CATIA V5 Analysis
Lesson 2: Pre-processing
Student Notes:
In this lesson, you will learn the FEA pre-processing (FE modeling ) concepts and how to perform pre-processing steps in GPS workbench.
Copyright DASSAULT SYSTEMES
Lesson content:
Case Study: FE Modelling of Drill Press Table Design Intent Stages in the Process What is Pre-processing Applying Material Generating Mesh Assigning Physical Property Applying Restraints and Loads Checking the Finite Element Model
Duration: Approximately 0.25 days
Copyright DASSAULT SYSTEMES
1
CATIA V5 Analysis
Case Study: FE Modelling of Drill Press Table
Student Notes:
The case study for this lesson is the Drill Press Table. The focus of this case study is to create a Finite Element model for Drill Press Table. Introduction to FEA
•Exercises
GPS preprocessing
•Exercises
Copyright DASSAULT SYSTEMES
(Case Study)
GPS Computation
•Exercises
GPS Postprocessing
Mesh Refinement
•Exercises
•Exercises
•Exercises
Master Project
Drill Press Table Component
Copyright DASSAULT SYSTEMES
Assembly Structural Analysis
Drill Press Table with Mesh, Restraints and Load
2
CATIA V5 Analysis Student Notes:
Design Intent You have to perform the Static Analysis of Drill press Table. The actual physical problem will be described which will provide input data for FE modeling of the drill press Table. You have to use this information to build an appropriate FE model. The table of drill press is composed of steel having following properties: The material is isotropic Young's Modulus = 2.1e+011 N_m2 Poisson's Ratio = 0.268 Density = 7862 kg/m3 Thermal Expansion = 1.19e-005 /Kdeg Yield Strength = 2.6e+008 N_m2 The mesh type must be 3D OCTREE Tetrahedron
Copyright DASSAULT SYSTEMES
The table is fixed to the stand with a Clamp restraint
Drill Press Table Component
A downward force of 10 N will be applied and transmitted to the top surface of the table through the drill-bit and work-piece The validity of the created FE model must be checked
Copyright DASSAULT SYSTEMES
3
CATIA V5 Analysis Student Notes:
Stages in the Process This will involve following steps to perform the case study. First, you will understand what is Pre-processing. Later you will see how to perform each Pre-processing step in the GPS workbench. 1. 2. 3. 4. 5. 6.
What is Pre-processing Applying Material Generating Mesh Assigning Physical Property Applying Restraints and Loads Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
Drill press Table FE Model
Copyright DASSAULT SYSTEMES
4
CATIA V5 Analysis
Step 1: What is Pre-processing
Student Notes:
You will get learn what is preprocessing and activities to be performed in pre-processing.
What is Pre-processing
2. 3. 4. 5. 6.
Applying Material Generating Mesh Assigning Physical Property Applying Restraints and Loads Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1.
Copyright DASSAULT SYSTEMES
5
CATIA V5 Analysis Student Notes:
What is Pre-processing Pre-processing involves all those steps which are required to convert a given physical problem into an equivalent Finite Element problem. This involves following steps: 1.
Copyright DASSAULT SYSTEMES
2.
Applying material structural property to a part, which is required to calculate deformation, strains and stresses
Pre-processing (FE Modeling)
Computation (Solving FE Model)
Meshing the part to create Finite Element model using elements and nodes
3.
Applying physical property to the mesh to associate physical properties and material to Finite Element model
4.
Applying restraints to the mesh which represents actual physical boundary conditions
5.
Applying loads on the mesh, which represents actual physical forces acting on the structure
6.
Model Checking to validate that all pre-processing steps are performed correctly to perform computation and nothing missed out
Copyright DASSAULT SYSTEMES
Post-processing (View Results)
Mesh Refinement Iterations
Create Reports Finite Element Analysis Process
6
CATIA V5 Analysis Student Notes:
Step 2: Applying Material You will learn tools to assign material property to part.
What is Pre-processing
2.
Applying Material
3. 4. 5. 6.
Generating Mesh Assigning Physical Property Applying Restraints and Loads Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1.
Copyright DASSAULT SYSTEMES
7
CATIA V5 Analysis
Material
Student Notes:
Structural properties of material are required to calculate deformation, strains and stresses. This include : Young Modulus Poisson Ratio Density of Material Yield Strength Thermal Expansion You can apply material in following two ways. select a material from default Material catalog
Copyright DASSAULT SYSTEMES
create your own user-defined material with required properties
Copyright DASSAULT SYSTEMES
8
CATIA V5 Analysis Student Notes:
Applying Material (1/2) You will see how to apply a material to part from material catalogue. 1.
Copyright DASSAULT SYSTEMES
2. 3.
2
In Apply Material toolbar click Apply Material icon. 1 Click on Metal tab and select Steel. Click on the PartBody in specification tree or on part displayed on screen and click OK.
Copyright DASSAULT SYSTEMES
3
9
CATIA V5 Analysis Student Notes:
Applying Material (2/2) 4.
5. 6.
In View Mode toolbar, click Customize View Parameters icon, to view part in Material mode. Check Material option and keep other options as shown. Click OK.
4
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
Part shown in Custom View Mode 6
10
CATIA V5 Analysis Student Notes:
Creating User Material (1/2) You may need to create a material with specified properties, which is not available in standard material catalogue. In this case, you can use User Material option to create a material with your own specification. This option creates material without any geometric support. Therefore, this can also be used to apply material to orphan meshes which do not have any geometric support. You will see how to create a User Material and how to edit the structural properties. 1.
2
Copyright DASSAULT SYSTEMES
2.
In Model Manager toolbar click User Material icon. Click on Metal tab and select Steel and click OK.
1
Copyright DASSAULT SYSTEMES
11
CATIA V5 Analysis Student Notes:
Creating User Material (2/2) 3. 4. 5.
In Materials.1 node in specification tree double-click on User Material.1. Click on the Analysis tab in Properties Dialogue box . Change the required structural properties as per specification and click OK.
3
4
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
12
CATIA V5 Analysis Student Notes:
Step 3: Generating Mesh You will learn what is mesh generation, different types of elements generated in mesh and tools to generate the mesh in CATIA. What is Pre-processing Applying Material
3.
