Essay: STATIC AND MODAL ANALYSIS OF REAR DOOR OF A PASSENGER CAR USING FEM

Key Words: Car Door, CAE, Hypermesh, NASTRAN
Project Area: Finite element analysis
Abstract: When performing the structure-borne road and engine vibration simulations on vehicle system models, the doors play an important part. They not only determine the general guidelines of car style, but also are vital for passenger’s safety. This accentuates the necessity of good predictive performance of door models, including attachment points, when performing vehicle system simulations. Present work focuses on improving the static and dynamic behavior of the rear door by interpreting the results obtained from the modal analysis and static stiffness analysis of the same. First, the car door three-dimensional model was established in the CATIA, then it was imported into the preprocessor tool Hypermesh to model the geometry, at last, imported into the analysis tool Nastran, and the related settings were made to calculate 15 modal frequencies of the door. Hyperview is used as a postprocessor tool to preview the results.
LIST OF TABLES
TABLE 1. ELEMENT QUALITY CRITERIA 16
TABLE 2 FEA MODEL ENTITIES 18
TABLE 3 FRAME STIFFNESS LOADS AND BOUNDARY CONDITION 26
TABLE 4 OVERALL STIFFNESS LOADS AND BOUNDARY CONDITIONS 28
TABLE 5 TORSIONAL RIGIDITY STIFFNESS LOADS AND BOUNDARY CONDITIONS 30
TABLE 6 BELTLINE STIFFNESS LOADS AN BOUNDARY CONDITION 32
LIST OF FIGURES
FIGURE 1 TATA TECHNOLOGIES LTD. HISTORY 1
FIGURE 2 METHODOLOGY 5
FIGURE 3 FEA STEPS 7
FIGURE 4 PRE-PROCESSING 10
FIGURE 5 ELEMENT TERMINOLOGY 10
FIGURE 6 ROD ELEMENT 11
FIGURE 7 BEAM ELEMENT 11
FIGURE 8 2D ELEMENTS 11
FIGURE 9 3D ELEMENTS 12
FIGURE 10 MESHING IN CRITICAL AREA 13
FIGURE 11 WARPAGE OF AN ELEMENT 14
FIGURE 12 ASPECT RATIO OF AN ELEMENT 14
FIGURE 13 SKEWNESS OF AN ELEMENT 15
FIGURE 14 TYPE OF CONNECTIONS 16
FIGURE 15 REAR DOOR ASSEMBLY 18
FIGURE 16 INNER PANEL 19
FIGURE 17 OUTER PANEL 19
FIGURE 18 LATCH REINFORCEMENT 19
FIGURE 19 INTRUSION BAR BRACKET 19
FIGURE 20 INTRUSION BAR 20
FIGURE 21 OUTER WAISTLINE REINFORCEMENT 20
FIGURE 22 INNER WAISTLINE REINFORCEMENT 20
FIGURE 23 BODY SIDE HINGE 20
FIGURE 24 DOOR SIDE HINGE 20
FIGURE 25 HINGE REINFORCEMENT 21
FIGURE 26 BOUNDARY CONSTRAINTS FOR MODAL ANALYSIS 23
FIGURE 27 FIRST FOUR MODE SHAPES 24
FIGURE 28 FRAME STIFFNESS LOADS AND BOUNDARY CONDITION 26
FIGURE 29 FRAME FRONT DISPLACEMENT IN HYPERVIEW 27
FIGURE 30 FRAME REAR DISPLACEMENTS IN HYPERVIEW 27
FIGURE 31 OVERALL STIFFNESS LOADS AND BOUNDARY CONDITIONS 28
FIGURE 32 DISPLACEMENT RESULTS IN HYPERVIEW 29
FIGURE 33 TORSIONAL RIGIDITY STIFFNESS LOADS AND BOUNDARY CONDITIONS 30
FIGURE 34 TORSION RIGIDITY DISPLACEMENT IN HYPERVIEW 31
FIGURE 35 TORSION RIGIDITY BOTTOM DISPLACEMENT IN HYPERVIEW 31
FIGURE 36 BELTLINE STIFFNESS LOADS AN BOUNDARY CONDITION 32
FIGURE 37 INNER BELTLINE DISPLACEMENT IN HYPERVIEW 33
FIGURE 38 OUTER BELTLINE DISPLACEMENT IN HYPERVIEW 33
TABLE OF CONENTS
RESPONSE OPTION SHEET III
ABSTRACT SHEET IV
ACKNOWLEDGEMENT V
LIST OF TABLES VI
LIST OF FIGURES VII
1. ABOUT TATA TECHNOLOGIES LIMITED. 1
2. INTRODUCTION 3
2.1. BACKGROUND 3
2.2. OBJECTIVE 4
3. METHODOLOGY 5
4. FINITE ELEMENT ANALYSIS 7
