SOLIDWORKS 2015 Simulation User Manual

Engineering Analysis with SOLIDWORKS Simulation 2015

1

Engineering Analysis with SOLIDWORKS Simulation 2015

Table of contents

About the Author

Acknowledgements

Error! Bookmark not defined.

Error! Bookmark not defined.

Table of contents

Before You Start

Notes on hands-on exercises and functionality of Simulation

Prerequisites

Selected terminology

1

7

1: Introduction

What is Finite Element Analysis?

Finite Element Analysis used by Design Engineers

Objectives of FEA for Design Engineers

What is SOLIDWORKS Simulation?

Fundamental steps in an FEA project

Errors in FEA

A closer look at finite elements

What is calculated in FEA?

How to interpret FEA results

Units of measure

Using online help

Limitations of Static studiesl

2: Static analysis of a plate

Using the SOLIDWORKS Simulation interface

Linear static analysis with solid elements

Controlling discretization error with the convergence process

Finding reaction forces

Presenting FEA results in a desired format

11

37

2

Engineering Analysis with SOLIDWORKS Simulation 2015

3: Static analysis of an L-bracket

Error! Bookmark not defined.

Stress singularities

Differences between modeling errors and discretization errors

Using mesh controls

Analysis in different SOLIDWORKS configurations

Nodal stresses, element stresses

4: Static and frequency analyses of a pipe support

Error! Bookmark not defined.

Use of shell elements

Frequency analysis

Bearing load

Error! Bookmark not defined.

5: Static analysis of a link

Symmetry boundary conditions

Preventing rigid body motions

Limitations of the small displacements theory

6: Frequency analysis of a tuning fork and a plastic partError! Bookmark not defined.

Frequency analysis with and without supports

Rigid body modes

The role of supports in frequency analysis

Symmetric and anti-symmetric modes

7: Thermal analysis of a pipe connector and a heater Error! Bookmark not defined.

Analogies between structural and thermal analysis

Steady state thermal analysis

Analysis of temperature distribution and heat flux

Thermal boundary conditions

Thermal stresses

Vector plots

Error! Bookmark not defined.

8: Thermal analysis of a heat sink

Analysis of an assembly

Global and local Contact conditions

Steady state thermal analysis

Transient thermal analysis

Thermal resistance layer

Use of section views in result plots

3

Engineering Analysis with SOLIDWORKS Simulation 2015

9: Static analysis of a hanger

Global and local Contact conditions

Hierarchy of Contact conditions

10: Thermal stress analysis of a bi- metal loop

Thermal deformation and thermal stress analysis

Eliminating rigid body motions

Converting Sheet Metal bodies to Solid bobies

"Parasolid" round trip

Saving model in deformed shape

14: Selected nonlinear problems

Large displacement analysis

Analysis with shell elements

Membrane effects

Following and non-following load

Nonlinear material analysis

Residual stress

15: Mixed meshing problem

Using solid and shell elements in the same mesh

Mixed mesh compatibility

Manual and automatic finding of contact sets

Shell Manager

Error! Bookmark not defined.

Error! Bookmark not defined.

11: Buckling analysis of I-beam

Buckling analysis

Buckling load safety factor

Stress safety factor

Error! Bookmark not defined.

12: Static analysis of a bracket using adaptive solution methodsError! Bookmark not

defined.

h-adaptive solution method p-adaptive solution method

Comparison between h-elements and p-elements

13: Drop test

Drop test analysis

Stress wave propagation

Direct time integration solution

Error! Bookmark not defined.

Error! Bookmark not defined.

Error! Bookmark not defined.

4

Engineering Analysis with SOLIDWORKS Simulation 2015

16: Analysis of a weldment using beam elements

Error! Bookmark not defined.

Different levels of idealization implemented in finite elements

Preparation of a SOLIDWORKS model for analysis with beam elements

Beam elements and truss elements

Analysis of results using beam elements

Limitations of analysis with beam elements

17: Review of 2D problems

Classification of finite elements

2D axi-symmetric element

2D plane stress element

2D plane strain element

Error! Bookmark not defined.5

18: Vibration Analysis - Modal Time History and Harmonic Error! Bookmark not

defined.

Modal Time History analysis (Time Response)

Harmonic analysis (Frequency Response)