Generating Mesh
4. 5. 6.
Assigning Physical Property Applying Restraints and Loads Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1. 2.
Copyright DASSAULT SYSTEMES
13
CATIA V5 Analysis Student Notes:
Mesh Generation (1/3) Meshing involves approximating actual physical structure into Finite Element model using several simple geometric shapes called elements. These Elements are interconnected to each other at points called Nodes. Within each element, displacement of nodes is defined by polynomial equation called Displacement Equation. The mesh is the representation of the mathematical idealization of the structure. On the basis of dimensionality elements can be classified as: 1-D Elements : These elements are used to represent structures where one of its dimension is really greater than the two others. Nodes
Copyright DASSAULT SYSTEMES
2-D Elements : These elements must be used to represent structures where two of its dimension are really greater than the third one.
3-D Elements : These elements must be used to represent parts where each dimension are of the same order of length.
Copyright DASSAULT SYSTEMES
14
CATIA V5 Analysis Student Notes:
Mesh Generation (2/3) Within each element, displacement of nodes is defined by polynomial equation called Displacement Equation. Elements can also be classified according to order of Displacement Equation as: Linear Elements : Linear Elements have linear displacement interpolation between the nodes. It means, when the linear elements are subjected to loads their shape follow linear deformation between the nodes. All elements described below are linear elements.
Copyright DASSAULT SYSTEMES
1-D Element :
Linear Beam Element
2-D Elements :
Linear Triangular Element
3-D Elements :
Linear Tetrahedron Element
Copyright DASSAULT SYSTEMES
Linear Quadrilateral Element
Linear Wedge Element
Linear Brick Element
15
CATIA V5 Analysis Student Notes:
Mesh Generation (3/3) Higher order elements : These elements use parabolic, cubic or higher order displacement interpolation function between the nodes. Thus, when the parabolic elements are subjected to loads their shape follow parabolic deformation equation. These elements have additional nodes on side between primary nodes. They are used to improve the accuracy of solution, however they increase the computation time. Higher order elements can be further classified according to dimensionality.
1-D Element :
Parabolic Beam Element
Copyright DASSAULT SYSTEMES
Primary nodes
2-D Elements :
Parabolic Triangular Element
3-D Elements :
Parabolic Tetrahedron Element
Copyright DASSAULT SYSTEMES
Parabolic Quadrilateral Element
Parabolic Wedge Element
Secondary nodes
Parabolic Brick Element
16
CATIA V5 Analysis Student Notes:
Using Beam Mesher (1/3) Beam Mesher is used to create 1-D beam element mesh. It provides linear as well as parabolic elements. You can use beam meshing for wireframe parts. You will see how to create beam mesh. 1. 2. 3. 4. 5. 6. 7.
In Mesh Parts toolbar, click Beam Mesher icon. Click on the edge to be meshed. Click on Element Type button to select parabolic element. Enter Element Size. Check Sag control option. Sag control is generally used in case of curved geometry. Enter sag size in the Sag: field. Enter Min size and click OK. In similar way, mesh all the edges using Beam Mesher.
1
2
Geometry to be meshed
3 4
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
6 7
17
CATIA V5 Analysis Student Notes:
Using Beam Mesher (2/3) 8.
Right-click on the Nodes and Elements in specification tree to open contextual menu. 9. Click on Mesh Visualization option. 10. Double-click on the Mesh Image icon to edit the image. 11. In Mesh Tab, check the Display nodes of elements option. 12. Click OK.
8
9
Copyright DASSAULT SYSTEMES
11 10
FE Model for the above geometry
Copyright DASSAULT SYSTEMES
12
18
CATIA V5 Analysis
Using Beam Mesher (3/3)
Student Notes:
In the FE mesh the effect of sag is important. Sag is the general maximum tolerance between discretization and the real part used for the computation. The element size you are using will not exactly map to the curved geometry. Sag is the perpendicular distance between the actual geometry and the Element. Lesser the sag value finer will be the mapping of elements with geometry and more accurate will be the FE model. Generally SAG value is taken 10% of the element mesh size. The effect of sag value can be studied using the beam meshing. Yellow color shows actual geometry curve. Green color shows FE Model.
Copyright DASSAULT SYSTEMES
In a similar way, the sag is applicable to the triangle and tetrahedron mesh also.
Copyright DASSAULT SYSTEMES
19
CATIA V5 Analysis Student Notes:
Using OCTREE Triangle Mesher (1/2) OCTREE Triangle Mesher is used to create 2-D triangular element mesh. It provides linear as well as parabolic elements. You can use this meshing for surface parts. You will see how to create OCTREE Triangle mesh. 1. 2. 3. 4. 5. 6.
1
2
In Mesh Parts toolbar, click OCTREE Triangle Mesher icon. Click on the surface to be meshed. In Global Tab, Enter element Size Check Absolute sag option and enter the value. In Element Type, check parabolic element. Click OK. 3
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
5 6
20
CATIA V5 Analysis Student Notes:
Using OCTREE Triangle Mesher (2/2) 7.
8.
Right-click on the Nodes and Elements in the specification tree to open contextual menu. Click on Mesh Visualization option. You will get the mesh image.
7
Copyright DASSAULT SYSTEMES
8
Copyright DASSAULT SYSTEMES
21
CATIA V5 Analysis Student Notes:
Using OCTREE Tetrahedron Mesher (1/3) OCTREE Tetrahedron Mesher is used to create 3-D tetrahedral elements popularly known as tet mesh. It provides linear as well as parabolic elements. You can use this meshing for solid parts. You will see how to create OCTREE Tetrahedron mesh. 1. 2. 3. 4. 5. 6.
In Mesh Parts toolbar, click OCTREE Tetrahedron Mesher icon. Click on the part to be meshed. In Global Tab, Enter element Size. Check Absolute sag option and enter the value. In Element Type, check parabolic element. Click OK.
1
2
3
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
5 6
For part geometry, once you switch to GPS workbench, OCTREE Mesh is automatically applied.
22
CATIA V5 Analysis Student Notes:
Using OCTREE Tetrahedron Mesher (2/3) 7.
8.
