Finite Element Analysis Guide Through ANSYS Wb v.16.2

Finite Element Analysis Method using

ANSYS Workbench v16.2

Step-by-Step Guide…

Credits and Copyright

Written by:          Bc. Syllignakis Stefanos

sylst3f@gmail.com

Main Editor: Ing. Petr Vosynek, Ph.D

petr.vosynek@gmail.com

Review and Editor: Ing. Marek Benešovský

*******@vutbr.cz

Preface

The presented material was created within the Erasmus+ project of the student Stefanos Syllignakis under the leadership of Petr Vosynek. It is basically support material for the subject 6KP and its English version 6KP-A (basics of computational modeling using finite element method) taught in the Institute of Solid Mechanics, Mechatronics and Biomechanics, Faculty of Mechanical Engineering, Brno University of Technology.

Computer labs of 6KP and 6KP-A are composed of active exercises under the current interpretation of the fundamentals associated with the type of elements and also from a separate project for a group of students. The texts were made in two versions, for the computing open_source system Salome_Meca (C_A) and for computing system ANSYS Workbench v16.2.

Table of Contents

Credits and Copyright

Preface

INTRODUCTORY

General Information

The Design Modeler

Basic Mouse Functionality

Selection Filters

Selection Panes

Graphic Controls

Additional Mouse Controls

Understanding Cell States

i. Typical Cell States

ii. Solution-Specific States

iii. Failure States

3D Geometry

Bodies and Parts

Boolean Operations

Feature Type

Feature Creation

CHAPTER_I: CHILD SWING

1.1 Problem Description

1.2 Workbench GUI

1.3 Preparing Engineering Data

1.4 Create Geometric Model

1.4.1 2D and 3D Simulations

1.4.2 More on Geometric Modeling

1.5 Divide Geometric Model Into Finite Elements

1.6 Set Up Loads and Supports

1.7 Solve the Finite Element Model

1.8 Viewing the Results

1.9 Second Part of Our Task

CHAPTER_II: BEAM SYSTEM

2.1 Problem Description

2.2 Start-Up

2.3 Create Body

2.4 Create Cross-Section

2.5 Start-up “Mechanical”

2.6 Generate Mesh

2.7 Specify Boundary Conditions

2.8 Specify Loads

2.9 Set up Solution Branch and Solve the Model

2.10 View the Results

CHAPTER_III: PLATE43

3.1 Problem Description

3.2 Start-Up

3.3 Creating the 2D Geometry Model

3.4 Set Up Mesh Controls

3.5 Set Up Supports, Loads

3.6 Set Up Solution Outcome Branch

3.7 View the Results

3.7.1 Perform Simulations

3.8 Modify the Model

3.8.1 Set Up New Supports, Loads

3.8.2 Set Up New Mesh Controls

3.8.3 View the Results

3.9 Structural Error

3.10 Finite Element Convergence

3.11 Stress Concentration

3.11.1 View the Path Results

CHAPTER_IV: SHAFT

4.1 Problem Description

Examples before beginning our task

Shaft Description

4.2 Start-Up

4.3 Create Body

4.3.1 Getting back to the Modeling

4.4 Set Up Mesh Controls

4.5 Set Up Supports, Loads

4.6 Set Up Solution Outcome Branch

4.7 View the Results

4.7.1 Activating 3D View

4.9 Stress Concentration Factor

4.9.1 Hand Calculations VS Computational Calculations of Stress Concentration

Hand Calculations

Computational Calculations

Solving the Equation

4.10 Redefining Mesh

CHAPTER_V: LEVEL OF GEOMETRY

5.1 Problem Description

Car Chassis Description

i. Beam Elements

5.2.i Start Up

5.3.i Create Body

5.4.i Set Up Mesh Controls

5.5.i Set Up Supports, Loads

5.6.i Set Up Solution Outcome Branch

5.7.i View the Results

ii. Solid Elements

5.2.ii Start Up

5.3.ii Create Body

5.4.ii Set Up Mesh Controls

5.5.ii Set Up Supports, Loads

5.6.ii Set Up Solution Outcome Branch

5.7.ii View the Results

iii. Surface Elements

5.2.iii Start Up

5.3.iii Create Body

5.4.iii Set Up Mesh Controls

5.5.iii Set Up Supports, Loads

5.6.iii View the Results

iv. Type of Elements Comparison

CHAPTER_VI: TUNING FORK

6.1 Problem Description

6.2 Start Up

6.3 Create Body

6.4 Set Up Mesh Controls

6.5 Set Up Supports, Loads

6.6 View the Results

6.7 Modify Model

Changing Material

Changing the Dimensions

INTRODUCTORY

General Information      

# The ANSYS Workbench represents more than a general purpose engineering tool.

It provides a highly integrated engineering simulation platform.