Modal Superposition Method

Damping

Error! Bookmark not defined.1

19: Analysis of random vibration

Random vibration

Power Spectral Density

RMS results

PSD results

Modal excitation

5

Engineering Analysis with SOLIDWORKS Simulation 2015

20: Miscellaneous topics

Mesh quality

Solvers and solvers options

Displaying mesh in result plots

Automatic reports

E drawings

Non uniform loads

Frequency analysis with pre-stress

Interference fit analysis

Rigid connector

Pin connector

Bolt connector

Remote load/mass

Weld connector

Bearing connector

Cyclic symmetry

Strongly nonlinear problem

Submodeling

Terminology issues in the Finite Element Analysis

Error! Bookmark not defined.1

21: Implementation of FEA into the design process Error! Bookmark not defined.5

Verification and Validation of FEA results

FEA driven design process

FEA project management

FEA project checkpoints

FEA reports

22: Glossary of terms

Error! Bookmark not defined.3

23: Resources available to FEA users

24: List of exercises

Error! Bookmark not defined.1

Error! Bookmark not defined.7

6

Engineering Analysis with SOLIDWORKS Simulation 2015

Before You Start

Notes on hands-on exercises and functionality of Simulation

This book goes beyond a standard software manual because its unique approach concurrently introduces you to SOLIDWORKS Simulation software and the fundamentals of Finite Element Analysis (FEA) through hands-on exercises. We recommend that you study the exercises in the order presented in the book. As you go through the exercises, you will notice that explanations and steps described in detail in earlier exercises are not repeated in later chapters. Each subsequent exercise assumes familiarity with software functions discussed in previous exercises and builds on the skills, experience, and understanding gained from previously presented problems.

Exceptions to the above are chapters 21, 22, 23, 24 which do not include hands-on exercises.

Exercises in this book require different levels of SOLIDWORKS Simulation functionality and this depends on which Simulation product is used. The

SOLIDWORKS Simulation Product Matrix document is available at: http://www.SOLIDWORKS.com/sw/products/simulation/simulation-matrices.htm

This book deals with structural analysis using SOLIDWORKS Simulation.

Therefore, Motion analysis won’t be covered. SimulationXpress is a simplified version of SOLIDWORKS Simulation and will not be covered either.

All exercises in this book use SOLIDWORKS models, which can be downloaded from www.SDCpublications.com. These exercises do not contain any Simulation studies; you are expected to create all studies, results plots, and graphs yourself. The only exceptions are exercises in chapter 4 (MISALIGNMENT), 20 and 21 which come with Simulation studies fully or partially defined. All problems presented here have been solved with SOLIDWORKS Simulation Premium running on Windows

7 in a 64 bit operating environment.

We encourage you to explore each exercise beyond its description by investigating other options, other menu choices, and other ways to present results. You will soon discover that the same simple logic applies to all functions in SOLIDWORKS

Simulation.

7

Engineering Analysis with SOLIDWORKS Simulation 2015

“Engineering Analysis with SOLIDWORKS Simulation” is an introductory text. The focus is more on understanding Finite Element Analysis than presenting all software capabilities. This book is not intended to replace software manuals. Therefore, not all

Simulation capabilities will be covered, especially those of fatigue, design studies, optimization, advanced nonlinear thermal and dynamic analyses.

Readers of "Engineering Analysis with SOLIDWORKS Simulation" may wish to review the book “Thermal Analysis with SOLIDWORKS Simulation” (Figure 23-1) and “Vibration Analysis with SOLIDWORKS” (Figure 23-2), both published by the

SDC Publications. These books are not introductory texts; they are designed for users who are familiar with topics presented in “Engineering Analysis with SOLIDWORKS

Simulation”.

The knowledge acquired by the readers of "Engineering Analysis with

SOLIDWORKS Simulation" will not be software specific. The same concepts, tools and methods will apply to any FEA software.

Prerequisites

The following prerequisites are recommended:













An understanding of Statics, Kinematics and Dynamics

An understanding of Mechanics of Materials

An understanding of Heat Transfer

An understanding of Mechanical Vibrations

Experience with parametric, feature based solid modeling using SOLIDWORKS

Familiarity with the Windows Operating System

8

Engineering Analysis with SOLIDWORKS Simulation 2015

Selected terminology

The mouse pointer plays a very important role in executing various commands and providing user feedback. The mouse pointer is used to execute commands, select geometry, and invoke pop-up menus. We use Windows terminology when referring to mouse-pointer actions.

Item

Click

Double-click

Click-inside

Drag and drop

Right-click

Description

Self-explanatory

Self-explanatory

Click the left mouse button. Wait a second, and then click the left mouse button inside the pop-up menu or text box. Use this technique to modify the names of items in SOLIDWORKS Simulation

Manager.

Use the mouse to point to an object. Press and hold the left mouse button down. Move the mouse pointer to a new location. Release the left mouse button.

Click the right mouse button. A pop-up menu is displayed. Use the left mouse button to select a desired menu command.

All SOLIDWORKS file names appear in CAPITAL letters, even though the actual file names may use a combination of capital and small letters. Selected menu items and SOLIDWORKS Simulation commands appear in bold. SOLIDWORKS configurations, SOLIDWORKS Simulation folders, icon names and study names appear in italics except in captions and comments to illustrations. SOLIDWORKS and Simulation also appear in bold font. Bold font may also be used to draw reader's attention to particular term.

9

Engineering Analysis with SOLIDWORKS Simulation 2015

10

Engineering Analysis with SOLIDWORKS Simulation 2015

1: Introduction

What is Finite Element Analysis?

Finite Element Analysis, commonly called FEA, is a method of numerical analysis.

FEA is used for solving problems in many engineering disciplines such as machine design, acoustics, electromagnetism, soil mechanics, fluid dynamics, and many others.

In mathematical terms, FEA is a numerical technique used for solving field problems described by a set of partial differential equations.

In mechanical engineering, FEA is widely used for solving structural, vibration, and thermal problems. However, FEA is not the only available tool of numerical analysis.