Right-click on the Nodes and Elements in the specification tree to open the contextual menu. Click on Mesh Visualization option. You will get the mesh image.
7
Copyright DASSAULT SYSTEMES
8
Copyright DASSAULT SYSTEMES
23
CATIA V5 Analysis
Using OCTREE Tetrahedron Mesher (3/3)
Student Notes:
The effect of sag is important in the triangle and tetrahedron mesh also, as in beam mesher. The two types of sag are global sag and local sag. Global sag is the general maximum tolerance between discretization and the real part used for the computation. Local sag is the maximum tolerance between discretization and the real part applied locally, to a user specified area of the model.
Copyright DASSAULT SYSTEMES
You can study the change in the mesh with change in either global or local sag value, from the images.
FE Model with Element size 15mm Absolute sag 1.5mm
Local sag is applied to the area of hole FE Model with Element size 15mm, Absolute sag 0.5 mm, Local sag 0.1mm
Copyright DASSAULT SYSTEMES
FE Model with Element size 15mm, Absolute sag 0.5 mm
24
CATIA V5 Analysis
Step 4: Assigning Physical Property
Student Notes:
You will learn what is Physical Property, different types of Physical Property and how to assign Physical Property to mesh. What is Pre-processing Applying Material Generating Mesh
4.
Assigning Physical Property
5. 6.
Applying Restraints and Loads Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1. 2. 3.
Copyright DASSAULT SYSTEMES
25
CATIA V5 Analysis Student Notes:
Physical Property Physical Property associates various physical properties to the mesh generated. In CATIA, physical property means cross-section, thickness, material properties. It uses geometry of the mesh or mesh part as support to apply Physical Property. You can also apply physical property directly to orphan meshes. Different physical property to be attached depends on the mesh used to create FE model as shown in following table.
Physical Property Assigned to Mesh
Mesh Type
Physical Property Name
Beam
1D Property
1. 2.
Cross-section Material
2D Property
1. 2.
Thickness Material
3D Property
1.
Material
OCTREE Triangle
Copyright DASSAULT SYSTEMES
OCTREE Tetrahedron
Copyright DASSAULT SYSTEMES
26
CATIA V5 Analysis Student Notes:
1D Property 1D Property offers you a set of standard cross-sections and material to be associated to the beam mesh. You can create a FE model for all standard available cross-sections using beam mesh.
Copyright DASSAULT SYSTEMES
Consider a case of creating a FE model for actual I-beam channel as shown using 1-D beam element. You will use line geometry with length equal to channel length and mesh it using Beam Mesher. Now you will see how to apply 1D Property to beam mesh.
1D Beam Mesh with line geometry
Copyright DASSAULT SYSTEMES
I-beam channel section to be FE modeled using Beam Mesh and 1D property
27
CATIA V5 Analysis Student Notes:
Applying 1D Property (1/2) 1. 2. 3. 4.
In Model Manager toolbar, click 1D Property icon. Click on the edge as a support in the Supports field. Check User-defined material option. Click in the Material field and select User Material.1 from the specification tree.
1
2
Copyright DASSAULT SYSTEMES
3
Copyright DASSAULT SYSTEMES
4
If material is already applied to the geometry it will be by default assigned in the Material field. You can change the material by checking User-defined material option.
28
CATIA V5 Analysis Student Notes:
Applying 1D Property (2/2) 5. 6. 7. 8. 9.
In Type field, select Thin I-beam from dropdown. Click on the Component edition button to enter thin I-beam parameters. Enter Beam Definition parameters and click OK. In Orientation geometry field, select xy plane from the specification tree. Click OK.
5
6 8
9
7
Copyright DASSAULT SYSTEMES
8
Copyright DASSAULT SYSTEMES
FE model for I-beam channel section using Beam Mesh
29
CATIA V5 Analysis Student Notes:
2D Property 2D Property allows you to associate thickness and material to the OCTREE Triangle mesh. Consider a case of creating the FE model for a sheet metal section, as shown using OCTREE Triangle elements. You will use sheet metal section surface geometry and mesh it using OCTREE Triangle Mesher. Now you will see how to apply 2D Property to OCTREE Triangle mesh to associate thickness and material.
Copyright DASSAULT SYSTEMES
Sheet metal section to be FE modeled using OCTREE Triangle Mesh and 2D Property
If material is already applied to the geometry it will by default get assigned in Material field. You can change the material by checking User-defined material option.
Copyright DASSAULT SYSTEMES
OCTREE Triangle Mesh with surface geometry
30
CATIA V5 Analysis Student Notes:
Applying 2D Property 1. 2. 3. 4. 5.
In Model Manager toolbar, click 2D Property icon. Click on the surface as a support in the Supports field. Check User-defined material option. Click in the Material field and select User Material.1 from the specification tree. Enter 5mm in Thickness field and click OK.
1
2
2 4 Copyright DASSAULT SYSTEMES
3
Copyright DASSAULT SYSTEMES
5
31
CATIA V5 Analysis Student Notes:
3D Property 3D Property lets you to assign material to be associated to the OCTREE Tetrahedron mesh. Consider a case in which turbine blade part geometry is meshed using OCTREE tetrahedron elements. Now you will see how to assign 3D Property.
Copyright DASSAULT SYSTEMES
Turbine blade to be FE modeled using OCTREE Triangle Mesh and 3D Property
If material is already applied to the geometry it will by default get assigned in Material field. You can change the material by checking User-defined material option.
Copyright DASSAULT SYSTEMES
32
CATIA V5 Analysis Student Notes:
Applying 3D Property 1. 2. 3. 4. 5.
In Model Manager toolbar click 3D Property icon. Click on the part geometry as a support in the supports field. Check User-defined material option. Click in the Material field and select User Material.1 from the specification tree. Click OK.
1
2
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
3
5
33
CATIA V5 Analysis
Exercise 2A
Student Notes:
Recap Exercise 15 min
In this exercise, you will perform Beam meshing for 1D component and assign 1D Property. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Use Beam Mesher
Copyright DASSAULT SYSTEMES
Assign 1D Property to beam mesh
Copyright DASSAULT SYSTEMES
34
CATIA V5 Analysis Student Notes:
Exercise 2A (1/2) 1.