It supports multi physics engineering solutions,

It provides bi-directional parametric associativity with most available CAD systems.

# These tutorials are designed to introduce you to

The capabilities, functionalities and features of the ANSYS Workbench.

The nature and design of the ANSYS Workbench User Interface.

The concepts of ANSYS Workbench Projects and related engineering simulation capabilities.

The integrated nature of ANSYS Workbench technology.

The power of the ANSYS Workbench in using applied parametric modeling and simulation techniques to provide quality engineering solutions.

The Design Modeler

# Sketching Mode:

Provides for the creation of sketches using standard or user defined model coordinate systems.

Supports the creation of 3D parametric solids from 2D sketches.

# Modeling Mode:

Provides tools for the creation and modification of 3D parts and models.

Tracks and supports modification of modeling operations.

Basic Mouse Functionality

# Model features are identified by graphically picking them using the left mouse button.

# Feature selection is done by activating one of the selection filters from the menu bar or from pop-up menus using the right mouse button.

# In selection mode, the cursor changes to reflect current selection filter.

# Adjacent and Flood Selections extend selections to adjacent areas. Additional information can be found in the ANSYS Workbench Help (documentation).

# Selection filters can also be set using pop-up menus (right mouse button in the Model View).

Selection Panes

Graphic Controls

Additional Mouse Controls

# While in Select Mode:

Center Mouse Button  Free Rotations.

Right Mouse Button  Box Zoom.

Shift+ Center Mouse Button  Zoom.

# While in Rotate, Pan or Zoom Mode:

Left click on model temporarily resets center of view and rotation at cursor location.

Left click in open area re-centers model and rotation center to centroid.

# Mouse Cursor is Context Sensitive.

Indication Current Mouse Actions [Viewing, Rotation, Selecting, Sketch AutoConstrains, etc.]

Understanding Cell States

ANSYS Workbench integrates multiple applications into a single seamless project flow, where individual cells can obtain data from and provide data to other cells. As a result of this flow of data, a cell’s state can change in response to changes made up to the project. ANSYS Workbench provides visual indications of a cell’s state at any given time via icons on the right side of each cell.

Cell states can be divided into the following categories:

i. Typical Cell States

Unfulfilled

Required upstream data does not exist. Some applications may not allow you to open them with the cell in this state. For example, if you have not yet assigned a geometry to a system, all downstream cells will appear as unfulfilled, because they cannot progress until you assign a geometry.

Refresh Required

Upstream data has changed since the last refresh or update. You may or may not need to regenerate output data. When a cell is in a Refresh Required state, you can Edit the cell, Refresh the data, Update Upstream Components, or Update the cell.

The advantage to simply refreshing a cell rather than performing a full update is that you can be alerted to potential effects on downstream cells before updating and can make any necessary adjustments. This option is especially useful if you have a complex system in which an update could take significant time and/or computer resources.

Attention Required

All of the cell’s inputs are current; however, you must take a corrective action to proceed. To complete the corrective action, you may need to interact with this cell or with an upstream cell that provides data to this cell. Cells in this state cannot be updated until the corrective action is taken.

This state can also signify that no upstream data is available, but you can still interact with the cell. For instance, some applications support an “empty” mode of operation, in which it is possible to enter the application and perform operations regardless of the consumption of upstream data.

Update Required

Local data has changed and the output of the cell needs to be regenerated.

Up to Date

An Update has been performed on the cell and no failures have occurred. It is possible to edit the cell and for the cell to provide up-to-date generated data to other cells.

Input Changes Pending

The cell is locally up-to-date but may change when next updated as a result of changes made to upstream cells.

ii. Solution-Specific States

Interrupted, Update Required

Indicates that you have interrupted the solution during an update, leaving the cell paused in an Update Required state.

This option performs a graceful stop of the solver, which will complete its current iteration; although some calculations may have been performed, output parameters will not be updated. A solution file will be written containing any results that have been calculated. The solve will be resumed with the next update command.

Interrupted, Up to Date

Indicates that you have interrupted the solution during an update, leaving the cell in an Up-to-Date state.