Other numerical methods include the Finite Difference Method, the Boundary

Element Method, and the Finite Volume Method to mention just a few. However, due to its versatility and numerical efficiency, FEA has come to dominate the engineering analysis software market, while other methods have been relegated to niche applications. When implemented into modern commercial software, both FEA theory and numerical problem formulation become completely transparent to users.

Finite Element Analysis used by Design Engineers

FEA is a powerful engineering analysis tool useful in solving many problems ranging from very simple to very complex. Design engineers use FEA during the product development process to analyze the design-in-progress. Time constraints and limited availability of product data call for many simplifications of computer models. On the other hand, specialized analysts implement FEA to solve very complex problems, such as vehicle crash dynamics, hydro forming, and air bag deployment.

This book focuses on how design engineers use FEA, implemented in

SOLIDWORKS Simulation, as a design tool. Therefore, we highlight the most essential characteristics of FEA as performed by design engineers as opposed to those typical for FEA performed by analysts.

FEA for Design Engineers: Another design tool

For design engineers, FEA is one of many design tools that are used in the design process and include CAD, prototypes, spreadsheets, catalogs, hand calculations, text books, etc.

11

Engineering Analysis with SOLIDWORKS Simulation 2015

FEA for Design Engineers: Based on CAD models

Modern design is conducted using CAD, so a CAD model is the starting point for analysis. Since CAD models are used for describing geometric information for FEA, it is essential to understand how to prepare CAD geometry in order to produce correct FEA results, and how a CAD model is different from an FEA model. This will be discussed in later chapters.

FEA for Design Engineers: Concurrent with the design process

Since FEA is a design tool, it should be used concurrently with the design process. It should drive the design process rather than follow it.

Limitations of FEA for Design Engineers

An obvious question arises: would it be better to have a dedicated specialist perform

FEA and let design engineers do what they do best – design new products? The answer depends on the size of the business, type of products, company organization and culture, and many other tangible and intangible factors. A general consensus is that design engineers should handle relatively simple types of analysis, but do it quickly and of course reliably. Analyses that are very complex and time consuming cannot be executed concurrently with the design process, and are usually better handled either by a dedicated analyst or contracted out to specialized consultants.

12

Engineering Analysis with SOLIDWORKS Simulation 2015

Objectives of FEA for Design Engineers

The ultimate objective of using FEA as a design tool is to change the design process from repetitive cycles of “design, prototype, test” into a streamlined process where prototypes are not used as design tools and are only needed for final design validation. With the use of FEA, design iterations are moved from the physical space of prototyping and testing into the virtual space of computer simulations (Figure 1-1).

Traditional Product

Design Process

Design

Simulation Driven Product

Design Process

CAD

Simulation

Prototyping Prototyping

Testing Testing

Production

Production

Figure 1-1: Traditional and Simulation* driven product development.

Traditional product development needs prototypes to support a design in progress.

The process in Simulation-driven product development uses numerical models, rather than physical prototypes to drive development. In an Simulation driven product design process, the prototype is no longer a part of the iterative design loop.

*Simulation means here Finite Element Analysis.

13

Engineering Analysis with SOLIDWORKS Simulation 2015

What is SOLIDWORKS Simulation?

SOLIDWORKS Simulation is a commercial implementation of FEA capable of solving problems commonly found in design engineering, such as the analysis of displacements, stresses, natural frequencies, vibration, buckling, heat flow, etc. It belongs to the family of engineering analysis software products originally developed by the Structural Research & Analysis Corporation (SRAC). SRAC was established in

1982 and since its inception has contributed to innovations that have had a significant impact on the evolution of FEA. In 1995 SRAC partnered with the SOLIDWORKS

Corporation and created COSMOSWorks, one of the first SOLIDWORKS Gold

Products, which became the top-selling analysis solution for the SOLIDWORKS

Corporation. The commercial success of COSMOSWorks integrated with

SOLIDWORKS CAD software resulted in the acquisition of SRAC in 2001 by

Dassault Systèmes, parent of SOLIDWORKS Corporation. In 2003, SRAC operations merged with the SOLIDWORKS Corporation. In 2009, COSMOSWorks was re-named SOLIDWORKS Simulation.

SOLIDWORKS Simulation is integrated with SOLIDWORKS CAD software and uses SOLIDWORKS for creating and editing model geometry. SOLIDWORKS is a solid, parametric, feature-driven CAD system developed specifically for the Windows

Operating System. Many other CAD and FEA programs were originally developed in a UNIX environment and only later ported to Windows, and therefore are less integrated with Windows than SOLIDWORKS and SOLIDWORKS Simulation.

Fundamental steps in an FEA project

The starting point for any SOLIDWORKS Simulation project is a SOLIDWORKS model, which can be a part or an assembly. First, material properties, loads, and restraints are defined. Next, as is always the case with using any FEA-based analysis tool, the model geometry is split into relatively small and simply shaped entities called finite elements. The elements are called “finite” to emphasize the fact that they are not infinitesimally small, but relatively small in comparison to the overall model size.