Open a part. Open 2A_Hollow_Shaft_1D_Start.CATPart.
2.
Create a Static Analysis Case. Access GPS workbench. Create a Static Analysis Case. a.
3.
Click OK for the warning message.
Mesh the geometry. Mesh the line geometry with Beam Mesher. a. b. c. d. e.
In Mesh Parts toolbar, click Beam Mesher icon. Click on the line. Select Element Type as Linear. Enter Element size 10 mm. Click OK.
2a
3a
Copyright DASSAULT SYSTEMES
3c
Copyright DASSAULT SYSTEMES
3d 3b
3e 35
CATIA V5 Analysis Student Notes:
Exercise 2A (2/2) 4.
Assign physical property to beam mesh. Apply 1D Property to the beam mesh generated. a. b. c. d. e.
4a
In Model Manager toolbar, click 1D Property icon. In Type field, select Tubular Beam from dropdown. Click on the Component edition button. Enter Outside radius 40 mm and Inside radius 20 mm and click OK. Click on the OK in 1D Property Dialogue box.
4b
Copyright DASSAULT SYSTEMES
4b
Copyright DASSAULT SYSTEMES
4c
4d
4e
36
CATIA V5 Analysis
Exercise 2A: Recap
Student Notes:
Use Beam Mesher.
Copyright DASSAULT SYSTEMES
Assign 1D Property to beam mesh.
Copyright DASSAULT SYSTEMES
37
CATIA V5 Analysis
Exercise 2B
Student Notes:
Recap Exercise 15 min
In this exercise, you will perform OCTREE Triangle meshing for 2D component and assign 2D Property. Detailed instructions for this exercise are provided.
By the end of this exercise you will be able to: Use OCTREE Triangle Mesher
Copyright DASSAULT SYSTEMES
Assign 2D Property to OCTREE Triangle mesh
Copyright DASSAULT SYSTEMES
38
CATIA V5 Analysis Student Notes:
Exercise 2B (1/3) 1.
Open a part. Open 2B_Hollow_Shaft_2D_Start.CATPart.
2.
Create a Static Analysis Case. Access GPS workbench. Create a Static Analysis Case.
3.
Mesh the geometry. Mesh the surface geometry with OCTREE Triangle Mesher. a.
Copyright DASSAULT SYSTEMES
b. c. d. e. f.
In Mesh Parts toolbar, click OCTREE Triangle Mesher icon. Click on the hollow shaft surface. Enter 150 mm in Size field. Check the Absolute sag option and enter 15 mm. Check Element Type as Parabolic. Click on OK.
3b
3c
3d
Copyright DASSAULT SYSTEMES
3a
3e
Please note that, this mesh is not optimal and should only be used for preliminary analysis.
3f 39
CATIA V5 Analysis Student Notes:
Exercise 2B (2/3) 4.
Create Mesh Image. Use Mesh Visualization option to create Mesh Image. a. b. c.
4a
Right-click on the Nodes and Elements in specification tree to open contextual menu. Click on Mesh Visualization option. Click OK for the warning message to update the mesh. You will get the mesh image.
Copyright DASSAULT SYSTEMES
4b
Copyright DASSAULT SYSTEMES
4c
40
CATIA V5 Analysis Student Notes:
Exercise 2B (3/3) 5.
Assign physical property to OCTREE Triangle mesh. Apply 2D Property to the OCTREE Triangle mesh generated. a. b. c. d.
In Model Manager toolbar, click 2D Property icon. In Supports field select OCTREE Triangle Mesh.1 from Specification tree. Enter 2mm in Thickness field. Click OK.
5a
5b
Copyright DASSAULT SYSTEMES
5b
Copyright DASSAULT SYSTEMES
5c 5d
41
CATIA V5 Analysis
Exercise 2B: Recap
Student Notes:
Use OCTREE Triangle Mesher.
Copyright DASSAULT SYSTEMES
Assign 2D Property to OCTREE Triangle mesh.
Copyright DASSAULT SYSTEMES
42
CATIA V5 Analysis
Exercise 2C
Student Notes:
Recap Exercise 15 min
In this exercise, you will perform Tetrahedron meshing for 3D component and assign 3D Property. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Use Tetrahedron Mesher
Copyright DASSAULT SYSTEMES
Assign 3D Property to Tetrahedron mesh
Copyright DASSAULT SYSTEMES
43
CATIA V5 Analysis Student Notes:
Exercise 2C (1/3) 1.
Open a part. Open 2C_Hollow_Shaft_3D_Start.CATPart.
2.
Create a Static Analysis Case. Access GPS workbench. Create a Static Analysis Case.
3.
Edit the OCTREE Tetrahedron Mesh. You will find OCTREE Tetrahedron mesh is automatically applied when you switch to GPS workbench. a.
Copyright DASSAULT SYSTEMES
b. c. d. e.
3a
Double-click on OCTREE Tetrahedron Mesh.1 : Hollow_Shaft in Nodes and Elements node in the specification tree. Enter 80 mm in the Size field. Check the Absolute sag option and enter 8 mm. Check Element Type as Parabolic. Click OK.
Please note that, this mesh is not optimal and should only be used for preliminary analysis.
Copyright DASSAULT SYSTEMES
3b 3c 3d 3e
44
CATIA V5 Analysis Student Notes:
Exercise 2C (2/3) 4.
Create Mesh Image Use Mesh Visualization option to create Mesh Image. a. b. c.
4a
Right-click on the Nodes and Elements in specification tree to open contextual menu. Click on Mesh Visualization option. Click OK for the warning message to update the mesh. You will get the mesh image.
Copyright DASSAULT SYSTEMES
4b
Copyright DASSAULT SYSTEMES
4c
45
CATIA V5 Analysis Student Notes:
Exercise 2C (3/3) 5.
Assign physical property to OCTREE Tetrahedron mesh. You will find 3D Property is automatically applied to OCTREE Tetrahedron mesh when you switch to GPS workbench. a.
Copyright DASSAULT SYSTEMES
b.
Double-click on 3D Property.1 in Properties.1 node in specification tree. You can see the Part material is already assigned to mesh. Click OK.