This option performs a graceful stop of the solver, which will complete its current iteration; output parameters will be updated according to the calculations performed thus far and a solution file will be written. You can use the solution for post processing (to look at the intermediate result, for example). Because the cell is already up-to-date, it will not be affected by a design point update; to resume the solve, right-click and select the Continue Calculation option.

Pending

Signifies that a batch or asynchronous solution is in progress. When a cell enters the Pending state, you can interact with the project to exit ANSYS Workbench or work with other parts of the project. If you make changes to the project that are upstream of the updating cell, then the cell will not be in an up-to-date state when the solution completes.

iii. Failure States

Refresh Failed, Refresh Required

The last attempt to refresh cell input data failed and the cell remains in a refresh required state.

Update Failed, Update Required

The last attempt to update the cell and calculate output data failed and the cell remains in an update required state.

Update Failed, Attention Required

The last attempt to update the cell and calculate output data failed. The cell remains in an attention required state.

If an action results in a failure state, you can view any related error messages in the Messages view by clicking the Show Messages button on the lower right portion of the ANSYS Workbench tab.

These parts will be transferred to Design Simulation as parts consisting of multiple bodies (volumes), but Shared Topology.

To form a new part, select two or more bodies from the graphics screen and use Tools Form New Part.

The Form New Part option is available only when bodies are selected and you are not in a feature creation or feature edit state.

Feature Type          

# Fixed:

Fixed extents will extrude the profiles the exact distance specified by the depth property. The feature preview shows an exact representation of how the feature will be created.

# Through All Type:

Will extend the profile through the entire model.

When adding material the extended profile must fully intersect the model.

# To Next:

Add will extend the profile up to the first surface it encounters.

Cut, Imprint and Slice will extend the profile up to and through the first surface or volume it encounters.

# To Faces:

Allows you to extend the Extrude feature up to a boundary formed by one or more faces.

For multiple profiles make sure that each profile has at least one face intersecting its extent. Otherwise, an extent error will result.

The “To Faces” option is different from “To Next”. To Next does not mean “to the next face”, but rather “through the next chunk of the body”.

The “To Faces” option can be used with respect to faces of frozen bodies.

# To Surface:

Feature Creation

# Sweep:

Solids, Surfaces and thin walled features can be created by using this feature to sweep a profile along a path.

Scale and Turns properties can be used to create helical sweeps.

Scale: Tapers or expands the profile along the path of the sweep.

Turns: Twists the profile as sweeps along the path.

A negative value for Turns will make the profile rotate about the path in the opposite direction.

Alignment:

Path Tangent:  Reorients  the  profile  as it is  swept along the path to  keep  the profile  in the path’s tangent direction.

Global: The profile’s orientation remains constant as it is swept along the path, regardless of the path’s shape.

# Skin/ Loft:

Takes a series of profiles from different planes to create 3D Geometry fitting through them.

A profile is a sketch with one closed or open loop or a plane from a face.

All profiles must have the same number of edges.

Open and closed profiles cannot be mixed.

All profiles must be of the same type.

Sketches and planes can be selected by clicking on their edges or points in the graphics area, or by clicking on the sketch or plane in the feature tree.

After selecting an adequate number of profiles, a preview will appear showing he selected profiles and the guide polygon.

The guide polygon is a gray poly-line which shows how the vertices between the profiles will line up with each other.

Skin/ Loft operation relies heavily on Right Mouse Button menu choices.

# Point:

The Point feature allows for controlled and fully dimensioned placement of points relative to selected model faces and edges.

Select a set of base faces and guide edges.

Select the Point (analysis) Type:

Spot Weld: Used for “welding” together otherwise disjointed parts in an assembly.

Point Load: Used for “hard points” (nodal points) in the analysis.

Sequence By Delta -- > Sigma, Offset, Delta.

Sequence By N -- > Sigma, Offset, N, Omega.

From Coordinates File -- > Formatted text file, similar to 3D curve.

Sigma: The distance between the beginning of the chain of guide edges and the placement of the first point.

Edge Offset: The distance between the guide edges and the placement of the spots on the set of base faces.

Delta: The distance, measured on the guide edges, between two consecutive points, for the Sequence By Delta option.

N: The number of points to be placed, relative to the chain of guide edges, in case of the Sequence By N option.

Omega: The distance between the end of the chain of guide edges and the placement of the last spot, for the Sequence By N option.

