measurement

• Time consuming and needs

expensive set up

• Applicable only if physical

prototype is available

• Results cannot be believed

blindly and a minimum of 3 to 5
prototypes must be tested

Though analytical methods could

also give approximate results if

the solution is not closed form, in

general analytical methods are

considered as closed form
solutions i.e. 100% accurate.

Finite Element Method: Linear,

nonlinear, buckling, thermal,
dynamic, and fatigue analysis

Boundary Element Method:
Acoustics, NVH

Finite Volume Method:
CFD (Computational Fluid

Dynamics) and Computational
Electromagnetics

Finite Difference Method: Thermal

and Fluid flow analysis (in
combination with FVM)

• Strain gauge

• Photo elasticity

• Vibration measurements

• Sensors for temperature and

pressure, etc.

• Fatigue test

23

Procedure for Solving Any Analytical or Numerical Problem

There are two steps to solving analytical or numerical problems:

Step 1) Writing of the governing equation – Problem definition, or in other words,

formulating the problem in the form of a mathematical equation.

Step 2) Mathematical solution of the governing equation.

The final result is the summation of step 1 and step 2. The result will be 100% accurate

when there is no approximation at either of the steps (analytical method).

Numerical methods make an approximation at step 1 and at step 2, therefore all

numerical methods are approximate.

Analytical “Approximation”

Numerical

“Approximation”

Step 1

Little or no approximation

✓

Step 2

Little or no approximation

✓

Accuracy

High accuracy

Approximate results

Brief Introduction to Different Numerical Methods

1) Finite Element Method (FEM):

FEM is the most popular numerical method.

The Finite Element Method (FEM) is a numerical technique used to determine the

approximated solution for a partial differential equations (PDE) on a defined domain (W).

To solve the PDE, the primary challenge is to create a function base that can approximate

the solution. There are many ways of building the approximation base and how this is

done is determined by the formulation selected. The Finite Element Method has a very

good performance to solve partial differential equations over complex domains that can

vary with time.

24

Applications - Linear, nonlinear, buckling, thermal, dynamic and fatigue analysis. FEM will

be discussed later.

Are FEA and FEM different?

Finite Element Method (FEM) and Finite Element Analysis (FEA) are one and the same.

The term “FEA” is more popular in industries while “FEM” is more popular at universities.

Many times, there is confusion between FEA, FEM, and one more similar but different

term FMEA (Failure Mode Effect Analysis). FEA/FEM is used by design or Research and

Development departments only, while FMEA is applicable to all of the departments.

2) Boundary Element Method (BEM):

This is a very powerful and efficient technique to solve acoustics or NVH problems. Just

like the finite element method, it also requires nodes and elements, but as the name

suggests it only considers the outer boundary of the domain. So, when the problem is of

a volume, only the outer surfaces are considered. If the domain is of an area, then only

the outer periphery is considered. This way it reduces the dimensionality of the problem

by a degree of one and thus solving the problem faster.

The Boundary Element Method (BEM) is a numerical method of solving linear PDE which

have been formulated as integral equations. The integral equation may be regarded as an

exact solution of the governing partial differential equation. The BEM attempts to use the

given boundary conditions to fit boundary values into the integral equation, rather than

values throughout the space defined by a partial differential equation. Once this is done,

in the post-processing stage, the integral equation can then be used again to calculate

numerically the solution directly at any desired point in the interior of the solution

domain. The boundary element method is often more efficient than other methods,

including finite elements, in terms of computational resources for problems where there

is a small surface/volume ratio. Conceptually, it works by constructing a “mesh” over the

25

modeled surface. However, for many problems boundary element methods are

significantly less efficient than volume-discretization methods like FDM, FVM or FEM.

3) Finite Volume Method (FVM):

The Finite Volume Method (FVM) is a method for representing and evaluating partial

differential equations as algebraic equations [LeVeque, 2002; Toro, 1999]. It is very similar

to FDM, where the values are calculated at discrete volumes on a generic geometry. In

the FVM, volume integrals in a partial differential equation that contain a divergence term

are converted to surface integrals, using the divergence theorem. These terms are then

evaluated as fluxes at the surfaces of each finite volume. Because the flux entering a given

volume is identical to that leaving the adjacent volume, these methods are conservative.

Another advantage of the finite volume method is that it is easily formulated to allow for

unstructured meshes. The method is used in many computational fluid dynamics

packages.

4) Finite Difference Method (FDM):

Finite Element and Finite Difference Methods share many common things. In general, the

Finite Difference Method is described as a way to solve differential equation. It uses

Taylor’s series to convert a differential equation to an algebraic equation. In the

conversion process, higher order terms are neglected. It is used in combination with BEM

or FVM to solve thermal and CFD coupled problems.

Finite Difference Method is the discretization of partial differential equations while Finite

Element Method, Boundary Element Method and Finite Volume Method are the

discretization of the integral form of the equations

Question: Is it possible to use all of the methods listed above (FEA, BEA, FVM, FDM) to

solve the same problem (for example, a cantilever problem)?

26

The answer is YES! But the difference is in the accuracy achieved, programming ease, and

the time required to obtain the solution.

When internal details are required (such as stresses inside the 3D object) BEM will lead

to poor results (as it only considers the outer boundary), while FEM, FDM, or FVM are

preferable. FVM has been used for solving stress problems but it is well suited for

computational fluid dynamics problems where conservation and equilibrium is quite

natural. FDM has limitations with complicated geometry, assembly of different material

components, and the combination of various types of elements (1D, 2D and 3D). For

these types of problems FEM is far ahead of its competitors.

Discretization of Problem:

All real-life objects are continuous. This means there is no physical gap between any two

consecutive particles. As per material science, any object is made up of small particles,

particles of molecules, molecules of atoms, and so on and they are bonded together by

the force of attraction. Solving a real-life problem with the continuous material

approach is difficult. The basis of all numerical methods is to simplify the problem by

discretizing (discontinuation) it. In other words, nodes work like atoms and the gap in

between the nodes is filled by an entity called an element. Calculations are made at the

nodes and results are interpolated for the elements.

27

There are two approaches to solve any problem

Discrete (mathematical

equivalent) model, chair

represented by shell and

beam elements, person via

lumped mass at C.G.

From a mechanical engineering point of view, any component or system can be

represented by three basic elements:

Mass ‘m’

Spring ‘k’

Damper ‘c’

All the numerical methods including the Finite Element Method follow the discrete

approach. Meshing (nodes and elements) is nothing but the discretization of a continuous

system with infinite degrees of freedom to a finite degrees of freedom.

Continuous approach

All real-life components

are continous

Discrete approach

Equivalent mathematical

modeling

Discrete
(mathematical
equivalent) model, chair
represented by
shell and beam
elements, person
via lumped
mass at C.G.

K

28

When Can We Say That We Know the Solution to The Above Problem?

If and only if we are able to define the deformed position of each and every particle

completely.

The minimum number of parameters (motion, coordinates, temperature, etc.)

required to define the position and state of any entity completely in space is known

as degrees of freedom (dof)

Consider the following 2-D (planar) problem. Suppose the origin is at the bottom left

corner and is known. To define the position of point A completely with respect to the

origin, we need two parameters i.e. x1 and y1, in other words 2 dofs (translation x and y).