Creating finite elements is commonly called meshing. When working with finite elements, the SOLIDWORKS Simulation solver approximates the sought solution

(for example stress) by assembling the solutions for individual elements.

14

Engineering Analysis with SOLIDWORKS Simulation 2015





From the perspective of FEA software, each application of FEA requires three steps:

 Preprocessing of the FEA model, which involves defining the model and then splitting it into finite elements

Solving for desired results

Post-processing for results analysis









We will follow the above three steps in every exercise. From the perspective of FEA methodology, we can list the following FEA steps:

Building the mathematical model

Building the finite element model by discretizing the mathematical model

Solving the finite element model

Analyzing the results

The following subsections discuss these four steps.

Building the mathematical model

The starting point to analysis with SOLIDWORKS Simulation is a SOLIDWORKS model. Geometry of the model needs to be meshable into a correct finite element mesh. This requirement of mesh-ability has very important implications. We need to ensure that the CAD geometry will indeed mesh and that the produced mesh will provide the data of interest (e.g. stresses, displacements or temperature distribution) with acceptable accuracy.

The necessity to mesh often requires modifications to the CAD geometry, which can take the form of defeaturing, idealization, and/or clean-up:

Term Description

Defeaturing

The process of removing geometry features deemed insignificant for analysis, such as outside fillets, chamfers, logos, etc.

Idealization

A more aggressive exercise that may depart from solid

CAD geometry by, for example, representing thin walls with surfaces and beams with lines.

Clean-up

Sometimes needed because geometry must satisfy high quality requirements to be meshable. To cleanup, we can use CAD quality control tools to check for problems like, for example, sliver faces, multiple entities, etc. that could be tolerated in the CAD model, but would make subsequent meshing difficult or impossible.

15

Engineering Analysis with SOLIDWORKS Simulation 2015

It is important to mention that we do not always simplify the CAD model with the sole objective of making it meshable. Often we must simplify a model even though it would mesh correctly “as is”, because the resulting mesh would be large (in terms of the number of elements) and consequently, the meshing and the analysis would take too long. Geometry modifications allow for a simpler mesh and shorter meshing and computing times.

Sometimes, geometry preparation may not be required at all. Successful meshing depends as much on the quality of geometry submitted for meshing as it does on the capabilities of the meshing tools implemented in the FEA software.

Having prepared a meshable, but not yet meshed geometry, we now define material properties (these can also be imported from a CAD model), loads and restraints, and provide information on the type of analysis that we wish to perform. This procedure completes the creation of the mathematical model (Figure 1-2). Notice that the process of creating the mathematical model is not FEA specific. FEA has not yet entered the picture.

Modification of geometry (if required)

Loads Restraints

MATHEMATICAL

MODEL

Material properties

Type of analysis

CAD geometry FEA geometry

Figure 1-2: Building the mathematical model.

The process of creating a mathematical model consists of the modification of CAD geometry (here removing outside fillets), definition of loads, restraints, material properties, and definition of the type of analysis (for example linear static) that is to be performed.

You may review the differences between CAD geometry and FEA geometry using part model BRACKET DEMO in its two configurations: 01 fully featured and 02

defeatured.

16

MATHEMATICAL

MODEL

Engineering Analysis with SOLIDWORKS Simulation 2015

Building the finite element model

The mathematical model now needs to be split into finite elements using the process of discretization, more commonly known as meshing (Figure 1-3). Geometry, loads, and restraints are all discretized. The discretized loads and restraints are applied to the nodes of the finite element mesh which is a discretized representation of geometry.

Solving the finite element model

Having created the finite element model, we now utilize a solver provided in SOLIDWORKS Simulation to produce the desired data of interest (Figure 1-3).

Analyzing the results

Often the most difficult step of FEA is analyzing the results. Proper interpretation of results requires that we understand all simplifications

(and errors they introduce) in the first three steps: defining the mathematical model, meshing, and solving.

Discretization

Numerical solver

FEA model FEA results

Figure 1-3: Building the finite element model.

The mathematical model is discretized into a finite element model. This completes the pre-processing phase. The FEA model is then solved with one of the numerical solvers available in SOLIDWORKS Simulation.

17

Engineering Analysis with SOLIDWORKS Simulation 2015

Errors in FEA

The process illustrated in Figure 1-2 and Figure 1-3 introduces unavoidable errors.

Formulation of a mathematical model introduces modeling errors (also called idealization errors), discretization of the mathematical model introduces discretization errors, and solving introduces solution errors. Of these three types of errors, only discretization errors are specific to FEA. Modeling errors affecting the mathematical model are introduced before FEA is utilized and can only be controlled by using correct modeling techniques. Solution errors are caused by the accumulation of roundoff errors.

A closer look at finite elements

Meshing splits continuous mathematical models into finite elements. The type of elements created by this process depends on the type of geometry meshed.

SOLIDWORKS Simulation offers three types of three dimensional (3D) elements: solid elements for meshing solid geometry, shell elements for meshing surface geometry and beam elements for meshing wire frame geometry. SOLIDWORKS

Simulation also works with two dimensional (2D) elements: plane stress elements, plane strain elements, and axi-symmetric elements.