4.1. BRIEF HISTORY: 7
4.2. THREE STEPS OF FEA: 7
4.3. COMMON APPLICATIONS: 8
5. IMPORTING AND REPAIRING CAD 9
6. PREPROCESSING 10
6.1. TERMINOLOGY: 10
6.2. ELEMENT TYPES: 11
6.2.1. 1-D elements: 11
6.2.2 2-D Elements: 11
6.2.3. 3-D Element: 12
6.3. ELEMENT QUALITY AND CHECKS: 13
6.3. CONNECTORS: 16
6.4. LOADING POINTS, MATERIALS AND PROPERTIES: 17
6.5. CONSTRAINTS: 17
7. REAR DOOR ASSEMBLY 18
7.1. COMPONENT STATISTICS AND MATERIAL PROPERTIES 19
8. SOLUTION AND POST PROCESSING 22
8.1. MODAL ANALYSIS: 22
8.2. STATIC ANALYSIS: 25
8.2.1. Frame Front and Rear stiffness: 26
8.2.2. Overall Stiffness: 28
8.2.3. Torsional Rigidity Top and Bottom Stiffness: 30
8.2.4. Inner and Outer Beltline Stiffness: 32
9. CONCLUSION AND RECOMMENDATIONS 35
10. REFERENCES 36
1. ABOUT TATA TECHNOLOGIES LIMITED.
Tata Technologies Ltd. (TTL) is a global engineering consulting organization with core specialization in automotive and aerospace. The company delivers customized solutions for engineering and design, product life cycle management and enterprise system integration for the manufacturing sector. TTL is a company of engineers, led by engineers, with more than 6,300 associates, representing 27 nationalities.
Figure 1 Tata Technologies Ltd. History
Founded in 1989, the company has been helping ambitious manufacturers create great products for over 20 years. It focuses on the manufacturing industry – on companies that make exciting products – covering every aspect of the value chain from concept to recycling. It also supports these clients through a comprehensive, integrated set of engineering services and IT processes and tools to manage the product development process and the complete manufacturing ecosystem.
Location:
TTL’s international headquarters is in Singapore, with key regional headquarters in India (Pune), USA (Novi, Michigan) and the UK (Luton). The company has global development centres in Germany, India, Thailand, the UK and the USA and also has offices in Canada, China, France, Germany, Ireland, Japan, Korea, Mexico, and the Netherlands.
Areas of business:
The TTL group offers solutions and services in:
• Engineering and design: Working with the world’s leading automotive and aerospace organizations leveraging global resources to provide engineering services wherever their clients need them to be.
• Product lifecycle management: Helping companies build better products, define better processes and reduce costs along the way. Includes branded products from Autodesk, Siemens, Dassault Systemés as well as training and support.
• Product development IT: Implementing best practice enterprise solutions that coordinate people, technology, information, and processes specific to product development organizations. Includes CRM, ERP, application lifecycle management, information lifecycle management.
• Manufacturing: Delivering a powerful combination of cutting-edge digital manufacturing, manufacturing automation and control systems, and comprehensive manufacturing domain expertise.
• Knowledge Lifecycle Management: Helping to harvest institutional knowledge, especially with iGET IT®, the comprehensive engineering internet-based training system.