# Examples:                                        

CHAPTER_I: CHILD SWING

1.1 Problem Description

The purpose of this chapter is to find out the deformation of the beam and the displacement of its end point. Furthermore we will examine, how the stress will look like, when a loading by some specific weight, defined by the force.

Native applications are directly supported in “Workbench GUI”, their program codes and database blind together. Native applications which will be used to this book are: “Project Schematic”, “Engineering Data”, and “Design Exploration”.

1.3 Preparing Engineering Data

Double clicking to “Engineering Data” cell, will start Engineering Data application, where we want to specify our material properties. In this task our material is made by steel [Young’s Modulus= 200GPa, Poisson’s Ratio= 0,3] and as we can see, we don’t have to make any changes, as the default material properties of structural steel match with our requirements.

1.4 Create Geometric Model

1.4.1 2D and 3D Simulations

Workbench supports 2D and 3D simulations. For 3D simulations Workbench supports three types of geometric bodies: [1] Solid Bodies (which have volume) [2] Surface Bodies (which do not have volume but have surface areas) [3] Line Bodies (which do not have volume or surface areas but have length). Thin shell structures are often modeled as surface bodies. Beam or frame structures are often modeled as line bodies. A 2D model must be created entirely on <XYPlane>.

1.4.2 More on Geometric Modeling

Creating a geometric model is sometimes complicated and not as trivial as that in our first task. However it often can be viewed as a series of two-step operations as demonstrated in this case: Drawing a sketch and then using the sketch to create a 3D body by one of the techniques provided by Design Modeler such as extrusion, revolution, sweeping, skinlofting, etc.

Geometric modeling is the first step towards the success of simulations. For an engineer to be successful in simulation he/she must be proficient enough in geometric modeling.

Time to focus on our task and get more specific in certain commands of the Design Modeler application.

Now you can create a line with the given dimensions in the newly created “Sketch 1”.

After sketching our geometry we need to create a “Line Body”. Also we are going to need 2 different kind of Cross_Section. The way to do that is described in the pictures above.

1.5 Divide Geometric Model Into Finite Elements

The procedure that Workbench solves a problem can be viewed as two major steps: Establishing a set of equations that govern the behavior of the problem and ② Solving the equations. The problem domain (i.e. the geometric model) is usually so complicated that it is almost impossible to establish and solve the governing equations directly. A core idea in the finite element method is to divide the entire problem domain into many smaller and simpler domains called “the finite elements”. The elements are connected by nodes. The governing equations for all elements will be solved simultaneously.

The dividing of geometric model into elements is called meshing and the collection of the elements is called the finite element mesh or sometimes called the finite element model. Strictly speaking, a finite element model should mean a finite element mesh PLUS it’s environment conditions.

Quality of meshing cannot be overemphasized. Although it is possible to let ANSYS Workbench perfomrn the meshing automatically, it’s quality is not guaranted.

In the real world, all things are part of the world and they interact with each other. When we take an object apart for simulation, we are cutting it away from the rest of the world. The cutting surfaces of the model is called the boundary of the model. Where we cut the boundary is arbitrary – as long as we can specify the boundary conditions on all of the boundary surfaces. In Workbench all conditions affecting the response of the model are called the environment conditions which include boundary conditions. Strictly speaking, environment conditions include conditions that are not specified on the boundaries, for example, temperature changes over the entire body (not just on the boundary). In Workbench we don’t use the term “boundary conditions”, instead we will use the term “environment conditions”, which includes boundary and non-boundary conditions.

In our case scenario, the things surrounding our geometry are:

Atmosphere air around all the rest of boundary surfaces. BUT assuming the atmosphere air has very little interaction with the model we simply neglect it. We model all other boundary surfaces as free boundaries.

Fixed support in one end.

Force on the other end equal to 500N.

1.6 Solve the Finite Element Model

To solve a finite element model, simply click <Solve> in Mechanical GUI. The solution procedure is entirely automatic. The time to complete a simulation depends on the problem size and complexity. After the solution, the numerical results are stored in a database.

1.7 Viewing the Results

After the solution, numerical results are stored in databases, they can be viewed upon your request. In our case we are most concerned about the vertical deflection. The deformation also can be animated in the GUI. Note that the deflection is measured at the tip.

1.8 Second Part of Our Task

In order to change the type of our cross section, we have to go back to Design Modeler and add one more type of cross section.