Before proceeding, we need to clarify an important terminology issue. In

CAD terminology, “solid” denotes the type of geometry: solid geometry

(as opposed to surface or wire frame geometry). In FEA terminology, “solid” denotes the type of element used to mesh the solid CAD geometry.

Solid elements

The type of geometry that is most often used for analysis with SOLIDWORKS

Simulation is solid CAD geometry. Meshing of this geometry is accomplished with tetrahedral solid elements, commonly called “tets” in FEA jargon. The tetrahedral solid elements in SOLIDWORKS Simulation can either be first order elements

(“draft quality”), or second order elements (“high quality”). The user decides whether to use draft quality or high quality elements for meshing. However, as we will soon prove, only high quality elements should be used for an analysis of any importance.

The difference between first and second order tetrahedral elements is illustrated in

Figure 1-4.

18

Engineering Analysis with SOLIDWORKS Simulation 2015

First order tetrahedral element before deformation

First order tetrahedral element after deformation

Second order tetrahedral element before deformation

Second order tetrahedral element after deformation

Figure 1-4: Differences between first and second order tetrahedral elements.

First and second order tetrahedral elements are shown before and after deformation.

Notice that the first order element has corner nodes only, while the second order element has both corner and mid-side nodes (one mid-side node is not visible for the second order element in this illustration). Single elements seldom experience deformations of this magnitude, which are exaggerated in this illustration.

19

Engineering Analysis with SOLIDWORKS Simulation 2015

In a first order element, edges are straight and faces are flat. After deformation the edges and faces must retain these properties.

The edges of a second order element before deformation may either be straight or curvilinear, depending on how the element has been mapped to model the actual geometry. Consequently, the faces of a second order element before deformation may be flat or curved.

After deformation, edges of a second order element may either assume a different curvilinear shape or acquire a curvilinear shape if they were initially straight.

Consequently, faces of a second order element after deformation can be either flat or curved.

First order tetrahedral elements model the linear field of displacement inside their volume, on faces, and along edges. The linear (or first order) displacement field gives these elements their name: first order elements.

If you recall from Mechanics of Materials, strain is the first derivative of displacement. Since the displacement field is linear, the strain field is constant.

Consequently the stress field is also constant in first order tetrahedral elements. This situation imposes a very severe limitation on the capability of a mesh constructed with first order elements to model the stress distribution of any complex model. To make matters worse, straight edges and flat faces cannot map properly to curvilinear geometry, as illustrated in Figure 1-5, left.

20

Engineering Analysis with SOLIDWORKS Simulation 2015

Second order tetrahedral elements have ten nodes (Figure 1-4) and model the second order (parabolic) displacement field and first order (linear) stress field in their volume, on faces and along edges. The edges and faces of second order tetrahedral elements can be curvilinear before and after deformation, therefore these elements can be mapped precisely to curved surfaces, as illustrated in Figure 1-5 right. Even though these elements are more computationally demanding than first order elements, second order tetrahedral elements are used for the majority of analyses with SOLIDWORKS

Simulation because of their better mapping and stress modeling capabilities.

A tetrahedral solid element is the only type of solid elements available in

SOLIDWORKS Simulation.

Mapping a hole with first order solid tetrahedral elements.

Mapping a hole with second order solid tetrahedral elements.

Figure 1-5: Failure of straight edges and flat faces to map to curvilinear geometry when using first order elements (left), and precise mapping to curvilinear geometry using second order elements (right).

Notice the imprecise first order element mapping of the hole; flat faces approximate the face of the curvilinear geometry. Second order elements map well to curvilinear geometry.

21

Engineering Analysis with SOLIDWORKS Simulation 2015

Shell elements

Shell elements are created by meshing surfaces or faces of solid geometry. Shell elements are primarily used for analyzing thin-walled structures. Since surface geometry does not carry information about thickness, the user must provide this information. Similar to solid elements, shell elements also come in draft and high quality with analogous consequences with respect to their ability to map to curvilinear geometry, as shown in Figure 1-6.

Mapping a cylinder with first order triangular shell elements

Mapping a cylinder with second order triangular shell elements

Figure 1-6: Mapping with first order shell elements (left) and second order shell elements (right).

The shell element mesh on the left was created with first order elements. Notice the imprecise mapping of the mesh to curvilinear geometry. The shell element mesh on the right was created with second order elements, which map correctly to curvilinear geometry.

We need to make two important comments about Figure 1-5 and Figure 1-6. First, a mesh should never be that coarse (large size of elements compared to the model). We use a coarse mesh only to show the differences between first and second order elements clearly. Second, notice the “kinks” on the side of the second order elements; they indicate locations of mid side nodes. The second order element does map precisely to second order geometry.

As in the case of solid elements, first order shell elements model linear displacements and constant strain and stress. Second order shell elements model second order

(parabolic) displacement and linear strain and stress.

22

Engineering Analysis with SOLIDWORKS Simulation 2015

The assumptions of modeling first or second order displacements in shell elements apply only to in-plane directions. The distribution of in-plane stresses across the thickness is assumed to be linear in both first and second order shell elements.

Triangular elements are the only type of shell elements available in SOLIDWORKS

Simulation.