P

Q

Q

y x z

29

Consider that the point A is a part of a line, now one angle should also be defined in

addition to the two translations i.e. 3 dofs (two translations and one rotation).

Suppose points A and B are shifted out of the plane and the line is rotated arbitrarily with

respect to all of the three axes. The minimum number of parameters to define the

position of point A completely would be 6 dofs i.e. 3 translations (Ux , Uy , Uz) and 3

rotations (θx , θy , θz).

DOF is a very important concept. In FEA, we use it for the individual calculation points.

y

x

x 1 y

1

A

B

A

B

y

x

z

30

The total DOFs for a given mesh model is equal to the number of nodes multiplied by

the number of dof per node.

All of the elements do not always have 6 dofs per node. The number of dofs depends on

the type of element (1D, 2D, 3D), the family of element (thin shell, plane stress, plane

strain, membrane, etc.), and the type of analysis. For example, for a structural analysis, a

thin shell element has 6 dof/node (displacement unknown, 3 translations and 3 rotations)

while the same element when used for thermal analysis has single dof /node

(temperature unknown).

For a new user, it is a bit confusing but there is a lot of logical, engineering, and

mathematical thinking behind assigning the specific number of dofs to different element

types and families.

Why Do We Carry Out Meshing? What Is FEM / FEA?

FEM

- A numerical method

- Mathematical representation of an actual problem

- Approximate method

The Finite Element Method only makes calculations at a limited (Finite) number of points

and then interpolates the results for the entire domain (surface or volume).

31

Finite – Any continuous object has infinite degrees of freedom and it is not possible to

solve the problem in this format. The Finite Element Method reduces the degrees of

freedom from infinite to finite with the help of discretization or meshing (nodes and

elements).

Element – All of the calculations are made at a limited number of points known as nodes.

The entity joining nodes and forming a specific shape such as quadrilateral or triangular

is known as an Element. To get the value of a variable (say displacement) anywhere in

between the calculation points, an interpolation function (as per the shape of the

element) is used.

Method - There are 3 methods to solve any engineering problem. Finite element analysis

belongs to the numerical method category.

It is not necessary to remember the mathematical definition of FEM word by word as

given in theoretical text books. Rather what is important is to understand the concept

and then be able to describe it in your own words.

How the Results are Interpolated from a Few Calculation Points

It is ok that FEA is making all the calculations at a limited number of points, but the

question is how it calculates values of the unknown somewhere in between the

calculation points.

This is achieved by interpolation. Consider a 4 noded quadrilateral element as shown in

the figure below. A “quad4” element uses the following linear interpolation formula:

u = a0 + a1 x + a2 y + a3 xy

FEA calculates the values at the outer nodes 1, 2, 3, 4 i.e. a0, a1, a2, a3 are known.

32

4 noded (linear) quad

The value of the variable anywhere in between could be easily determined just by

specifying x and y coordinates in above equation.

For an 8 noded quadrilateral, the following parabolic interpolation function is used:

u = a0 + a1 x + a2 y + a3 xy + a4 x2 + a5 y2 + a6x2 y + a7 xy2

1 2 3

8 noded (parabolic) quad

How is the Accuracy if we Increase the Number of Calculation Points (Nodes and
Elements)?

In general, increasing the number of calculation points improves the accuracy.

Suppose somebody gives you 3 straight lines and asks you to best fit it in a circle, then

find the area of the triangle and compare it with the circle area. This is then repeated with

4, 6, 8, 16, 32 and 64 lines.

1 2 3 4 ? ? ?

8 4 7 5 6

33

By increasing the number of lines, the error margin reduces. The number of straight lines

is equivalent to the number of elements in Finite Element Analysis.

The exact answer for the area of the circle (π r2) is 100. 3 lines gives the answer of 41,

while 4 lines gives 64, and so on. An answer of 41 or 64 is not at all acceptable, but 80 or

90 is, considering the time spent and the relative design concept.

If a higher number of nodes and elements leads to a higher accuracy, then why not always

create a very fine mesh with the maximum possible number of nodes and elements? The

reason is because the solution time is directly proportional to (dof)n.. n can be 1 to 4,

depending on the type of analyses and solver. Also, large size models are not easy to

3

Lines

4

Lines

6

Lines

8

Lines

Shaded Area is Error

34

handle on computers due to the graphics card memory limitations. The analyst has to

maintain a fine balance between the desired level of accuracy and the element size (dof)

that can be handled satisfactorily using the available hardware resources.

Assume the Analytical Method approach gives answers very close to 100 and the time it

takes is 1 month, while the Finite Element Analysis with a reasonable mesh size gives an

answer of 90 within 1 day. In industry, getting fast solutions with logical or reasonable

accuracy is more important than absolute accuracy.

That’s why the analytical method approach is also known as the Scientists way to solve

any problem while the Numerical method is the Engineers way to solve the problem.

Advantages of FEA

• Visualization

• Design cycle time

• No. of prototypes

• Testing

• Optimum design

Visualization of results: For simple geometries such as a simply supported beam or a

cantilever beam, it is easy to visualize the point of the maximum stress and displacement.

But in real life, parts or assemblies with complex geometric shapes are made up of

different materials with many discontinuities subjected to flexible constraints and

complex loading varying with respect to time and point of application. This is further

complicated by residual stresses and joints like spot and arc welds, etc. Because of this, it

is not easy to predict the failure location. Imagine someone shows you a complicated

engine block and asks you to predict the failure location for a given set of forces. It is not

easy to predict it successfully unless you have years of experience in the field. But with

35

tools like CAD and CAE, if modelled in an appropriate fashion, one can easily get stress

contour plots that clearly indicate the locations of high stress or displacement.

Previously, components used to be designed by highly experienced engineers who had

seen a lot of testing and failures of the components in real life. These days, in most

organizations, design engineers are very young, using tools like CAD / CAM / CAE and are

confident about their designs.

What is Stiffness and Why Do We Need it in FEA?

Stiffness ‘K’ is defined as Force/length (units N/mm). Physical interpretation – Stiffness is

equal to the force required to produce a unit displacement. The stiffness depends on the

geometry as well as the material properties.

Consider 3 rods of exactly the same geometrical dimensions – Cast Iron, Mild Steel, and

Aluminium. If we measure the force required to produce a 1 mm displacement then the

Cast Iron would require the maximum force, followed by Steel and Aluminium

respectively, indicating K

CI

> KMS > KAl

36

Mild Steel Mild Steel Mild Steel

Now consider 3 different cross sectional rods of the same material. Again, the force

required to produce a unit deformation will be different. Therefore, stiffness depends on

the geometry as well as the material.

Importance of the stiffness matrix - For structural analysis, stiffness is a very important

property. The equation for linear static analysis is [F] = [K] [D]. The force is usually known,

the displacement is unknown, and the stiffness is a characteristic property of the

element. This means if we formulate the stiffness matrix for a given shape, like line,

quadrilateral, or tetrahedron, then the analysis of any geometry could be performed by

meshing it and then solving the equation F = K D. Methods for formulating the stiffness

matrix –

1) Direct Method

2) Variational Method

3) Weighted Residual Method

The direct method is easy to understand but difficult to formulate using computer

programming. While the Variational and Weighted Residual Methods are difficult to

understand, but easy from a programming point of view. That’s the reason why all

software codes either use the Variational or Weighted Residual Method formulation.