Note: We don’t have to close Mechanical GUI, just Alt+Tab back to Geometry Mode.

After you are finished adding the new cross section to our model, hit Alt+Tab again to get you back to “Mechanical GUI”. Now all we have to do is update the geometry (since we still got the geometry with the previous cross section shown to the Mechanical) and solve the problem again.

There is a lot different things that we can do to change the geometry and see results of different aspects. Let’s try and change the cross section’s alignment. Go back to Design Modeler and change the alignment according to the picture.

After finishing the configurations in Design Modeler, Alt+Tab again to get back to Mechanical GUI, update geometry from source again, mesh the model and solve it.

CHAPTER_II: BEAM SYSTEM

2.1 Problem Description

In this chapter we are asked to create a 3D Cube Beam System. The Cube Beam System has a square cross-section which is given below.

2.2 Start-Up

As we progress forward to more complicated tasks/geometries, the steps that we were explaining so detailed in  the previous chapters won’t be explicated as much.

2.3 Create Body

The Lines From Edges feature allows the creation of Line Bodies in ANSYS DesignModeler that are based on existing model edges. The feature can produce multiple line bodies, depending on the connectivity of the selected edges and faces. Select 3D model edges, and faces through two Apply/Cancel button properties.

The Lines From Points feature allows the creation of Line Bodies in ANSYS DesignModeler that are based on existing points. Points can be any 2D sketch points, 3D model vertices, and point feature points (PF points). The feature's selections are defined by a collection of point segments. A point segment is a straight line connecting two selected points. The feature can produce multiple line bodies, depending on the connectivity of the chosen point segments. The formation of point segments is handled through an Apply/Cancel button property.

After you are done sketching, right-click on Solid choose suppress body and you should have the same looks as above.

Cross-Section Alignments

The default cross section alignments usually need to be adjusted so that they are consistent with the reality. In this chapter we decided to leave them default. In other words cross section alignments do not affect the structural response too much in this case.

2.6 Generate Mesh

2.10 View the Results

CHAPTER_III: PLATE

3.1 Problem Description

In this chapter we are interested to know the concepts of Finite Element Simulation, like “Stress Discontinuity”, “Structural Error”, “Stress Singularity”, “Finite Element Convergence”.

To demonstrate this concepts we are going to use a Plate geometry with notch, which is made out of steel and has the given dimensions. The bar has Fixed Support on the left side and is subject to a tension of 50MPa on the right side.

3.2 Start-Up

Launch Workbench, create a Static Structural system by choosing it from the list on the left (toolbox). Save the project before we begin, to an appropriate location and name.

As soon as DesignModeler opens, go to Units and select Millimeters.

3.3 Creating the 2D Geometry Model

Let’s start creating our Geometry. Choose XYPlane as your sketch plane, open Sketching tab and create our Plate Bar.

3.4 Set Up Mesh Controls

3.5 Set Up Supports, Loads

3.7 View the Results

3.7.1 Perform Simulations

3.8.1 Set Up New Supports, Loads

Make sure you got the correct Units selected in the Unit tab. Specify fixed support on the left edge and horizontal force of 50 MPa on the right edge.

Insert Direction Deformation and two Normal Stresses (Averaged and Unaveraged), under the solution branch.

3.8.2 Set Up New Mesh Controls

3.8.3 View the Results

3.9 Structural Error

3.10 Finite Element Convergence

One of the core concepts of the finite element method is that, as mentioned, the finer the mesh, the more accurate the solution. Ultimately, the solution will reach the analytical solution. But how fast does it approach that solution? This is what we want to answer in this part of the chapter.

3.11 Stress Concentration

If we want to see how the stress concentrates in a specific area, we will need to create a path and then we will investigate the stresses along that path. Path command is also useful to make finer mesh in that specific area.

A path can be defined by two points, or an edge. Coordinates of the points can be either picked from the model or typed in the Details View.

Any result objects can scope on a path. After solving, a result vs path data table along with a graph will be generated.

3.11.1 View the Path Results

CHAPTER_IV: SHAFT

4.1 Problem Description

A structure of revolution by itself does not necessarily define an axisymmetric problem. It is also necessary that the loading, as well as the support boundary conditions, be rotationally symmetric.

Axisymmetric elements are 2D elements that can be used to model axisymmetric geometries with axisymmetric load. In simpler words, we are converting a 3D Geometry to a 2D Geometry making the model smaller, therefore faster execution and faster post processing.