Copyright DASSAULT SYSTEMES
4a
4b
46
CATIA V5 Analysis
Exercise 2C: Recap
Student Notes:
Use OCTREE Tetrahedron Meshing.
Copyright DASSAULT SYSTEMES
Assign 3D Property to OCTREE Tetrahedron mesh.
Copyright DASSAULT SYSTEMES
47
CATIA V5 Analysis
Step 5: Applying Restraints and Loads
Student Notes:
You will learn what are boundary conditions, different types of restraints and loads and tools to apply restraints.
What is Pre-processing Applying Material Generating Mesh Assigning Physical Property
5.
Applying Restraints and Loads
6.
Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1. 2. 3. 4.
Copyright DASSAULT SYSTEMES
48
CATIA V5 Analysis
Restraints (1/3)
Student Notes:
Restraints are used to specify support or boundary conditions for FE model. Restraints restrict displacement of supports of structure in desired direction. This is done by providing zero displacement values for specific Degrees of Freedoms of nodes present at support in FE model. CATIA provides following types toolbars for restraints : Restraints
Mechanical Restraints
Copyright DASSAULT SYSTEMES
Advanced Restraints The restraints are directly applied onto the geometry (surfaces, lines, points). The type of restraint that can be applied will depend upon the geometry selected. Degrees of Freedom (DOF) are the variables solved during analysis, which for a pure structural analysis are the nodal displacements and rotations.
Copyright DASSAULT SYSTEMES
49
CATIA V5 Analysis Student Notes:
Restraints (2/3) Restraint Type
Icon
Clamp
Surface Slider
Slider
Support Point, vertex, edge, face, virtual part
Face
Virtual part
Purpose of Restraint You will apply to surface or curve geometry support. DOFs of all nodes lying on that support are blocked.
You will apply on surface to slide along a coinciding rigid surface. Nodes on surface will have only translation DOFs parallel to coinciding rigid surface.
You will define the sliding direction. The virtual part is allowed to slide along an axis parallel to the sliding direction and passing through the fixed point.
You will allow virtual part to rotate around support point.
Copyright DASSAULT SYSTEMES
Ball Joins
Point, vertex, virtual part
Virtual parts are structures created without a geometric support. They represent bodies for which no geometry model is available, but which play a role in the structural analysis of single part or assembly systems.
Copyright DASSAULT SYSTEMES
50
CATIA V5 Analysis Student Notes:
Restraints (3/3) Restraint Type
Icon
Pivot
Sliding Pivot
User-defined Restraint
Virtual part
Virtual part
Point, vertex, edge, face, virtual part
Lines, surface, part
Purpose of Restraint You will define the pivot direction. The virtual part is allowed to rotate around an axis parallel to the pivot direction and passing through the fixed point.
You will define the sliding pivot direction. The virtual part is allowed to translate along and to rotate around an axis parallel to the sliding pivot direction and passing through the fixed point. You can fix any combination of available nodal degrees of freedom on arbitrary geometries.
You will select the support. The program automatically chooses three points and restrains some of their degrees of freedom according to the 3-2-1 rule. The resulting restraint prevents the body from rigid body translations and rotations, without over-constraining it.
Copyright DASSAULT SYSTEMES
Iso-static Restraint
Support
Copyright DASSAULT SYSTEMES
51
CATIA V5 Analysis Student Notes:
Applying Clamp Restraint You will see how to apply clamp restraint. 1. 2. 3.
In Restraint toolbar, click Clamp icon. Select the required surface to clamp in Supports field. Click OK.
1
Copyright DASSAULT SYSTEMES
2
Copyright DASSAULT SYSTEMES
2 3
52
CATIA V5 Analysis
Loads (1/3)
Student Notes:
Loads are inputs to the system. The purpose of FEA is to study behavior of the structure to the input loads. They can be in the forms of forces, moments, pressures, temperature, accelerations. CATIA provides following types of loads which can be applied on the structure. Pressure Body Motion Forces Force Densities
Copyright DASSAULT SYSTEMES
Enforced Displacements Assembled Loads The loads are directly applied onto the geometry (surfaces, lines, points). The type of load that can be applied will depend upon the geometry selected.
Copyright DASSAULT SYSTEMES
53
CATIA V5 Analysis Student Notes:
Loads (2/3) Load Type
Icon
Support Face
Description The force direction is everywhere normal to the surface.
Pressure
N/m2
Acceleration
N/Kg or m/s2
Body 1D, Body 2D, Body 3D, Mesh Part, Virtual part
It represents mass body force fields of uniform magnitude applied to parts.
Angular Vel. in rad/s Angular Accl. in rad/s2
Body 1D, Body 2D, Body 3D, Mesh Part, Virtual part
It represents mass body force fields induced by rotational motion applied to parts.
Point, Vertex, Edge, Face, Virtual part
It represents force system statically equivalent to a given pure force resultant at a given point.
Rotation Force
Distributed Force
Moment
Copyright DASSAULT SYSTEMES
Units (SI)
N
Nm
Point, Vertex, Edge, Face, Virtual part
It represents force systems statically equivalent to a given pure couple (single moment resultant).
The distributed force applied directly to the nodes of the selected entity (In the distribution, all the nodes are equally taken into account) whereas the pressure and the surface force density applies to the element face of the selected entity. So the later types of load are more accurate.
Copyright DASSAULT SYSTEMES
54
CATIA V5 Analysis Student Notes:
Loads (3/3) Load Type
Icon
Line Force Density
Surface Force Density
Copyright DASSAULT SYSTEMES
Volume Force Density
Unit N/m
N/m2
N/m3
Force Density
N
Enforced Displacements
Translation in mm Rotation in deg
Assembled Load
Copyright DASSAULT SYSTEMES
-
Support
Description
Edge
It represents line traction fields of uniform magnitude applied to curve geometries.
Face
It represents surface traction fields of uniform magnitude applied to surface geometries.
Body 3D, Mesh part
It represents volume body force fields of uniform magnitude applied to parts.
Point, Vertex, Face, Body
It helps to create the equivalent of the existing line force density, surface force density and body force by giving only as input a force in Newton.