37

Rod Element Stiffness Matrix Derivation by The Direct Method

Methodology for derivation of stiffness matrix by the direct method:

Assume there are n dof’s for a given element (for example, a quad4 element’s total dofs

= 4*6 = 24).

Step 1) Assume the 1st dof ≠ 0, and all the other dof = 0. This will lead to equation 1.

Step 2) Assume the 2nd dof ≠ 0, and all the other dof = 0. This will lead to equation 2.

:

:

Step n) Assume the nth dof ≠ 0, and all the other dof = 0. This will lead to equation n.

Step n+1) Sum all the equations, 1 + 2 + 3 + 4 ………..+ n.

Step n+1 will give us the most generalized formulation of the stiffness matrix.

Stiffness matrix formulation (Direct Method)

U

i

F

i

i

j

38

Case 1:

ui >0, uj=0

∑Fx = 0 Fi + Fj =0 Fi = -F

j

σx = F/A ε = u/L

σx = ε E F/A= Eu/L

Fi = (AE/L)*ui Fj = -Fi = - (AE/L)*ui ………...…….. (A)

Case 2: ui =0 uJ>0

Fj = (AE/L)*uj Fi = -Fj = - (AE/L)*uj ………… (B)

U

Fi = -F

j

Case 3: General case - ui , uj > 0

From (A) and (B)

Fi = (AE/L)*ui – (AE/L)*uj

Fj = -(AE/L)*ui + (AE/L)*uj

i

j j F

j

STATICS

∑F x = 0

∑M x = 0

∑F

y

= 0

∑M y = 0

∑F

z

= 0

∑M z = 0

39

Properties of the stiffness matrix

• The order of the stiffness matrix corresponds to the total dofs.

• A singular stiffness matrix means the structure is unconstrained and has rigid

body motion.

• Each column of the stiffness matrix is an equilibrium set of nodal forces

required to produce the unit respective dof.

• A symmetric stiffness matrix shows the force is directly proportional to

displacement.

• Diagonal terms of the matrix are always positive meaning a force directed in

say the left direction cannot produce a displacement in the right direction.

Diagonal terms will be zero or negative only if the structure is unstable.

Rod elements support only tension or compression and no shear force or bending. In the

above equation, the order of the stiffness matrix is 2x2, where the number of unknowns

is 2.

Number of unknowns = no. of dofs - no. of dofs constraint by a Single Point Constraints

(at fixed nodes, dofs are specified by the user as 0)

Usually in comparison to the total dofs for the model, the constraints are negligible and

therefore the total no. of unknowns is approximately the total dofs.

The order of the stiffness matrix = total dof x total dof

40

Summary - Stiffness Matrix, Assembly of 2 Rod Elements

F

Because of a force at point 3, what would the force be at Points 1 and 2? Before reading

the answer, please shut your eyes and try to visualize the forces at the various points.

For equilibrium Σ Fx = 0. The reaction force at point 1 is –F and at point 2 = 0.

The free body diagram is:

-F F

2b 3

Total force at point 2 = - F + F = 0

In any finite element model, the summation of forces and moments is zero at the internal

nodes (except the nodes which are restrained and at which the external force and

moment is applied). The overall summation of the forces and the moments for the

complete model is 0. (The external forces and moments = the reaction forces and

moments). This is one of the important checks for ensuring correct results.

1 2 3

A 1 E 1 L 1 A 2 E 2 L

2

F 1 2

a

A 1 E 1 L

1

-

F

A 2 E 2 L

2

41

Example: Assembly of 2 rod elements

K1 = A1E1 / L1 = 104 N/mmK2 = A2E2 / L2 = 2 * 104 N/mm

A 1 E 1 L 1 A 2 E 2 L 2 1 2 3

F = 1000 N

R = 2 mm

L

1

= 259.74

L = 519.48

R = 4 mm

42

Some more discussion on assembly the global stiffness matrix from the local stiffness
matrices for 1D bar elements. (found on Youtube, recording by Jack Chessa)

43

We need to understand that in the before depicted “Force - Stiffness - Displacement”

relationship the global and local coordinate system are the same (element is oriented in

x-direction). Typically, they are different. Hence, local and global quantities are “linked”

through a transformation matrix as shown below.

For the more general case – which we will have a look at next – local quantities are

marked as

with

In order to take displacements in y-direction into account

we are expressing the displacements d in node 1 with respect to the local and global

coordinate system.

44

The displacements in the global coordinate system are written as .

From the image above, we can directly derive:

Written in Matrix form

45

Including node 2 of the element, the above equation may be written as

alternatively

With T being the transformation matrix: Multiplying global quantities  with T

transforms them into local quantities Nodal forces may be written in the same

way:

alternatively

Quite obviously, if global quantities are requested, we need to rearrange the above

equation.

Here it is

thus

As we already know, multiplying local quantities with  transforms into global

quantities.

More generally, we include the nodal forces (node 2) in our equation from above (here

and are 0).

46

Taking into account

from above follows

And again, making use of

and

results in

or simply

with

Let’s have a look at the matrix

node 1) and

47

The [ ] matrix is commonly abbreviated as

Example

Let’s apply these basics to the following “problem” which was originally formulated by

Professor B. Wender (University Ulm / Germany).

Objective: Determine the nodal displacements and the force in element I

Given:

48

Let us first determine the values of regarding every element, respectively.

Units in kN and mm.

Element I

  

c2 = 0; s2 = 1; cs = 0

 

49

Element II

  

c2 = 0,3622; s2 = 0,6378; cs = 0,4806

 

Element III

  

c2 = 0,6710; s2 = 0,3280; cs = 0,4698





 

50

Force equilibrium

51

With above the system of equations may be written as:

Taking the constraints:

into account leads to the 2 equations

and

Force in element I (with values from above)

35,784 kN

The corresponding simulation results based on OptiStruct are shown below. Note: The

model set-up and analysis are discussed in Chapter “Linear Static Analysis”.

52

Displacements in uy - direction (-0.492 mm)

Displacements in ux- direction (0.939 mm)

53

Principal Stresses

Force in element I

In case you are not experienced with truss structures you may like the lesson (video

below) on solving a truss (not related to FEA).

Topics covered include determining whether the truss is statically determinate, finding

external reaction forces, and finding internal forces

(https://www.youtube.com/watch?v=qzmeFq8rckw)

54

2.2 Element Types

In the following, mostly used element types are listed. Their number of nodes and

DOFs are given so that the user understands the compatibility between different

element types – matching DOFs number.