Joint ventures, subsidiaries, associates:
• Tata HAL Technologies: Tata Technologies and Hindustan Aeronautics (HAL), Asia’s premier aerospace manufacturer, merge their formidable engineering, design and manufacturing resources and market reach to provide clients with comprehensive “design through build” aerospace solutions. This joint venture is India’s only dedicated aero structure provider that offers access to HAL’s design and manufacturing facilities and Tata Technologies’ global delivery centres.
Clients:
TTL serves clients in 25 countries, with a delivery model specifically designed for engineering and IT engagements that offers a unique blend of deep, local expertise integrated with our six global delivery centres, Pune-Hinjawadi (India), Bangalore (India), Detroit (USA), Coventry (UK), Stuttgart (Germany), and Bangkok (Thailand).
2. INTRODUCTION
The production of new vehicle is a resource consuming process. In an increasing pace of development and constant demands of cost reduction, the building of prototypes is considered too expensive. However, the vehicle performance still need to be evaluated before the vehicles reach the market. Hence, with increasing computational power, simulation models seem a natural successor to conventional prototypes. In this present work, Static and Dynamic load characteristics of the rear door will be calculated and analysed using several finite element analysis commercial software such as Hypermesh, Nastran & Hyperview. The structural problems discovered by this analysis will be modified if required.
2.1. Background
Under the action of the engine, the road, and various vibration excitation sources, the body structure vibrates. If the frequency of this vibration source is similar to the natural frequency of the body member, it leads to its structural resonance, wherein the amplitude of the vibration increases drastically and could lead to its failure. Hence, modal analysis of the assembly is of great importance. It helps to find the natural frequencies of all the members in the body and analyzing which, we can avoid the occurrence of the resonance.
When performing the structure-borne road and engine vibration simulations on vehicle system models, the doors play an important part. They not only determine the general guidelines of car style, but also are vital for passenger’s safety from side crashes. The doors are fixed to the vehicle structure through hinges, a lock mechanism and door seals. This gives the door some freedom of motion and since the doors comprise large surfaces, this motion has great impact on the air pressure in the compartment. This accentuates the necessity of good predictive performance of door models, including attachment points, when performing vehicle system simulations.
An effective and comfortable approach to analyze structural dynamics is to work under steady-state conditions in the frequency domain. The models considered here are used in Eigen modes and frequency response simulations.
2.2. Objective
The objectives of this project are:
1. To analyse the natural frequency of the door and consequently avoid resonance with the other vibration sources in the vehicle structure.
2. To obtain the displacements and stresses at critical locations in various components of the door assembly.
3. To calculate and analyse the following stiffness values:
a. Door Frame front and rear stiffness
b. Torsional Rigidity bottom and top stiffness
c. Inner and outer beltline stiffness
d. Overall Stiffness
4. To improve the static and dynamic behavior of the rear door by changing the geometrical dimension and/or structural properties based on the results of the analysis.
3. METHODOLOGY
Following Methodology is adopted for the completion of this project:
• Specifying Geometry- The geometry to be analyzed imported from a solid modeler CATIA.
• Modeling the Geometry-The geometry is modeled into small elements. This involves defining the types of elements into which the structure will be broken, as well as specifying how the structure will be subdivided into elements.
• Specifying Element Type and Material Properties- The material properties are defined. In an elastic analysis of an isotropic solid these consist of the Young’s modulus, density and Poisson’s ratio of the material.
• Applying Boundary conditions and External Loads- The boundary conditions e.g. location of supports and the external loads are specified.
Figure 2 Methodology
• Generating a solution- The solution is generated based on the previously input parameters.
• Post processing- Based on the initial conditions and applied loads, data is returned after a solution is processed. This data can be viewed in a Hyperview.
• Refining the Mesh- Finite element methods are approximate methods and, in general, the accuracy of the approximation increases with the number of elements used. The number of elements needed for an accurate model depends on the Problem and the specific results to be extracted from it. Thus, in order to judge the number of elements in the object and see if or how the results change.
• Interpreting Results- This step is perhaps the most critical step in the entire Knowledge of mechanics to interpret and understand the output of the model. This is critical for applying correct results to solve real engineering problems and in identifying when modeling mistakes have been made.