Restraint
-
It assigns non-zero displacement values in previously restrained directions. Assembled Load is defined in an assembled analysis and therefore applied on the assembled mesh. This load is concatenation of several loads defined in sub analysis.
55
CATIA V5 Analysis Student Notes:
Applying Pressure Loads You will see how to apply Pressure load. 1. 2. 3. 4.
In Loads toolbar, click Pressure icon. Click on the required surface as a support in the Supports field. Enter value 1N_m2 in Pressure field. Click OK.
1
2
Copyright DASSAULT SYSTEMES
2
Copyright DASSAULT SYSTEMES
3 4
56
CATIA V5 Analysis Student Notes:
Applying Distributed Force You will see how to apply Distributed Force. 1. 2. 3. 4. 5.
In Forces toolbar, click Distributed Force icon. Click on the required surface as a support in the Supports field. Enter the force value 1N in Y field of Force Vector. Select the Handler point as shown in required. Click OK.
1
4 2
Copyright DASSAULT SYSTEMES
2
Copyright DASSAULT SYSTEMES
3 4 5
57
CATIA V5 Analysis
Step 6: Checking the Finite Element Model
Student Notes:
You will learn the tool to validate the created FE model.
What is Pre-processing Applying Material Generating Mesh Assigning Physical Property Applying Restraints and Loads
6.
Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
1. 2. 3. 4. 5.
Copyright DASSAULT SYSTEMES
58
CATIA V5 Analysis Student Notes:
Finite Element Model Check (1/2) Model Check allows you to verify all pre-processing steps done and model is ready for computation. This provides common platform where you can check all pre-processing data. If any information is missing, it shows status KO against that row and provides related error message. Each Tab in Model Checker provides following information:
Status : OK
green
KO
red
Bodies Tab
Copyright DASSAULT SYSTEMES
Missing Mesh Missing Properties Missing Material Missing Support Diagnosis Problems
Copyright DASSAULT SYSTEMES
59
CATIA V5 Analysis
Finite Element Model Check (2/2)
Student Notes:
Connections Tab Kind of Constraints Part involved Connection Properties Connection Status
Copyright DASSAULT SYSTEMES
Others Tab Loads Restraints Virtual Parts
Copyright DASSAULT SYSTEMES
60
CATIA V5 Analysis
To Sum Up
Student Notes:
Copyright DASSAULT SYSTEMES
In the following slides you will find a summary of the topics covered in this lesson.
Copyright DASSAULT SYSTEMES
61
CATIA V5 Analysis
What is Pre-processing
Student Notes:
Pre-processing involves all the steps which are required to covert a given physical problem into an equivalent Finite Element problem. This involves following steps: 1. 2. 3. 4. 5. 6.
Applying material structural property to a part Meshing the part using elements and nodes Applying physical property to the mesh Applying restraints to the mesh Applying loads to the mesh Model checking to validate that all the pre-processing steps are done.
Applying Material
Copyright DASSAULT SYSTEMES
Structural properties are required to calculate the deformation, strains and stresses. You can apply material by selecting it from the default material catalog. You may need to create the material with specified properties, which is not available in the standard material catalog. In this case, you can use User Material option to create the material with your own specification.
Copyright DASSAULT SYSTEMES
62
CATIA V5 Analysis Student Notes:
Generating Mesh Meshing involves approximating actual physical structure into Finite Element Model using several simple geometric shapes called elements. Mesh is representation of the mathematical idealization of the structure. On the basis of dimensionality, elements can be classified as 1D, 2D, and 3D elements. According to the order of the displacement equation, elements can be classified as Linear and Higher order elements. You can use Beam Mesher, OCTREE Triangle Mesher, and OCTREE Tetrahedron Mesher to mesh wireframes, surfaces, and solids respectively.
Copyright DASSAULT SYSTEMES
Assigning Physical Property In CATIA, physical property means cross-section, thickness, and material properties. It uses geometry of the mesh or mesh part as support to apply Physical Property. You can also apply physical property directly to orphan meshes. The physical property to be attached depends on the mesh used to create FE model as shown in the table.
Copyright DASSAULT SYSTEMES
Mesh Type
Physical Property Name
Beam
1D Property
OCTREE Triangle
OCTREE Tetrahedron
2D Property
3D Property
Physical Property Assigned to Mesh 1. 2.
Cross-section Material
1. 2.
Thickness Material
1.
Material
63
CATIA V5 Analysis Student Notes:
Applying Restraints and Loads The restraints are used to specify the support or boundary conditions for FE model. Restraints restrict the displacement of supports of the structure in required direction, by providing zero displacement values for specific Degrees of Freedoms at nodes present at support in FE model. Loads are inputs to the system. They can be form of forces, moments, pressures, temperatures, accelerations, etc. The loads are directly applied onto the geometry (surfaces, lines, points). The type of load that can be applied will depend upon the geometry selected.
Checking the Finite Element Model
Copyright DASSAULT SYSTEMES
Model Check allows you to verify that all pre-processing steps are completed. If any information is missing, it shows status KO against that row and provides related error message. Model Checker contains following 3 tabs.
Status: OK
Green
KO
Red
Bodies Connections Others
Copyright DASSAULT SYSTEMES
64
CATIA V5 Analysis Student Notes:
Main Tools Material 1
Apply Material: Lets you apply the material directly from the default Material catalog.
1
Mesh Parts 2
Beam Mesher: Lets you create 1-D element mesh.
3
OCTREE Triangle Mesher: Lets you create 2D triangular element mesh.
4
OCTREE Tetrahedron Mesher: Lets you create 3D tetrahedron element mesh.
4 3 2
Model Manager 5
Copyright DASSAULT SYSTEMES
6
1D Property: offers you a set of standard crosssections and material to be associated to the beam mesh. 2D Property: Lets you to associate thickness and material to the OCTREE Triangle mesh.
7
3D Property: Lets you to assign material to be associated to the OCTREE Tetrahedron mesh.
8
User Material: Lets you create your own user-defined material with required properties.