Rod Element

Example of rod element

Nodes 2 nodes

DOFs 3 or 6 degrees of freedom per node

Beam Element

Example of beam element

Nodes 2 nodes

DOFs 6 degrees of freedom per node

55

Shell Element

Example of shell elements (CTRIA3, CQUAD4, CTRIA6, CQUAD8)

First Order 4 or 3 nodes

Second Order 6 or 8 nodes

DOFs 6 degrees of freedom per node

Solid Element

Example of tetrahedron, pyramid, penta and hexa elements

56

First Order 4, 5, 6, 8 nodes

Second Order 8, 12, 15, 20 nodes

DOFs 3 degrees of freedom per node

Higher Order Elements

Higher order elements are those with one or more mid-side nodes, or geometry based

elements, such as p-version elements. These types of elements offer the benefits of ease

of modeling and a higher degree of accuracy per element. P-version type elements also

have a built-in ability to check convergence by increasing the integration level although

it is more difficult to understand their fundamental behavior.

Higher order elements give rise to issues such as the sophisticated methods required to

apply pressure to the face of a shell element. The required distribution of nodal loads to

accomplish the same resultant force (F=P*A) on a 4 -node and an 8-node shell element is

shown below.

Consistent Pressure Loads for Shells (F = P x A)

57

Most codes handle these details, but you should understand these and the other

fundamentals of higher order elements to avoid confusion. Higher order elements are

most often used in 3-D solid modeling because the potential to reduce modeling effort

and the number of elements required to capture the geometry is greater. Solution time

is not often reduced however because the global stiffness matrix is based on nodal DOF

in the model.

Formulations for 2D elements

1) Plane Stress

Degrees of Freedom (DOFs) – 2 / node {Ux, Uy (in-plane translations)}

Stress in z direction (thickness) is zero (σz = 0)

S

z

Practical Applications: Thin sheet metal parts, like aircraft skin, narrow beams.

2) Plain Strain - DOFs – 2 / node {U

x

, Uy (in-plane translations)} Strain in z direction

(thickness) is zero (εz = 0)

y x

Total dof = 8

U

y

U

x

U

y

U

x

U

y

U

x

U

y

U

x

y x

Total dof = 8

U

y U x U y U x

U

y

U

x

U

y

U

x

58

z

Practical Applications: Under ground pipes, wide beams, dams

Plane stress and plane strain elements are used for 2D (planar) problems.

3) Plate - DOFs – 3 / node {θ

x

, θy (in plane rotations) + Uz (out of plane translation)}

Practical Applications: Bending load application.

Plate elements are three- or four-node elements formulated in three-dimensional

space. These elements are used to model and analyze objects such as pressure

vessels, or structures such as automobile body parts. The out-of-plane rotational

DOF is not considered for plate elements. You can apply the other rotational DOFs

and all the translational DOFs as needed. Nodal forces, nodal moments (except when

about an axis normal to the element face), pressures (normal to the element face),

acceleration/ gravity, centrifugal and thermal loads are supported. Surface-based

loads (pressure, surface force, and so on, but not constraints) and element

properties (thickness, element normal coordinate, and so on) are applied to an

entire plate element. Since these items are based on the surface number of the lines

forming the element, and since each element could be composed of lines on four

different surface numbers, how these items are applied depend on whether the

mesh is created automatically (by either the mesher from a CAD model or the 2D

mesh generation), or whether the mesh is created by hand. The surface number of

Total dof = 12

y z x

θ

y

θ

x U z

θ

y

θ

x

U

z

θ

y

θ

x

U

z

θ

y

θ

x U z

59

the individual lines that form an element are combined as indicated in the table

above to create a surface number for the whole element. Loads and properties are

then applied to the entire element based on the element’s surface number 4)

Membrane - DOFs – 3 / node {Ux, Uy (in plane translations) + θz (out of plane

rotation)}

Practical Applications: Balloon, Baffles

4) Thin Shell - Thin shell elements are the most general type of element.

DOFs: 6 dof / node (Ux , Uy , Uz , θx , θy , θz).

Thin Shell

(Ux , Uy , Uz , θx , θy ,

=

Plate

Membrane

+

θz)

=

Uz, θx, θy

+

Ux , Uy ,

θz

(3T+3R)

=

(1T+2R)

+

(2T+1R)

Total dof = 12

y

z

x

U

y

U

x

θ

z

U

y

U

x

θ

z

U

y

U

x

θ

z

U

y

U

x

θ

z

60

Practical Application: Thin shell elements are the most commonly used elements.

5) Axisymmetric Solid - DOFs - 2 / node {U

x

, Uz (2 in plane translations, Z axis is axis

of rotation)}

Why is the word ‘solid’ in the name of a 2D element? This is because though the

elements are planar, they actually represent a solid. When generating a cylinder in

CAD software, we define an axis of rotation and a rectangular cross section. Similarly,

for an axisymmetric model we need to define an axis of rotation and a cross section

(planar mesh).

The 2D planar mesh is mathematically equivalent to the 3D cylinder.

Practical Applications: Pressure vessels, objects of revolutions subjected to axisymmetric

boundary conditions

y x

U y U x U y U x

U

y

U x

U

y

U x

61

Summary of element types:

Side Note: Why is 2D Meshing Carried Out on A Mid Surface?

Mathematically, the element thickness specified by the user is assigned half on the

element top and half on the bottom side. Hence, in order to represent the geometry

appropriately, it is necessary to extract the mid surface and then mesh on the mid

surface.

Midsurface

t - thickness of plate

t

t

62

Practical example: All sheet metal parts, plastic components like instrument panels, etc.

In general, 2D meshing is used for parts having a width / thickness ratio > 20.

Limitations of Mid Surface and 2D Meshing

2D meshing would lead to a higher approximation if used for

- variable part thickness

surfaces are not planar and have different features on two sides.

Constant Strain Triangle (CST) Information

Some remarks regarding the Constant Strain Triangle (CST) element.

The explanation below is taken from:

The CST (Constant Strain Triangle) –An insidious survivor from the infancy of FEA, by R.P.

Prukl, MFT (this paper is also uploaded to the

Academic Blog; https://altairuniversity.com/wp-

content/uploads/2013/06/The_CST.pdf

The CST was the first element that was developed for finite element analysis (FEA)

and 40-50 years ago it served its purpose well. In the meantime, more accurate

elements have been created and these should be used to replace the CST.

63

The Explanation

Consider a 3-noded plane stress element in the xy-plane with node points 1, 2 and

3. The x-deflections are u1, u2, u3 and the y-deflections v1, v2 and v3, totalling six values

altogether.

The displacement function then has the following form (using six constants ai to describe

the behavior of the element):

The direct strains can then be calculated by differentiation:

What Does This Mean?

The strains in such an element are constants. We know, however, that in a beam we

have compression at the top and tension at the bottom. Our single element is,

therefore, not capable of modelling bending behavior of a beam, it cannot model

anything at all. Note: Three-noded elements for other applications than plane stress

and strain are quite acceptable, e.g., plate bending and heat transfer.

The Remedy

Use elements with four nodes. We then have eight constants to describe the behavior of

the element:

64

The direct strains are then as follows:

The strain in the x-direction is now a linear function of its y-value. This is much better

than for the triangular element. Use triangular elements which also include the

rotational degree of freedom about the z-axis normal to the xy-plane.

65

For a Given FE Model, How Many Equations Does a Software Solve?