Certain classes of shapes can be modeled using either solid or shell elements, such as the plate shown in Figure 1-7. Often the nature of the geometry dictates what type of element should be used for meshing. For example, a part produced by casting would be meshed with solid elements, while a sheet metal structure would be best meshed with shell elements.

Second order tetrahedral solid elements Second order triangular shell elements

Figure 1-7: Plate modeled with solid elements (left) and shell elements (right).

The actual choice between solids and shells depends on the particular requirements of analysis and sometimes on personal preferences.

23

Engineering Analysis with SOLIDWORKS Simulation 2015

Beam elements

Beam elements are created by meshing curves (wire frame geometry). They are a natural choice for meshing weldments. Assumptions about the stress distribution in two directions of the beam cross section are made.

A beam element does not have any physical dimensions in the directions normal to its length. It is possible to think of a beam element as a line with assigned beam cross section properties (Figure 1-8).

Figure 1-8: Conceptual representation of a beam element.

A beam element is a line with assigned properties of a beam cross section as required by beam theory. This illustration conceptualizes how a curve (here a straight line) defines an I-beam but does not represent actual geometry of beam cross-section.

Before we proceed with the classification of finite elements we need to introduce the concept of nodal degrees of freedom which are of paramount importance in FEA. The degrees of freedom (DOF) of a node in a finite element mesh define the ability of the node to perform translation and rotation. The number of degrees of freedom that a node possesses depends on the element type. In SOLIDWORKS Simulation, nodes of solid elements have three degrees of freedom, while nodes of shell elements have six degrees of freedom.

This is because in order to describe the transformation of a solid element from the original to the deformed shape, we only need to know three translational components of nodal displacement. In the case of shell and beam elements, we need to know the translational components of nodal displacements and the rotational displacement components.

Using solid elements we study how a 3D structure deforms under a load. Using shell elements we study how a 3D structure with one dimension “collapsed” deforms under a load. This collapsed dimension is thickness which is not represented explicitly in the

24

Engineering Analysis with SOLIDWORKS Simulation 2015 model geometry. Beam elements are intended to study 3D structures with two dimensions removed from the geometry and not represented explicitly by model geometry. It is important to point out that solids, shells and beams are all 3D elements capable of deformation in 3D space.

2D elements

There are also cases where a structure’s response to load can be fully described by 2D elements that have only two in-plane degrees of freedom. These are plane stress, plane strain and axi-symmetric elements.

Plane stress elements are intended for the analysis of thin planar structures loaded inplane, where out-of-plane stress is assumed to be equal zero. Plane strain elements are intended for the analysis of thick prismatic structures loaded in-plane, where out-ofplane strain is assumed to be equal zero. Axi-symmetric elements are intended for the analysis of axi-symmetric structures under axi-symmetric load. In all of these special cases, the structure deformation can be fully described using elements with only two degrees of freedom per node. For plane stress and plane strain, these are two components of in-plane translation. For axi-symmetric elements these are radial and axial displacements.

2D elements are summarized in Figure 1-9.

25

Engineering Analysis with SOLIDWORKS Simulation 2015

Thin 3D model Representative slice ready for meshing with 2D plane stress elements

Thick 3D model Representative slice ready for meshing with 2D plane strain elements

Axi-symmetric 3D model Representative slice ready for meshing with 2D axi-symmetric elements

Figure 1-9: Application of 2D elements: plane stress (top), plane strain (middle), and axi-symmetric (bottom).

Just like solids and shells, 2D elements may be of first or second order.

26

Engineering Analysis with SOLIDWORKS Simulation 2015

Figure 1-10 presents the basic library of elements in SOLIDWORKS Simulation.

Solid elements are tetrahedral, shell elements and 2D elements are triangles and beam elements are lines. Elements such as hexahedral solids or quadrilateral shells are not available in SOLIDWORKS Simulation.

3D elements 2D elements

Solid elements Shell elements Beam elements Plate elements

First order element

Linear (first order) displacement field

Constant stress field

Second order element

Parabolic (second order) displacement field

Linear stress field

Figure 1-10: Basic element library of SOLIDWORKS Simulation.

The majority of analyses use the second order tetrahedral element. Element order is not applicable to a beam element. 2D elements are sometimes referred to as plate elements.

Beam element cross-section is defined by cross section and second moments of inertia of the analyzed structural member. It does not have any physical shape. The above I beam is shown only for the ease of visualization.

27

Engineering Analysis with SOLIDWORKS Simulation 2015

What is calculated in FEA?

Each degree of freedom of a node in a finite element mesh constitutes an unknown. In structural analysis, nodal degrees of freedom represent displacement components, while in thermal analysis they represent temperatures. Nodal displacements and nodal temperatures are the primary unknowns for structural analysis and thermal analysis, respectively.

Structural analysis finds displacements, strains and stresses. If solid elements are used, then three displacement components (three translations) per node must be calculated.

With shell and beam elements, six displacement components (six translations) must be calculated. 2D elements require calculations of two displacement components. Strains and stresses, are calculated based on the nodal displacement results.