We only model the cross section, and ANSYS accounts for the fact that it is really a 3D, axisymmetric structure.

Examples before beginning our task

Shaft Description

In this chapter we consider the finite element discretization of axisymmetric solids. We were given a Steel Shaft with dimensions which are given below. Purpose of this chapter is to evaluate stress concentration factor of the shaft notch, compare the result with the experimental data and fully understand the concept of Axi-symmetry and its possibilities.

4.2 Start-Up

Open ANSYS Workbench, create a Static Structural system, and make sure that you saved your case study before moving forward. Next step is opening Engineering Data tab, to check if the material properties are correct. After doing, that highlight Geometry and change the Analysis Type on your right, from 3D to 2D. Double-click Geometry to start sketching.

4.3 Create Body

After DesignModeler opens, get to the Units tab, and select Millimeter. Highlight XYPlane and start sketching.

4.3.1 Getting back to the Modeling

4.4 Set Up Mesh Controls

After finishing your sketch, close DesignModeler and open up Mechanical. First thing we need to adjust before start dealing with the Analysis, is to change Geometry’s behavior.

4.5 Set Up Supports, Loads

4.7 View the Results

4.7.1 Activating 3D View

To help you understand the ideology of Axisymmetry, I will have to show you how to activate a couple of options to make a better visualization output of the results.

4.9 Stress Concentration Factor

A stress concentration is a location in an object where stress is concentrated. An object is strongest when force is evenly distributed over its area, so a reduction in area, e.g. caused by a crack, results in a localized increase in stress. A material fail, via a propagating crack, when a concentrated stress exceeds the material’s theoretical cohesive strength. The real fracture strength of a material is always lower than the theoretical value because most materials contain small cracks or contaminants that concentrate stress.

The stress concentrators are geometrical irregularities that cause an increase in the average effort that should be present in regions near these discontinuities, the relationship between the maximum stress that occurs and the average effort that should occur is defined as stress concentration factor; which is determined by experimental or analytical methods and presented in graphical form for ease interpretation.

The stress concentration factor for a tube in tension with fillet, our case, can be determined as the relation of the maximum normal stress in the discontinuity and the nominal stress, and is obtained through the equation:

4.9.1 Hand Calculations VS Computational Calculations of Stress Concentration

Hand Calculations

As we can see in the graph, there are 2 parameters that are taken into consideration to acquire stress concentration factor. First parameter would be to determine which line we need to choose, to accomplish that we have to solve the equation t/h with our given values. Second parameter would be to acquire the correct output for the X axis, solving the equation t/r.

To acquire the Stress Concentration Factor for the computational calculations we are going to need Max. Normal Stress (Y Axis) and Nominal Stress, which in our case equals to 50MPa because of Pressure.

Solving the Equation 

Conclusion: As we can see the results between Hand and Computational Calculations are almost the same. The difference of 11% is probably because of the geometry. Geometry proportion does not meet the criterion for the experimental data in the Stress Concentration Factor diagram, [Eq. ]. The Geometry proportion coefficient should be greater than 28.

4.10 Redefining Mesh

At this point we come across with an opportunity, to help you understand the concepts and the possibilities of Mesh and its options. To be more specific, we will change our element and node parameters (make it smaller, and finer), to check what happens to the Stress Concentration Factor. We are aiming to reduce the difference to a minimum value.

We can see that, we may got a difference in the Stress Concentration Factor but it is negligible.

CHAPTER_V: LEVEL OF GEOMETRY

5.1 Problem Description

Beam Element - A beam element is a slender structural member that offers resistance to forces and bending under applied loads. A beam element differs from a truss element in that a beam resists moments (twisting and bending) at the connections.

These three node elements are formulated in three-dimensional space. The first two nodes (I-node and J-node) are specified by the element geometry. The third node (K-node) is used to orient each beam element in 3-D space (see Figure 1). A maximum of three translational degrees-of-freedom and three rotational degrees-of-freedom are defined for beam elements (see Figure 2). Three orthogonal forces (one axial and two shear) and three orthogonal moments (one torsion and two bending) are calculated at each end of each element. Optionally, the maximum normal stresses produced by combined axial and bending loads are calculated. Uniform inertia loads in three directions, fixed-end forces, and intermediate loads are the basic element based loadings.

The basic guidelines for when to use a beam element are:

The length of the element is much greater than the width or depth.

The element has constant cross-sectional properties.