Assume there are 20,000 nodes for a mesh model consisting of only thin shell elements

(6 dof/node).

Total dofs = 20000*6 = 120,000.

Stiffness matrix order = 120,000x120,000

Number of equations the FEA software will solve internally = 120,000

Can we solve the same problem using 1D, 2D and 3D elements?

Is it not possible to use 3D elements for long slender beams (1D geometry), for sheet

metal parts (2D geometry), and 2D shell elements for representing big casting parts?

The same geometry could be modelled using 1D, 2D, or 3D elements. What matters is the

number of elements and nodes (DOF), the accuracy of the results, and the time consumed
in the analysis.

For example, consider a cantilever beam with a dimension of 250 x 20 x 5 mm that is

subjected to a 35 N force:

1 D beam

N=2

Total DOF = 6 x 2 = 12

N = 909 E =

Total dof = 909 x 6 = 5454

2

D shell

66

Table (see next page) on The Equivalence of Variational FEM and Weighted Residual
FEM in Solid Mechanics

The problem: A one dimensional rod element is subjected to a concentrated tensile force

at one end (free end) and the other end is fixed as discussed above.

The governing differential equation and boundary conditions:

Nodes

Elements

Stress

N/mm2

Displacement

mm

Analytical

--

--

105

4.23

1D

2

1

105

4.23

2D

909

800

103

4.21

3D

17,448

9,569

104

4.21

N = 17,448 E =

Total dof = 17,448 x 3 = 52,344

3

D Tetra

67

AE (d2u/dx2) = 0

u |

x =0

=0

AE (du/dx) |

x=L

= P

68

Thin Shell Elements – element size vs accuracy

In the following we investigate the “performance” of quad and tria-elements by

looking at a plate with a circular hole. The modeling results are then compared with

a given analytical answer.

Analytical Answer

The Stress Concentration Factor (SCF) is defined as = max. stress / nominal stress

In this example the nominal stress is = F/A = 10,000

N/ (1000 mm*10 mm) =1 N/mm

2

for an infinite plate

SCF =3

Hence, the maximum stress = Stress Concentration Factor (SCF) * nominal stress = 3

N/mm2

In the first part of this study the effects of element type (quad versus tria elements) on

the modeling results are investigated. The global mesh size is 100.

The boundary conditions for all models are the same: the translational degrees of

freedom (x-, y-, z- displacements=0) of all nodes along the left edge of the model are

constrained (green symbols) whereas the nodes along the right edge are subjected

to forces in the x-direction (total magnitude 10.000 N).

1

,000

1

mm

Ф

10

10

69

In order to better control the mesh pattern surrounding the hole, two so called

“washers” have been introduced (i.e. the initial surface is trimmed by two circles

with a radii of 45 mm and 84 mm, respectively.

In the stress contour plots shown below, the maximum principal stress is depicted,

respectively. Note that by default the element stresses for shell (and solid elements)

are output at the element center only. In other words, these stresses are not exactly

the ones “existing” at the hole. To better resolve the stresses at the hole, the element

stresses are output at the grid points using bilinear extrapolation (in HyperMesh

activate the Control cards > Global output request > Stress > Location: Corner).

Effect of Element Type (quads vs trias)

Model 1: The hole is meshed with 16 tria elements. The maximum principal stress

(corner location) is 2.32 N/mm2 (the analytical result is 3 N/mm2).

70

Model 2: The hole is meshed with 16 quad elements. The maximum principal stress

(corner location) is 2.47 N/mm2 (the analytical result is 3 N/mm2).

Despite the fact, that both results differ significantly from the analytical reference

value of 3 N/mm2, it is apparent that the quad elements (17 % error) are “better”

71

than tria elements (23 % error). All in all, both models are inappropriate when it

comes to quantitatively assessing the stresses at the hole.

Moreover, another even more important lesson to be learned is that the FEM program

does not tell you that the mesh is inacceptable

– this decision is up to the CAE engineer

Effect of Mesh Density

In the following the effect of element size, i.e. number of elements at the hole, on the

modeling results is discussed.

Model 3: The hole is meshed with 4 quad elements. The maximum principal stress

(corner locati on) is 1.60 N/mm2 (the analytical result is 3 N/mm2).

Model 4: The hole is meshed with 8 quad elements. The maximum principal stress

(corner location) is 2.06 N/mm2 (the analytical result is 3 N/mm2).

72

Model 5: The hole is meshed with 16 quad elements. The maximum principal stress

(corner location) is 2.47 N/mm2 (the analytical result is 3 N/mm2).

73

Model 6: The hole is meshed with 64 quad elements. The maximum principal stress

(corner location) is 3.02 N/mm2 (the analytical result is 3 N/mm2).

Element Type

# Elements at
Hole

Stress (N/mm2)

(corner location)

Model 1

Tria

16

2.32

Model 2

Quad

16

2.47

Model 3

Quad

4

1.6

Model 4

Quad

8

2.0

Model 5

Quad

16

2.47

Model 6

Quad

64

3.02

74

Conclusion:

The conclusion from the first exercise was that quad elements are better than

triangular elements. As indicated by the results shown before: the greater the

number of elements in the critical region (i.e. hole), the better its accuracy.

While we have been looking at linear elements (nodes at the element corners only),

Professor Dieter Pahr (University Vienna, Austria), documented the differences

between second order tria and quad elements. His study is also based on a plate

with a hole. The image below is taken from his course notes: “Modeling, Verification

and Assessment of FEM simulation Results”.

In the figure above, the von Mises stress is depicted for linear and second order

quad- and tria- elements. The vertical axis is error (%), and the horizontal axis is

number of elements at ¼ of the hole

In this image, the displacements at the hole is depicted for linear and second order quad-

and tria- elements

75

Conclusion:

Second order quad elements behave/perform best, whereas linear trias are

“problematic”. These element related effects are less severe while looking at

displacements (nodal results).

If this is so, then why not always create a very fine mesh with the maximum possible

number of nodes and elements? Why is the usual guideline for meshing 12-16

elements around holes in critical areas?

The reason is because the solution time is directly proportional to the (dof)2. Also

large size models are not easy to handle on the computer due to graphics card

memory limitations. Analysts have to maintain a fine balance between the level of

accuracy and the element size (dof) that can be handled satisfactorily with the

available hardware configuration.

76

2.3 Open Source FEM Courses

There are literally thousands of recorded FEM lectures available on the web (especially

YouTube).

For instance, the lecture by Dr. Cynthia Furse, University of Utah (related to

electromagnetic field simulation (http://youtu. be/9uPxFZ_T3ok)

or the lecture series by Prof. K.J. Bathe (http://youtu.be/20WSeL4tz2k)

This video series is a comprehensive course of study

that presents effective finite element procedures

for the linear analysis of solids and structures.

Professor K. J. Bathe, teaches the basic principles

used for effective finite element analysis, describes

the general assumptions, and discusses the

77

implementation of finite element procedures. Upon completion of this video course, a

second course covering Nonlinear Analysis is available.