4. FINITE ELEMENT ANALYSIS
The finite element Analysis (FEA) is a numerical technique for finding approximate solutions to boundary value problems for partial differential equations. Useful for problems with complicated geometries, loadings, and material properties where analytical solutions cannot be obtained.
4.1. Brief History:
• Grew out of aerospace industry
• Post-WW II jets, missiles, space flight
• Need for light weight structures
• Required accurate stress analysis
• Paralleled growth of computers
FEA includes subdivision of a large problem into smaller, simpler, parts. The simple equations that model these finite elements are then assembled into a larger system of equations that models the entire problem.
4.2. Three Steps of FEA:
FEA is performed in three stages, Pre-Processing (Finite Element Modelling), Solving and Post Processing and those are outlined below.
Figure 3 FEA steps
1. Preprocessing:
• Define the geometric domain of the problem.
• Define the element type(s) to be used.
• Assign the material properties to components .
• Define the connections (Spot weld,bolt etc).
• Apply Load and the physical constraints (boundary conditions).
2. Solution:
• computes the unknown values of the primary field variable(s). Computed values are then used by back substitution to compute additional, derived variables, such as reaction forces, element stresses.
3. Postprocessor:
• Postprocessor software contains sophisticated routines used for sorting, printing, and plotting selected results from a finite element solution.
4.3. Common Applications:
• Mechanical/Aerospace/Civil/Automotive
• Engineering
• Structural/Stress Analysis
• Static/Dynamic
• Linear/Nonlinear
• Fluid Flow
• Heat Transfer
• Electromagnetic Fields
• Soil Mechanics
• Acoustics
• Biomechanics
5. IMPORTING AND REPAIRING CAD
Prior to Pre-processing, the geometry to be modeled is imported into the Modeling Software and the geometric issues, if any, are repaired. While the importation of data generally occurs with little error, there are variety of tools to remedy these geometric issues, if any. There are many features on a part that are not critical to the structure of the part and have little or no effect on the analysis. These features can include
• Lightening Holes – For part weight reduction
• Edge Fillets – For reduction of sharp corners allowing safer part handling
• Surface Fillets – To meet manufacturing requirements
• Free edges
• Scar lines
• Duplicate surfaces
• Intersection of parts (assembly of components)
These features often are process driven and are not function critical.
6. PREPROCESSING
Any continuous object has infinite degrees of freedom and it’s just not possible to solve the problem in this format. Preprocessing (Meshing) is the act of preparing a model for analysis. Complex geometry is broken down into simple shapes (elements). The basic idea is to make calculations at only limited (Finite) number of points and then interpolate the results for the entire domain (surface or volume). The part is meshed and then definitions for the type and thickness of the material(s) are added then forces and constraints are applied.
Figure 4 Pre-processing
6.1. Terminology:
• Element: control volume into which geometry is discretized.
• Node: A node represents a physical position on the structure being modelled and is used by an element entity to define the location and shape of that element
• Face: boundary of an element.
• Edge: boundary of a face.
Figure 5 Element Terminology
• DOF: The minimum number of parameters (motion, coordinates, temp. etc.) required to define the position of any entity completely in the space is known as a degree of freedom (dof).
6.2. Element Types:
Finite element modelling mainly involves the discretization of the structure into elements or domains that are defined by nodes which describe the elements. Element selection is based on the type of problem, boundary conditions, geometry considerations, and results required.
6.2.1. 1-D elements: Used for geometries having one of the dimensions that is very large in comparison to the other two. The shape of the 1-D element is a line.
Figure 6 Rod Element
Figure 7 Beam Element
Practical Examples: Long shaft, rod, beam, column, spot welding, bolted joints, pin joints, bearing modeling, etc.
6.2.2 2-D Elements: 2-D elements represent 3-D space by assuming an infinite depth, fixed depth, or axisymmetric geometry. They have a reduced stiffness matrix and therefore reduced solution time with no loss in accuracy if the assumptions for the element hold.
Figure 8 2D Elements
Practical Examples: All sheet metal parts, plastic components like instrument panels, etc. In general, 2-D meshing is used for parts having a width / thickness ratio > 20.