The element must be able to transfer moments.

The element must be able to handle a load distributed across its length.

Solid Element – Solid elements are three-dimensional finite elements that can model solid bodies and structures without any a priori geometric simplification.

Finite element models of this type have the advantage of directness. Geometric, constitutive and loading assumptions required to effect dimensionality reduction, for example to planar or axisymmetric behavior, are avoided. Boundary conditions on both forces and displacements can be more realistically treated. Another attractive feature is that the finite element mesh visually looks like the physical system.

Summarizing, use of solid elements should be restricted to problem and analysis stages, such as verification, where the generality and flexibility of full 3D models is warranted. They should be avoided during design stages. Furthermore they should also be avoided in thin-wall structures such as aerospace shells, since solid elements tend to perform poorly because of locking problems.

Shell Element – Shell elements are 4- to 8-node isoparametric quadrilaterals or 3- to 6-node triangular elements in any 3-D orientation. The 4-node elements require a much finer mesh than the 8-node elements to give convergent displacements and stresses in models involving out-of-plane bending. Figure 1 shows some typical shell elements.

The General and Co-rotational shell element is formulated based on works by Ahmad, Iron and Zienkiewicz and later refined by Bathe and Balourchi. It can be applied to model both thick and thin shell problems. Also, the geometry of a doubly curved shell with variable thickness can be accurately described using this shell element.

The Thin shell element is based on thin plate theory. The bending behavior of the element is based on a discrete Kirchhoff approach to plate bending using Batoz's interpolation functions. This formulation satisfies the Kirchhoff constraints along the boundary and provides linear variation of curvature through the element. The membrane behavior of the element is based on the Allman triangle which is derived from the Linear Strain Triangular (LST) element. A general curved surface is approximated by this element as a set of facets formed by the planes defined by the three nodes of each element. For these reason a well-refined mesh is necessary.

The element geometry is described by the nodal point coordinates. Each shell element node has 5 degrees of freedom (DOF) - three translations and two rotations. The translational DOF are in the global Cartesian coordinate system. The rotations are about two orthogonal axes on the shell surface defined at each node. The rotational boundary condition restraints and applied moments also refer to this nodal rotational system. The two rotational axes (V1 and V2) are usually automatically determined by the processor and you do not have to specifically orient them.

Car Chassis Description

To be able to make the comparison between beam, solid and surface elements we are going to need a geometry which is compatible with all 3 parameters. That is why we are going to use a part of a Car Chassis with dimensions and loads which are given below.

i. Beam Elements

5.2.i Start Up

Once you opened up ANSYS Workbench, create a new Static Structural System and save your study case to a proper destination folder. Afterwards open the Engineering Data tab and make sure that the material properties match our data. Getting back now to the Project tab, we need to make an adjustment, since we are working with Beam Elements. For that reason, highlight Geometry from the Static Structural System and tick the box in the Basic Geometry Options tab, the once concerning the Line Bodies. Double click on Geometry to start sketching.

5.3.i Create Body

As you noticed in the Problem Description paragraph, our model is symmetric, meaning that we got the option here to sketch only half of the geometries body without having differences at the end results. So, getting back to the sketching part, we will need firstly to create just a single line and then it’s Cross-Section.

After creating the geometry, in our case the single Line, head back to Modelling tab.

5.4.i Set Up Mesh Controls

Your Geometry Body is ready, close DesignModeler and open up Mechanical GUI, by double clicking on the Model from the Static Structural System (we do not need to make any modifications in this case before opening up Mechanical GUI).

5.6.i Set Up Solution Outcome Branch

ii. Solid Elements

5.2.ii Start Up

Next part of this chapter would be, creating the same geometry, with the same boundary conditions, the same loads. Only difference would be that, this time we will use solid elements for our analysis. Open up your previous study case (Car Chassis), and create a new Static Structural System, check again your Engineering Data to much with our data and leave everything else as default· open up DesignModeler, and change your Units to Millimeters.

5.4.ii Set Up Mesh Controls

After finishing with sketching the geometry, close DesignModeler and open up Mechanical GUI, by double clicking on the Model from the Static Structural System (there is no need to make any modifications).