Professor Chessa, University of Texas, El Paso (http://youtu.be/CBypsx_u3M8)

Prof. C.S. Uppadhay Department of Aero Space IIT Kanpur

(http://youtu.be/NYiZQszx9cQ)

78

Introduction to Finite Element Method by Dr. R. Krishnakumar, Department of

Mechanical Engineering, IIT Madras. This introduction consists of a series of 33 videos.

For more details on NPTEL visit http://nptel.ac.in

https://www.youtube.com/watch?v=KR74TQesUoQ&list=PLbMVogVj5nJRjnZA9oryB

mDdUNe7lbnB0

Again, these are just a few classes we came across by looking for public FEA classes. In

case you like to add (or recommend) other classes, please let us know.

Just drop a mail to [e-mail]

79

3 What is Needed to Run a Finite

Element Analysis?

This chapter includes material from the book “Practical Finite Element Analysis (From Finite to

Infinite)”. It also has been reviewed and has additional material included by Matthias Goelke and

Jan Grasmannsdorf.

3.1 Three Main Stages of a Finite Element Analysis

In a high-level summary, the “working” steps involved in a finite element analysis may be

categorized as:

• Modeling (pre-processing)

• Solution

• Visualization of solution results (post-processing)

This image depicts the three elementary working steps involved in a FEM analysis. Some

details about the individual steps are summarized below.

80

3.2 Modeling / Pre-Processing

CAD Data

Most commonly, an FEM simulation process starts with the import of the component’s

(or part’s) CAD geometry (e.g. CATIA, STEP, UG, IGES, solidThinking, etc.) into the pre-

processor i.e. HyperMesh

Geometry Clean-up

In many cases, the imported geometry is not ready for meshing. Quite often the geometry

needs a cleanup first due to

• “broken” surfaces

• surfaces which are not stitched together

• redundant (multiple) surfaces

• surfaces which are too small to be meshed in a reasonable way later on

• many other geometry failures

Another issue related to geometry is depicted in the following image:

In the image on the left, the imported geometry is shown. Note the lateral offset of the

green edges. Here, the surface edges (in green) do not meet at a single point i.e. there is

a very small lateral offset of the surface edges. As meshing is carried out with respect to

the surfaces, this small offset will be automatically taken into account during meshing,

which, unfortunately will result in very poor-quality elements. The image in the middle

depicts the meshed “initial” geometry. Note how the mesh is locally distorted. The

updated (cleaned) and meshed geometry is shown on the right.

81

Here, the surface edges (in green) do not meet in a single point, i.e. there is a very small

lateral offset of the surface edges. As meshing is carried out with respect to the surfaces,

this small offset will be automatically taken into account during meshing, which,

unfortunately will result in very poor-quality elements.

Once these “hurdles” are mastered, one needs to ask whether all the CAD information is

really needed. What about little fillets and rounds, tiny holes or even company logos

which can often be found in CAD data? Do they really contribute to the overall

performance of the component?

Meshing

Once the geometry is in an appropriate state, a mesh is created to approximate the

geometry. Either a beam mesh (1D), shell mesh (2D) or a solid mesh (3D) will be created.

This meshing step is crucial to the finite element analysis as the quality of the mesh

directly reflects on the quality of the results generated. At the same time, the number of

elements (number of nodes) affects the computation time. That is the reason why in

certain cases a 2D and 1D mesh is preferred over 3D mesh. For example, in sheet metals

a 2D approximation of the structure uses much less elements and thus reduces the CPU

time (which is the time while you are waiting for your results).

82

See the picture above for structures that are typically meshed with 1D, 2D and 3D

elements. Which element type would you choose for which part?

Despite the fact that meshing is (at least optionally) a highly automated process, mesh

quality, its connectivity (i.e. compatibility), and element normals needs to be checked. If

necessary, these element “issues” may need to be improved by updating (altering) the

underlying geometry or by editing single elements.

Material and Property Information

After meshing is completed, material (e.g. Young’s Modulus) and property information

(e.g. thickness values) are assigned to the elements.

Loads, Constraints and Solver Information

Various loads and constraints are added to the model to represent the loading conditions

that the part(s) are subjected to. Different load cases can be defined to represent

different loading conditions on the same model. Solver information is also added to tell

the solver what kind of analysis is being run, which results to export, etc.

To determine your relevant loads, your engineering skills are needed. Think of all kinds of

load situations that can occur on your structure and decide whether you want to use

them in your simulation or not. To determine the load from a static or dynamic event, a

Multibody Simulation (MBS) might be helpful.

The FEM model (consisting of nodes, elements, material properties, loads and

constraints) is then exported from within the preprocessor HyperMesh. The exported

FEM model, typically called solver input deck, is an ASCII file based on the specific syntax

of the FEM solver chosen for the analysis (e.g. RADIOSS or OptiStruct). A section out of

an OptiStruct solver deck is depicted in the figure below.

83

As you will see, the bulk of information stored in the analysis file is related to the

definition of nodes (or grids). Each single node is defined by its nodal number (ID) and its

x-, y- and z coordinates. Each element is then defined by its element number (ID) and its

nodes (IDs are referenced). This completes the pre-processing phase.

3.3 Solution

During the solution phase of a simple linear static analysis or an eigenfrequency study,

there is not much for you to do. The default settings of the Finite Element program do

handle these classes of problems pretty well. Practice will show you that if the solution

process is aborted by an “error”, it is due to mistakes you have made during the model

building phase. Just to mention a few typical errors:

• Element quality (http://altair-2.wistia.com/medias/rmretoumym)

• Invalid material properties

• Material property not assigned to the elements

• Insufficiently constrained model (the model shows a rigid body motion due to

external loads)

84

Some of these model issues are discussed in additional videos/webinars available on the

Learning Library (https://altairuniversity.com/learning-library/)

3.4 Visualization / Post-Processing

Once the solution has ended successfully, post-processing (in HyperView for contour

plots and HyperGraph for 2D/3D plots) of the simulation results is done next. Stresses,

strains, and deformations are plotted and examined to see how the part responded to

the various loading conditions. Based on the results, modifications may be made to the

part and a new analysis may be run to examine how the modifications affected the part.

This eventually completes the FEM process.

Remarks

Practice will show, that in many projects, the above depicted process must be re-entered

again, because simulation results indicate that the part is not performing as requested. It

is quite obvious that going back to CAD (to apply changes) and working through the entire

FEM process becomes tedious.

85

Note:

The individual working steps of the FEM process are not only subjected to many “user”

errors e.g. typo while defining material or loads. A lot of attention must also be paid to

the chosen modeling assumptions (for instance, simplification of geometry, chosen

element type and size, etc.). Even though the FEM solver may detect some of the most

striking errors, the likelihood that your results have bypassed “errors” is high.

The following chapters aim at creating awareness about FEM challenges and pitfalls.

A very efficient (and exciting) technology to speed up this process is called Morphing.

Employing morphing allows the CAE engineer to modify the geometry of the FEM model,

i.e. apply a shape change to an actual mesh, e.g. change radii, thickness of ribs, shape of

hard corners, etc. Quite often the morphed FEM model can be exported instantaneously

(without any remeshing) allowing the CAE engineer to re-run the analysis of the modified

part on the fly.