Limitations of mid surface and 2-D meshing: 2-D meshing would lead to a higher approximation if-
o used for variable part thickness
o surfaces are not planar and have different features on two sides.
6.2.3. 3-D Element: Solid elements are generally used for 3-D structures not fitting into the shell description. Castings, forgings, blocky structures, and volumes are all good examples of 3-D solid element structures. Solid elements have the benefit of eliminating many assumptions found in the other element types but are generally more difficult to model.
Figure 9 3D Elements
Practical Examples : Transmission casing, clutch housing, engine block, connecting rod, crank shaft etc
In this project work, 2D meshing has been used with shell element. Shells are essentially 2-D elements that represent 3-D space. Shell elements has 6 degree of freedom and are 4 noded and 8 noded elements. Shells are excellent for thin 3-D structures, such as body panels, sheet metal, injection molded plastic or any part that can be described as having a thickness that is small relative to its global dimensions. Deflections are given at the nodes, but stresses can be found at the upper and lower surfaces as well as at the midplane
Some points to be noted:
• Meshing with more element can give higher accuracy. The downside is increased memory and CPU time.
• Greater the number of elements in the critical region (i.e. hole), the better is its accuracy. Critical areas are locations where high stress locations will occur. Dense meshing and structured mesh (no trias / pentas) is recommended in these regions. Areas away from the critical area are general areas. Geometry simplification and coarse mesh in general areas are recommended (to reduce the total DOFs and solution time).
Figure 10 Meshing in Critical Area
• Even without increasing the number of elements, one can achieve a better result just by the appropriate arrangement of the nodes and elements. This is known as biasing. Tria elements help in creating a smooth mesh transition from a dense mesh to a coarse mesh.
6.3. Element Quality and Checks:
Quality check list concerning the various mesh quality parameters like skew, aspect ratio, Jacobian etc. are the measures of how far a given element deviates from ideal shape. Some of the qualities checks are based on angles (like skew, included angles) while others on side ratios & area (like aspect, stretch). The following checks are done on the elements before proceeding to analysis:
• Connectivity test of a group of elements.
• Duplicate elements.
• Free 1-d: Test for free ends in one-dimensional elements.
• Free edges: Free edges should match with the geometry outer edges / free edges. Any additional free edges are an indication of unconnected nodes.
• Shell Normal: The shell normal is the direction of the normals of the shell element s. All the normals should point in same direction.
• Warpage: The amount by which an element or element face (in the case of solid elements) deviates from being planar. Warpage of up to fifteen degrees is generally acceptable. Warpage in two-dimensional elements is calculated by splitting a quad into two trias and finding the angle between the two planes which the trias form. The quad is then split again, this time using the opposite corners and forming the second set of trias. The angle between the two planes which the trias form is then found. The maximum angle found between the planes is the warpage of the element. Warpage in three-dimensional elements is performed in the same fashion on all faces of the element.
Figure 11 Warpage of an Element
• Aspect: The ratio of the longest edge of an element to its shortest edge. Aspect ratio should be less than 5:1 in most cases. The reason for this restriction is that if the element stiffness in two directions is very different the structural stiffness matrix has both very large numbers and almost zero numbers on the main diagonal. The computed displacements and stresses may have little accuracy
Figure 12 Aspect Ratio of an element
• Skew: Skew in trias is calculated by finding the minimum angle between the vector from each node to the opposing mid-side and the vector between the two adjacent mid-sides at each node of the element. Ninety degrees minus the minimum angle found is reported as the skew. Skew in quads is calculated by finding the minimum angle between two lines joining opposite mid-sides of the element. Ninety degrees minus the minimum angle found is reported.
Figure 13 Skewness of an element
• Chord dev: Test elements for chordal deviation.
• Min and Max angle, quads: The angle between two sides of a quad element should be 90 degrees as much as possible. Typical required values are to have all angles between 45 degrees and 135 degrees.
• Length: The elements that have a length less than the values specified are highlighted when the length function is selected.
• Jacobian: A measure of the deviation of an element from an ideally shaped element. The Jacobian value ranges from 0.0 to 1.0, where 1.0 represents a perfectly shaped element. However, Jacobian values of 0.6 and above are generally acceptable. The determinant of the Jacobian relates the local stretching of the parametric space required to fit it onto global coordinate space.