5.5.ii Set Up Supports, Loads

5.6.ii Set Up Solution Outcome Branch

5.7.ii View the Results

iii. Surface Elements

5.2.iii Start Up

In this study case, it will not be needed to create a new Static Structural System and sketching the geometry from all over again. There is an easier way by Duplicating the Solid Elements study case, with this option the newly created Static Structural System has the exact same geometry, mesh and boundary conditions like the Static Structural System that we Duplicated. After Duplicating it, open up DesignModeler to make some modifications regarding the Surface Elements.

5.3.iii Create Body

One of the better features of Workbench’s DesignModeler is the Mid-Surface Extraction tool. This tool is fairly simple to use, and after some practice, you will be creating shell models in no time. The Mid-Surface Extraction utility is located underneath the ‘Tools’ Menu.

The easiest way to create Mid-Surfaces is to manually go through and select the face pairs. You will notice that after selecting the “top” and “bottom” face, they will appear as two different colors. It is important to note that the order in which you click the two faces determines the ”top” and ”bottom” of the shell element (important for applying pressures/defining contact). The shell normal is positive going from the pink (2nd pick) to the purple (1st pick) surface.

You can select multiple face pairs, then go back and hit the apply button for “Face Pairs” in the detail window. If there are several face pairs that have the same thickness, you can select one pair, then go back and change the selection type to be automatic. This will fill in some blanks in the details window.

Finally, change “Find Face Pairs Now” to be “Yes” and DesignModeler will go out and find all face pairs that meet this criteria. Hit generate and all of your midplanes will be generated, and all thicknesses will be stored for later use in Simulation.

5.4.iii Set Up Mesh Controls

We are done with the DesignModeler, so feel free to close the window, and open Mechanical GUI by double clicking at the Model from the Static Structural System. A pop up window will appear asking you if you want to read the up-stream data, which means that the Mechanical GUI will automatically load the new changes we made in the DesignModeler, click Yes.

5.5.iii Set Up Supports, Loads

As you probably already understood, we are not going to change the mesh, the supports, the loads or the solution outcomes. Thanks to the Duplication the parameters are already settled and we just need to define the new changed geometry.

5.6.iii View the Results

iv. Type of Elements Comparison

We could compare and comment the results of all 3 different type of elemets.

CHAPTER_VI: TUNING FORK

6.1 Problem Description

In this chapter, we want to perform a Modal Analysis to investigate the natural frequencies of a Tuning Fork. The specific tuning fork is designed to tune chamber A 440Hz. In the case that the tuner does not meet the stated requirements, we will modify the geometry, material or mass of the tuner in order to get the correct frequency output.

For that reason, we will set from the start some parameters (Parametric Model) which will help us to modify the geometry’s dimensions easier and without the need to sketch the tuning fork from scratch.

6.2 Start Up

Open up ANSYS Workbench, locate Modal from the Toolbox/ Analysis Systems and drag and drop it to the Project Schematic as you did with the Static Structural Systems. Save your study case to a proper destination folder, head to the Engineering Data tab to make sure that your material properties match with the given ones.

6.3 Create Body

When the DesignModeler loads, make sure to change the Units type to Millimeter and move to the Sketching tab to create our tuning form geometry.

As you noticed in the Problem Description paragraph, our model is symmetric, meaning that we got the option here to sketch only half of the geometry body without having differences at the end results. So, getting back to the sketching part, we will need to create a sketch like the figure below.

6.4 Set Up Mesh Controls

Your Geometry Body is ready, close DesignModeler and open up Mechanical GUI, by double clicking on the Model from the Modal Analysis System (we do not need to make any modifications in this case before opening up Mechanical GUI).

6.5 Set Up Supports, Loads

6.6 View the Results

6.7 Modify Model

i. Changing Material

In this section, we will define a new material to see if we have a difference in the frequency outputs. We will change the material from Structural Steel to Copper Alloy. In order to do that, we will need to assign the new material in the Engineering Data tab, let’s see how to do that. Close Mechanical UI, and open Engineering Data tab.

ii. Changing the Dimensions

Since, changing the material did not help us get the required frequency results, we will try now and change some dimensions from our tuner and see how it affects the frequency results. Changing all the dimension would not be much of a help for us, we will modify the l=length dimension and possibly the thickness of the tuner.

We can always follow the procedure we did in Chapter_III [section 3.8], and change the dimensions in the DesignModeler-Head back to the Mechanical UI-Update Geometry from Source-Solve and get the new result outputs.

In this section, I will introduce you a new way to make modifications in the geometry, which will be easier and faster. We will assign some parameters, and by changing those parameters we will be able to see instantly the frequency result outputs.