86

An example of morphing a given finite element model is depicted below

(http://altair-2.wistia.com/medias/dp9q29f3jn)

A nice introduction to freehand morphing
(https://altairuniversity.com/learning-library/morph-volumes-front-of-car-1/)

87

4 Analysis Types

This chapter includes material from the book “Practical Finite Element Analysis (from finite to

Infinite)” as well as information from the HyperWorks Help Documentation. Additional material
was added by Matthias Goelke and Jan Grasmannsdorf.

The term CAE (Computer Aided Engineering) includes the following types of analyses:

1) Linear static analysis 6) Fatigue analysis

2) Nonlinear analysis 7) Optimization

3) Dynamic analysis 8) CFD analysis

4) Buckling analysis 9) Crash analysis

5) Thermal analysis 10) NVH analysis

1) Linear Static Analysis

Strain

Linear

Linear means straight line. In linear analysis, the FE solver will therefore always follow a

straight line from base to deformed state. As an example, in terms of linear material

behaviour, σ =ε E is the equation of a straight line (y = m x) passing through the origin.

“E”, the Elastic Modulus, is the slope of the line and is a constant. In real life after crossing

the yield point, the material follows a nonlinear curve but solvers follow the same straight

Software follows this path for linear

static calculation

Actual stress-strain curve

Stress

88

line. Components are broken into two separate pieces after crossing the ultimate stress

point, but software based linear analysis never shows failure in this fashion. It shows a

single unbroken part with a red color zone at the location of the failure. An analyst has to

conclude whether the component is safe or has failed by comparing the maximum stress

value with yield or ultimate stress.

Static

There are two conditions for static analysis:

1) The force is static i.e. there is no variation with respect to time (dead weight)

dF/dt = 0 F

t

2) Equilibrium condition ∑ forces (Fx , Fy , Fz) and ∑ Moments (Mx , My , Mz) = 0.

The FE model must fulfil this condition at each and every node. The complete model

summation of the external forces and moments is equal to the reaction forces and

moments.

The basic finite element equation to be solved for structures experiencing static loads can

be expressed as:

K u = P

where K is the stiffness matrix of the structure (an assemblage of individual element

stiffness matrices). The vector u is the displacement vector, and P is the vector of loads

89

(i.e. all the loading taking place in a component: external loads applied to the structure,

reaction forces…). The above equation is the equilibrium of external and internal forces.

The stiffness matrix is singular, unless displacement boundary conditions are applied to

fix the rigid body degrees of freedom of the model.

The equilibrium equation is solved either by a direct or an iterative solver (for nonlinear

analysis). By default, the direct solver is invoked, whereby the unknown displacements

are simultaneously solved using a Gauss elimination method that exploits the sparseness

and symmetry of the stiffness matrix, K, for computational efficiency.

Once the unknown displacements at the nodal points of the elements are calculated, the

stresses can be calculated by using the constitutive relations for the material. For linear

static analysis where the deformations are in the elastic range, i.e.: the stresses, σ, are

assumed to be linear functions of the strains, ε, Hooke’s law can be used to calculate the

stresses. Hooke’s law can be stated as:

σ=C ε

with the elasticity matrix C of the material. The strains are a function of the

displacements.

Please note that none of the terms in the equation is dependent on time or displacement.

This is why it is called, as we have learned before, a linear static analysis.

Practical Applications: A linear static analysis is the most commonly used analysis. All

aerospace, automobile, offshore and civil engineering industries perform linear static

analyses.

90

2) Nonlinear Analysis

*More details about Non-Linear Finite Element Analysis is provided in the free eBook

"Introduction to Non-Linear Analysis using OptiStruct”

Nonlinearity

Nonlinear Analysis Can Mean:

A nonlinear analysis is performed when we need to consider

A. Material based non- linearity: this is related to for instance, nonlinear elastic,

elastoplastic, viscoelastic, and/or viscoplastic behavior. The Force (stress) vs.

displacement (strain) curve is nonlinear (polynomial).

Within E (non-metal) Beyond E (metals)

Geometric

Material

Contact

Large

Deformation

Gap elements &

Contact simulation

Beyond Elastic Limit ‘E’

‘metals’

Within Elastic Limit ‘E’

‘Non metals’

Creep

(

Progressive) deformation of material at
constant stress.

- Long-time process

Strain

Strain

Stress

Stress

Nonlinear

Linear

91

The stress-strain diagram, along with the hardening* rule for the material, is required

as input data.

Metallic nonlinearity applications: Automobile, aerospace, ship industries. An analysis

is done to know the exact value of stress or strain when it crosses the yield point. For

low cycle fatigue analysis, this data is considered as input for the strain life approach.

Non-metallic nonlinearity applications: Automobile, aerospace industry, analysis of

rubber, plastic, asbestos, fiber components.

Creep - At elevated temperatures, even a small magnitude force, if kept applied over

a long time period (for months and years), would cause failure. Applications – nuclear

/ thermal power plants, civil engineering etc.

B. Geometric nonlinearity: In real life, the stiffness [K] is a function of displacement [d]

(remember: for linear analysis [K] is constant, independent of [d]). This means in a

geometric nonlinear analysis; the stiffness K is re-calculated after a certain predefined

displacement. As an example, think of a buckling case. The stiffness of a geometry

changes dramatically when or after buckling has occurred. The new “deformed”

geometry must now be taken into account, in order to get reasonable (realistic)

results.

In geometric linear analysis all deformations and rotations are small (infinitesimal).

Forces may follow the deformation or keep their direction. This can be controlled thru

the choice of coordinate systems (in geometric nonlinear analysis there are moving

and fixed coordinate systems).

92

The images depict two examples of these differences: A cantilever beam solved with

small displacements, large displacements with a follower force, and large

displacements without a follower force. The image below depicts a simple rigid rotated

by an angle solved with small and finite rotations.

C. Contact nonlinearity / boundary nonlinearity: In contact analysis, the stiffness K also

changes as a function of displacement (when parts get into contact or separate)

Note: Nonlinear analysis deals with true stress and strain (unlike engineering stress and

strain in linear static analysis)

93

Nonlinear Quasi Static (small deformation)

This solution sequence uses small deformation theory, similar to the way it is used with

Linear Static Analysis. Small deformation theory means that strains should be within

linear elasticity range (some 5 percent strain) and rotations within small rotation range

(some 5 degrees rotation). The Small Deformation Analysis is used mostly for contact

nonlinearities.

Nonlinear Quasi Static (large deformation)

Large displacement nonlinear static analysis is used for the solution of problems wherein

the load-response relationship is nonlinear and structural large displacements are

involved. The source of this nonlinearity can be attributed to multiple system properties,

for example, materials, geometry, nonlinear loading and constraint. Currently, in

OptiStruct the following large displacement nonlinear capabilities are available, including

large strain elasto-plasticity, hyperelasticity of polynomial form, contact with small

tangential motion, and rigid body constraints.

3) Dynamic Analysis

(*More information about this topic is included in the free eBook "Learn Dynamic

Analysis with Altair OptiStruct")

a) Linear Dynamics

Describes those systems in which forces increase linearly with parameters such as

position and velocity. Perhaps the best known linear system is a mass oscillating on a

spring, or the “simple harmonic oscillator.” In this situation, force on the mass increases

linearly with displacement by a factor of “k,” the spring constant. A graph of the potential

energy of this system is parabolic, since F(x) = - dU / dx.