Copyright DASSAULT SYSTEMES
7 6 5 8
65
CATIA V5 Analysis
Exercise 2D
Student Notes:
Recap Exercise 15 min
In this exercise, you will apply boundary conditions, load and check the FE model for 1D mesh. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Apply Clamp Restraint Apply Distributed Force
Copyright DASSAULT SYSTEMES
Use Model Checker tool
Copyright DASSAULT SYSTEMES
66
CATIA V5 Analysis Student Notes:
Exercise 2D (1/4) 1.
Apply Boundary Conditions. Open 2D_Hollow_Shaft_1D_Start.CATAnalysis Apply Clamp Restraint. a. b.
Copyright DASSAULT SYSTEMES
c.
In Restraint toolbar, click Clamp icon Select the vertex to clamp in Supports field. Click OK.
1a
1b
Please note that, the support for Clamp in this case should be vertex and not point.
Copyright DASSAULT SYSTEMES
1c
67
CATIA V5 Analysis Student Notes:
Exercise 2D (2/4) 2.
Apply Load. Apply Distributed Force. a. b. c.
In Forces toolbar, click Distributed Force icon. Click on the vertex as a support in the Supports field. Select Type in Axis System as User from dropdown list.
2a
2c
Copyright DASSAULT SYSTEMES
2b
Copyright DASSAULT SYSTEMES
68
CATIA V5 Analysis Student Notes:
Exercise 2D (3/4) d.
e. f.
In Current axis field select Axis_System_User_Defined.1 from the specification tree. Enter the force value 1N in Z field of Force Vector. Click OK.
2d
Copyright DASSAULT SYSTEMES
2d
Copyright DASSAULT SYSTEMES
2e 2f
69
CATIA V5 Analysis Student Notes:
Exercise 2D (4/4) 3.
Check the FE Model. Use Model check tool to check model inconsistency. a. b.
c.
In Model Manager toolbar, click Model Checker icon. Check for the green signal and message that The whole model is consistent. Click OK.
3a
3b
Copyright DASSAULT SYSTEMES
Please note that, if the signal is Red, it means that model is not consistent. In this case, you will get ‘KO’ in ‘Status’ column in ‘Body’ tab.
Copyright DASSAULT SYSTEMES
3c
70
CATIA V5 Analysis
Exercise 2D: Recap
Student Notes:
Apply Clamp Restraint. Apply Distributed Force.
Copyright DASSAULT SYSTEMES
Use Model Checker tool.
Copyright DASSAULT SYSTEMES
71
CATIA V5 Analysis
Exercise 2E
Student Notes:
Recap Exercise 15 min
In this exercise, you will apply boundary conditions, load and check the FE model for 2D mesh. High-level instructions are provided for this exercise. By the end of this exercise you will be able to: Apply Clamp Restraint Apply Distributed Force
Copyright DASSAULT SYSTEMES
Use Model Checker tool
Copyright DASSAULT SYSTEMES
72
CATIA V5 Analysis Student Notes:
Exercise 2E (1/3) 1.
Apply Boundary Conditions. Open 2E_Hollow_Shaft_2D_Start.CATAnalysis Apply Clamp Restraint. Select Edge shown as support for clamp.
Copyright DASSAULT SYSTEMES
Edge to be Clamped
Copyright DASSAULT SYSTEMES
73
CATIA V5 Analysis Student Notes:
Exercise 2E (2/3) 2.
Applying Load. Apply Distributed Force. Select the edge shown as support. Select User-defined Axis System. Enter 1N force in Z field as shown.
Copyright DASSAULT SYSTEMES
Edge to be selected to apply Distributed force
Copyright DASSAULT SYSTEMES
User-defined Axis system to be selected
74
CATIA V5 Analysis
Exercise 2E (3/3) Checking the FE Model. Use Model checker tool to check model inconsistency.
4.
View Mesh Image. Activate the Mesh Image by double-click on Mesh image in specification tree.
Copyright DASSAULT SYSTEMES
3.
Student Notes:
Copyright DASSAULT SYSTEMES
75
CATIA V5 Analysis
Exercise 2E: Recap
Student Notes:
Apply Clamp Restraint. Apply Distributed Force.
Copyright DASSAULT SYSTEMES
Use Model Checker tool.
Copyright DASSAULT SYSTEMES
76
CATIA V5 Analysis
Exercise 2F
Student Notes:
Recap Exercise 15 min
In this exercise, you will apply boundary conditions, load and check the FE model for 3D mesh. High-level instructions are provided for this exercise. By the end of this exercise you will be able to: Apply Clamp Restraint Apply Pressure
Copyright DASSAULT SYSTEMES
Use Model Checker tool
Copyright DASSAULT SYSTEMES
77
CATIA V5 Analysis Student Notes:
Exercise 2F (1/3) 1.
Apply Boundary Conditions. Open 2F_Hollow_Shaft_3D_Start.CA TAnalysis Apply Clamp Restraint. Select the face of hollow shaft shown as support for clamp.
Local Axis System
Copyright DASSAULT SYSTEMES
Face to be Clamped
Copyright DASSAULT SYSTEMES
78
CATIA V5 Analysis Student Notes:
Exercise 2F (2/3) 2.
Applying Load. Apply Pressure. Select the surface shown as support. Enter -1N_m2 in Pressure field as shown.
Copyright DASSAULT SYSTEMES
Surface to be selected to apply Pressure
Copyright DASSAULT SYSTEMES
79
CATIA V5 Analysis
Exercise 2F (3/3) Checking the FE Model. Use Model checker tool to check model inconsistency.
4.
View Mesh Image. Activate the Mesh Image by double-click on Mesh image in the specification tree.
Copyright DASSAULT SYSTEMES
3.
Student Notes:
Copyright DASSAULT SYSTEMES
80
CATIA V5 Analysis
Exercise 2F: Recap
Student Notes:
Apply Clamp Restraint. Apply Distributed Force.
Copyright DASSAULT SYSTEMES
Use Model Checker tool.