Thermal analysis finds temperatures, temperature gradients, and heat flow. Since temperature is a scalar value (unlike displacements, which are vectors), then regardless of what type of element is used, there is only one unknown (temperature) to be found for each node. All other thermal results such as temperature gradient and heat flux are calculated based on temperature results. The fact that there is only one unknown to be found for each node, rather than three or six, makes thermal analysis less computationally intensive than structural analysis.

How to interpret FEA results

Results of structural FEA are provided in the form of displacements and stresses. But how do we decide if a design “passes” or “fails”? What constitutes a failure?

To answer these questions, we need to establish some criteria to interpret FEA results, which may include maximum acceptable displacements, maximum stress, or the lowest acceptable natural frequency.

While displacement and frequency criteria are quite obvious and easy to establish, stress criteria are not. Let us assume that we need to conduct a stress analysis in order to ensure that stresses are within an acceptable range. To judge stress results, we need to understand the mechanism of potential failure. If a part breaks, what stress measure best describes that failure? SOLIDWORKS Simulation can present stress results in any desired form, but it is up to us to decide which stress measures should be used to analyze results.

Discussion of various failure criteria is out of the scope of this book. Any textbook on the Mechanics of Materials provides information on this topic. Here we will limit our discussion to commonly used failure criteria: Von Mises Stress failure criterion and

Maximum Normal Stress failure criterion.

28

Engineering Analysis with SOLIDWORKS Simulation 2015

Von Mises Stress failure criterion

Von Mises stress, also known as Huber stress, is a stress measure that accounts for all six stress components of a general 3-D state of stress

(Figure 1-11).

Figure 1-11: General state of stress represented by three normal stresses: σ x

,

σ y

, σ z and six shear stresses.

Two components of shear stress and one component of normal stress act on each side of this elementary cube. Due to symmetry of shear stresses, the general 3D state of stress is characterized by six stress components: σ x

, σ y

, σ z and τ xy

= τ yx

, τ yz

= τ zy

, τ xz

= τ zx

29

Engineering Analysis with SOLIDWORKS Simulation 2015

Von Mises stress

σ

vm

, can be expressed either by six stress components as:

= 0.5 × − + − + ( − ) + 3 × + +

Von Mises stress σ vm

, can be also expressed three principal stresses (Figure 1-12) as:

= 0.5 × [( − ) + ( − ) + ( − ) ]

Notice that von Mises stress is a non-negative, scalar stress measure. Von Mises stress is commonly used to present results because the structural safety for many engineering materials showing elasto-plastic properties (for example, steel or aluminum alloy) can be evaluated using von Mises stress.

The maximum von Mises stress failure criterion is based on the von Mises-Hencky theory, also known as the shear-energy theory or the maximum distortion energy theory. The theory states that a ductile material starts to yield at a location when the von Mises stress becomes equal to the stress limit. In most cases, the yield strength is used as the stress limit. According to the von Mises failure criterion, the factor of safety (FOS) is expressed as:

= / where σ

limit

is yield strength.

30

Engineering Analysis with SOLIDWORKS Simulation 2015

Maximum Normal Stress failure criterion

By properly adjusting the angular orientation of the stress cube in Figure 1-11, shear stresses disappear and the state of stress is represented only by three principal stresses:

σ

1

, σ

2

, σ

3

, as shown in Figure 1-12. In SOLIDWORKS Simulation, principal stresses are denoted as P1, P2, P3.

Figure 1-12: The general state of stress represented by three principal stresses: σ

1

, σ

σ

3

.

2

,

The Maximum Normal Stress Failure criterion is used for brittle materials. Brittle materials do not have a specific yield point. This criterion assumes that the ultimate tensile strength of the material in tension and compression is the same. This assumption is not valid in all cases. For example, cracks considerably decrease the strength of the material in tension while their effect is not significant in compression because the cracks tend to close.

This criterion predicts failure will occur when σ

1 exceeds the stress limit, usually the ultimate tensile strength. According to the maximum principle stress failure criterion, the factor of safety FOS is expressed as:

= / where

σ

limit

is ultimate tensile strength.

31

Engineering Analysis with SOLIDWORKS Simulation 2015

Units of measure

Internally, SOLIDWORKS Simulation uses the International System of Units (SI).

However, for the user’s convenience, the unit manager allows data entry in any of three systems of units: SI, Metric, and English. Results can be displayed using any of the three systems. Figure 1-13 summarizes the available systems of units.

Mass

Length

Time

Force

Gravitational acceleration

Mass density

Temperature

International

System (SI)

kg

Metric (MKS)

kg m cm s

N m/s

2 kg/m

3

K s

Kgf

G kg/cm

3

°C

English (IPS)

lb in s lbf in/s

2 lbf/in

3

°F

Figure 1-13: Unit systems available in SOLIDWORKS Simulation.

SI, Metric, and English systems of units can be interchanged when entering data and analyzing results in SOLIDWORKS Simulation.