94

A particle of mass m oscillating in the potential well of this system will have an angular

frequency of . The system becomes more complex when damping or a driving

force is added. Damping alone will cause the particle to sit down in the potential well or

“attractor.” When the system is forced, the system will oscillate at one frequency

determined by the relative strengths of the forcing and damping. If the forcing is too weak

or too strong, the system may oscillate at the forcing frequency. In this case, the free

movement of the system is essentially drowned by the forcing and damping and the

amplitude of oscillation is weak. At some frequency, however, the system will resonate

where maximum oscillating amplitude occurs. Again, in the linear system, this resonant

frequency is unique and is determined by the forcing, damping, and natural frequencies

of the system. In this driven and damped linear system, periodic inputs result in periodic

outputs. If there is error in a measurement, this error will increase linearly as the system

progresses.

b) Nonlinear Dynamics

Describes those nonlinear systems where one or more “forcing elements” does not vary

linearly with space parameters. For example, if the spring coefficient in the spring system

described before varied with displacement, then the spring force would vary with the

square of displacement.

Although linear systems make for pretty equations and an efficient summary of behavior,

nonlinear systems seem to pervade real natural systems. Friction forces, damping

elements, resistive elements in circuits -- these and many other factors often vary in a

nonlinear fashion. As a result, the differential equations describing these systems involve

very messy solutions that can only be solved numerically. Even if there were analytic

solutions to these systems the behavior in some cases would be difficult or impossible to

predict due to the exponential increase in error

95

Static Vs Dynamic System

To help us understand what a dynamic system is it is interesting to compare it with a

static system. There are two basic aspects that make the dynamic systems differ from

static systems:

• The loads are applied as a function of time. F(t)

• The responses are time dependent. X(t)

Example Dynamic System

Dynamic analysis for simple structures like the one described above can be carried out

manually. In general, it is possible to find an analytical response for it or by using

analytical tools it is possible to determine the mathematical functions that can represent

the system responses.

But for complex structures Finite Element Analysis (FEA) should be used to calculate the

dynamic responses. This kind of analysis is well known as Structural Dynamic Analysis

96

Types of Dynamic Analyses

Frequency Response Analysis

Frequency response analysis is used to calculate the response of a structure about steady

state oscillatory excitation. Typical applications are noise, vibration and harshness (NVH)

analysis of vehicles, rotating machinery, and transmissions.

Frequency response analysis is used to compute the response of the structure, which is

actually transient, in a static frequency domain. The loading is sinusoidal. A simple case

is a load of given amplitude at a specified frequency. The response occurs at the same

frequency, and damping would lead to a phase shift.

97

Excitation and response of a frequency response analysis.

The loads can be forces, displacements, velocity, and acceleration. They are dependent

on the excitation frequency W. The results from a frequency response analysis are

displacements, velocities, accelerations, forces, stresses, and strains. The responses are

usually complex numbers that are either given as magnitude and phase angle or as real

and imaginary part.

Transient Response Analysis

Transient response analysis is used to calculate the response of a structure to time-

dependent loads. Typical applications are structures subject to earthquakes, wind,

explosions, or a vehicle going through a pothole. The loads are time-dependent forces

and displacements. Initial conditions define the initial displacement and initial velocities

in grid points.

The results of a transient response analysis are displacements, velocities, accelerations,

forces, stresses, and strains. The responses are usually time-dependent.

98

The transient response analysis computes the structural responses solving the following

equation of motion with initial conditions in matrix form.

Mu’’ + Bu’ + Ku = P(t)

u(t=0) = u

0

u’(t=0) = v0

The matrix K is the global stiffness matrix, the matrix M the mass matrix, and the matrix

B is the damping matrix formed by the damping elements. The initial conditions are part

of the problem formulation and are applicable for the direct transient response only. The

equation of motion is integrated over time using the Newmark beta method. A time step

and an end time need to be defined.

Response Spectrum Analysis

Response Spectrum Analysis (RSA) is a technique used to estimate the maximum

response of a structure for a transient event. Maximum displacement, stresses, and/or

forces may be determined in this manner. The technique combines response spectra for

a prescribed dynamic loading with results of a normal modes analysis. The time-history

of the responses is not available.

Response spectra describe the maximum response versus natural frequency of a 1-DOF

system for a prescribed dynamic loading. They are employed to calculate the maximum

modal response for each structural mode. These modal maxima may then be combined

using various methods, such as the Absolute Sum (ABS) method or the Complete

Quadratic Combination (CQC) method, to obtain an estimate of the peak structural

response.

RSA is a simple and computationally inexpensive method to provide an approximation of

peak response, compared to conventional transient analysis. The major computational

effort is to obtain a sufficient number of normal modes in order to represent the entire

99

frequency range of input excitation and resulting response. Response spectra are usually

provided by design specifications; given these, peak responses under various dynamic

excitations can be quickly calculated. Therefore, it is widely used as a design tool in areas

such as seismic analysis of buildings.

While in a linear static analysis, the equation F = K * u is solved, a dynamic analysis is

based on some other equations:

[M] x ‘‘ + [C] x ‘ + [K] x = F(t)

x ‘‘ = d2x /dt2 = acceleration, x ‘ = dx /dt = velocity, x = displacement

[M] x ‘‘ = 0, [C] x ‘ = 0, [K] and F(t) = constant - Linear Static

[M] x ‘‘ = 0, [C] x˙ ‘ = 0, [K] is a function of {u}, F(t) = constant - Nonlinear Static

F(t) = 0, [C] x˙ ‘ = 0 and [M], [K] = constant - Free Vibration

All the terms in above equation are present - Forced Vibration

Practical applications: Natural frequency is a characteristic and basic design property of

any component, while forced vibrations is applicable for components subjected to force,

displacement, velocity, or acceleration varying with respect to time or frequency.

4) Linear Buckling Analysis

Some key aspects:

• Applicable for only compressive load

• Slender beams and sheet metal parts

100

• Bending stiffness <<< Axial stiffness • Large lateral deformation

The problem of linear buckling in finite element analysis is solved by first applying a

reference level of loading, P

Ref

, to the structure. A standard linear static analysis is then

carried out to obtain stresses which are needed to form the geometric stiffness matrix

KG. The buckling loads are then calculated by solving an eigenvalue problem:

[K-λKG] x = 0

Where K is the stiffness matrix of the structure and l is the multiplier to the reference

load. The solution of the eigenvalue problem generally yields n eigenvalues l, where n is

the number of degrees of freedom (in practice, only a subset of eigenvalues is usually

calculated). The vector x is the eigenvector corresponding to the eigenvalue.

The eigenvalue problem is solved using a matrix method called the Lanczos method. Not

all eigenvalues are required. Only a small number of the lowest eigenvalues are normally

calculated for buckling analysis.

The lowest eigenvalue l

crit

is associated with buckling. The critical or buckling load is:

Pcrit = lcrit PRef

Output from software: Critical value of load.