Copyright DASSAULT SYSTEMES
81
CATIA V5 Analysis
Case Study: FE Modeling of Drill Press Table
Student Notes:
Recap Exercise 30 min
Copyright DASSAULT SYSTEMES
You will practice what you learned, by completing the case study model. In this exercise, you will create FE model for Drill Press Table. Recall the design intent of this model: Understand the structural properties of Drill Press Table. Check for standard material with these properties in material catalogue or create new User material. Decide the mesh (1D, 2D or 3D) to be used to map actual problem into FE model. As per the geometry dimensions use appropriate Mesher. Understand and assign the physical property to the created mesh part. Understand and apply the restraints (boundary conditions) on the mesh part. Understand and apply the forces acting on the Drill Press Table. Check the created FE model.
Copyright DASSAULT SYSTEMES
82
CATIA V5 Analysis Student Notes:
Case Study: Introduction
Copyright DASSAULT SYSTEMES
The case study for this lesson is the Drill Press Table. The focus of this case study is to create a Finite Element model for Drill Press Table. You will perform following steps independently in order to achieve this. 1. Create and apply specified Material. 2. Decide and create relevant mesh. 3. Decide and assign corresponding physical property. 4. Decide and apply boundary conditions. 5. Decide the loading conditions and apply load. 6. Check the FE model. You will understand the actual physical problem and use this information to perform above steps to create FE model.
Drill press Table Component
Copyright DASSAULT SYSTEMES
Drill press Table FE Model
83
CATIA V5 Analysis Student Notes:
Design Intent (1/4) You will now understand the physical problem. The figure shows the drill press assembly. You can see, while drilling operation, the Drill Press Table is fixed to the stand as shown in fig. The workpiece is located firmly on the table with clamps in order to get drilled. Understand the structural properties of Drill Press Table. The table of drill press is composed of steel having following properties. The material is an isotropic material. Young's Modulus = 2.1e+011 N_m2.
Drill Press Table fixed to stand
Poisson's Ratio = 0.268. Density = 7862 kg/m3.
Stand
Thermal Expansion = 1.19e-005 /Kdeg.
Copyright DASSAULT SYSTEMES
Yield Strength = 2.6e+008 N_m2. Check for the standard material with these properties in material catalogue or create new material with User Material and edit properties.
Copyright DASSAULT SYSTEMES
84
CATIA V5 Analysis Student Notes:
Design Intent (2/4) Decide the mesh (1D, 2D or 3D) to be used to map actual problem into FE model. In this case, it is not possible to use beam FE model. The surface FE model will take more efforts to covert part model to surface model and may oversimplify the geometry by removing stiffeners. You can directly model this part as 3D mesh to take advantage of existing part model.
Mesh generated
Use OCTREE Tetrahedron mesh Understand the physical property to be applied on the mesh parts: The type of physical property to be applied depends on the type of mesh used.
Clamp applied
Copyright DASSAULT SYSTEMES
If Part model is 3D Geometry, the OCTREE Tetrahedron mesh and 3D Property is automatically applied when you switch to GPS workbench. Understand the restraints (boundary conditions) on the parts: As the Table is fixed to the stand, it means that the surface of table which is in contact with stand surface will not deform. It means all DOFs are fixed for this surface of table. Thus, you can apply Clamp restraint for this surface.
Copyright DASSAULT SYSTEMES
85
CATIA V5 Analysis Student Notes:
Design Intent (3/4) Understand the forces acting on the Drill Press Table. Now you will study the forces acting on the table. The torque applied by the electric motor is transmitted to table through drill-bit and workpiece. The drill press operator applies downward force of 10 N to move drill in vertically downward direction. This force will be transmitted to table through drill-bit and workpiece. The torque and downward force will be transmitted to table through bottom surface of workpiece. You can assume both forces remain constant with respect to time. As the applied loads are stationary with time, you will perform Static Analysis. For the purpose of simplicity you will neglect Torque and you will perform the analysis assuming only downward force acting on the table.
Pressure is applied only on the green area
Use Static Analysis Case
Copyright DASSAULT SYSTEMES
The downward force can be approximated as pressure on the area equal to bottom of workpiece.
Copyright DASSAULT SYSTEMES
86
CATIA V5 Analysis Student Notes:
Design Intent (4/4) Validate the FE model created. It is necessary to check the FE model to ensure that all steps required to perform computation are done. Use Model Check tool.
Copyright DASSAULT SYSTEMES
You can summarize the pre-processing information received from the above study: Now you can map this pre-processing information into FE Model in CATIA.
Copyright DASSAULT SYSTEMES
Drill press Table FE Model
87
CATIA V5 Analysis
Do It Yourself : FE Modeling of Drill Press Table
Student Notes:
The following steps offer hints to guide you through the creation of FE model for Drill Press Table. 1.
Open the given part Drill_Press_Table_Start model. Switch to GPS workbench. Browse through the files and open the model ‘Drill_Press_Table_Start .CATPart
2.
Create User Material. Create a User Material steel and edit its structural properties for material specifications provided. Name the Material as Modified_Steel.
Copyright DASSAULT SYSTEMES
3.
Edit OCTREE Tetrahedron Mesh. Keep the default mesh size and sag values as 10% of mesh size. Generate Mesh Visualization.
Copyright DASSAULT SYSTEMES
88
CATIA V5 Analysis Student Notes:
Do It Yourself : FE Modeling of Drill Press Table 4.
Edit 3D Property. Select the Modified_Steel in property.
5.
Apply Boundary Conditions. Apply Clamp Restraint to the surfaces shown.
6.
Clamp applied
Apply Loads.
Copyright DASSAULT SYSTEMES
You have to apply 10 N Load as pressure on selected area shown. Measure the surface area and calculate the pressure value. Pressure applied
7.
Check the Model. Check the model for consistency.
Copyright DASSAULT SYSTEMES
89
CATIA V5 Analysis
Case Study: FE Modeling of Drill Press Table Recap
Student Notes:
Understand the structural properties of Drill Press Table. Check for standard material with these properties in material catalogue or create new material. Decide the mesh (1D, 2D or 3D) to be used to map actual problem into FE model. As per the geometry dimensions use appropriate Mesher. Understand and assign the physical property to be applied on the created mesh part.
Copyright DASSAULT SYSTEMES
Understand and apply the restraints (boundary conditions) to be applied on the mesh part. Understand and apply the forces acting on the Drill Press Table. Check the created FE model.
Copyright DASSAULT SYSTEMES
90