As SOLIDWORKS Simulation users, we are spared much confusion and trouble with systems of units. However, we may be asked to prepare data or interpret the results of other FEA software where we do not have the convenience of the unit manager. Therefore, we will make some general comments about the use of different systems of units in the preparation of input data for FEA models. We can use any consistent system of units for FEA models, but in practice, the choice of the system of units is dictated by what units are used in the CAD model. The system of units in

CAD models is not always consistent; length can be expressed in [mm], while mass density can be expressed in [kg/m

3

]. Contrary to CAD models, in FEA all units must be consistent. Inconsistencies are easy to overlook, especially when defining mass and mass density and can lead to serious errors.

32

Engineering Analysis with SOLIDWORKS Simulation 2015

In the SI system, based on meters [m] for length, kilograms [kg] for mass, and seconds [s] for time, all other units are easily derived from these base units. In mechanical engineering, length is commonly expressed in millimeters [mm], force in Newtons [N], and time in seconds [s]. All other units must then be derived from these basic units: [mm], [N], and [s].

Consequently, the unit of mass is defined as a mass which, when subjected to a unit force equal to 1N, will accelerate with a unit acceleration of 1 mm/s

2

.

Therefore, the unit of mass in a system using [mm] for length and [N] for force, is equivalent to 1000 kg or one metric ton. Therefore, mass density is expressed in metric tonnes [tonne/mm

3

]. This is critically important to remember when defining material properties in FEA software without a unit manager. Review Figure 1-14 and notice that an erroneous definition of mass density in [kg/m

3

] rather than in

[tonne/mm

3

] results in mass density being one trillion (10

12

) times higher.

System SI

Unit of mass

Unit of mass density

Density of aluminum

System of units derived from

SI

Unit of mass

Unit of mass density

Density of aluminum

English system (IPS)

Unit of mass

Unit of mass density

Density of aluminum

[m] [N] [s]

kg kg/m

3

2794 kg/m

3

[mm] [N] [s]

tonne tonne/mm

3

2.794 x 10

-9 tonne/mm

3

[in] [lbf] [s]

slug/12 slug/12/in

3

2.614 x 10

-4 slug/12/in

3

Figure 1-14: Mass density of aluminum in the three systems of units.

Comparison of numerical values of mass densities of 1060 aluminum alloy defined in the SI system of units with the system of units derived from SI, and with the English (IPS) system of units.

33

Engineering Analysis with SOLIDWORKS Simulation 2015

Using online help

SOLIDWORKS Simulation features very extensive online Help and Tutorial functions, which can be accessed from the Help menu in the main SOLIDWORKS tool bar or from the Simulation menu. The Study advisor can be accessed from the

Study drop down menu (Figure 1-15).

(1)

(2)

(3)

Figure 1-15: Accessing online Help, and Study Advisor.

Online Help, Tutorials, and Validation can be accessed from the main SOLIDWORKS toolbar (1) or from the Simulation menu (2). The Study Advisor can be accessed from the Study drop down menu (3).

34

Engineering Analysis with SOLIDWORKS Simulation 2015

Limitations of Static studies

Static study is the only type of study available in some SOLIDWORKS packages.

Working with Static study we need to accept important limitations: material is assumed as linear, and loads are static.

Linear material

Whatever material we assign to the analyzed parts or assemblies, the material is assumed to be linear, meaning that stress is proportional to the strain (Figure 1-16).

Stress

σ

Linear

Material

Nonlinear

Material

α

α

E =





 tan



Strain

ε

Linear range

Figure 1-16: The linear material model assumed in SOLIDWORKS Simulation.

With a linear material, stress is linearly proportional to strain. The linear range is where the linear and nonlinear material models are not significantly different.

Using a linear material model, the maximum stress magnitude is not limited to yield or to ultimate stress as it is in reality. Material yielding is not modeled, and whether or not yield may in fact be taking place can only be established based on the stress magnitudes reported in results. Most analyzed structures experience stresses below the yield stress, and the factor of safety is most often related to the yield stress.

Therefore, the limitations imposed by linear material seldom impede SOLIDWORKS

Simulation Professional users.

35

Engineering Analysis with SOLIDWORKS Simulation 2015

Static loads

All structural loads and restraints are assumed not to change with time. Dynamic loading conditions cannot be analyzed with Static study. This limitation implies that loads are applied slowly enough to ignore inertial effects.

Nonlinear material analysis and dynamic analysis can be performed with

SOLIDWORKS Simulation Premium.

36

Engineering Analysis with SOLIDWORKS Simulation 2015

2: Static analysis of a plate

Topics covered











Using the SOLIDWORKS Simulation interface

Linear static analysis with solid elements

Controlling discretization error with the convergence process

Finding reaction forces

Presenting FEA results in a desired format

Project description

A steel plate is supported and loaded, as shown in Figure 2-1. We assume that the support is rigid (this is also called built-in support, fixed support or fixed restraint) and that a 100000N tensile load is uniformly distributed along the end face, opposite to the supported face.

Fixed restraint

100000N tensile load uniformly distributed

Figure 2-1: SOLIDWORKS model of a rectangular plate with a hole.

We will perform a displacement and stress analysis using meshes with different element sizes. Notice that repetitive analysis with different meshes does not represent standard practice in FEA. However, repetitive analysis with different meshes produces results which are useful in gaining more insight into how FEA works.

37