• Taper: Taper ratio for quadrilateral elements is defined by first finding the area of the triangle formed at each corner grid point: These areas are then compared to one half of the area of the quadrilateral. HyperMesh then finds the smallest ratio of each of these triangular areas to ½ the quad element’s total area. The resulting value is subtracted from 1, and the result reported as the element taper.
• Min and max angle, trias: The Angle between two sides of a tri element should be 60 degrees as much as possible. Typical required values are to have all tria angles between 20 degrees to 120 degrees.
Element Quality Criteria:
No. Parameters Criterion
1 Element Length- Min 1mm
2 Element Length- Max 20mm
3 Aspect Ratio ≤ 5
4 Warpage ≤ 15
5 Jacobian ≤ 0.6
6 Skewness ≤ 60
7 Quad Element min Interior Angle 45°
8 Quad Element max Interior Angle 135°
9 Tria element min interior angle 20°
10 Tria element max interior angle 120°
11 Total number of triangles ≤ 15%
Table 1. Element Quality Criteria
6.3. Connectors:
Connectors are a geometric representation of connections between entities. The parts in the assemblies need to be held together, whether by bolts, welds, rivets, or adhesives. There are many different ways to model these connection types in FEA, which are specific to the type of analysis being done. Numerous types of connection elements can be modelled such as:
Spot Weld Bolt
Trim Masses Area Connections
Figure 14 Type of Connections
6.4. Loading Points, Materials and Properties:
Assigning material to various parts with values of Young modulus, density, Poisson’s ratio in consistent units. Normally young’s modulus for various parts come in same range but their yield strength limit is different and which can be used for comparing von mises stress in post processing. Assigning the property to the material includes assigning thickness to the various parts. Thickness of the parts varies in range 0.6 to 5 mm. Loading Points are explained in detailed in the analysis chapter.
6.5. Constraints:
Constraints depends on the type of analysis being performed. Modal analysis can also be done on free-free model, i.e. without any constraint. This type of modal analysis has first six modes as rigid modes, i.e. whole body moves as a rigid. In this project, modal analyses is performed by applying constraints in all the directions at the door hinges. Static analysis is performed applying different load cases and constraints which are explained in detail later.
7. REAR DOOR ASSEMBLY
Figure 15 Rear Door Assembly
FEA Model Entities No.
Nodes 70830
2D Elements (Quads, Trias) 64480
3D Elements (Mastique Elements, Hexa Adhesives) 1504
1D Elements 32
OD/Rigid 4000
Spot Welds 122
Table 2 FEA Model Entities
7.1. Component statistics and Material Properties
Sr. No. Component Material Properties
1
Figure 16 Inner Panel
Material: EDD SS4011S2
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 160 N/mm2
Thickness – 0.7 mm
2
Figure 17 Outer Panel
Material: BH180 SS4011S3
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 180 N/mm2
Thickness – 0.63 mm
3
Figure 18 Latch Reinforcement
Material: D513 SS4010
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 190 N/mm2
Thickness – 0.7 mm
4
Figure 19 Intrusion Bar Bracket
Material: D513 SS4010
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 190 N/mm2
Thickness – 1.2 mm
5
Figure 20 Intrusion Bar
Material: DP350 SS4020
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 350 N/mm2
Thickness – 1.6 mm
6
Figure 21 Outer Waistline Reinforcement
Material: D513 SS4010
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 190 N/mm2
Thickness – 0.8 mm
7
Figure 22 Inner Waistline Reinforcement
Material: D513 SS4010
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 190 N/mm2
Thickness – 1.2 mm
8
Figure 23 Body Side Hinge
Material: E34 SS4012A
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 340 N/mm2
Thickness – 5 mm
9
Figure 24 Door Side Hinge
Material: E34 SS4012A
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 340 N/mm2
Thickness – 5 mm
10
Figure 25 Hinge Reinforcement
Material: DP350 SS4020
E = 2.1e5 N/mm2
ρ = 7.89e-9 tons/mm3
Ƞ = 0.29
σy = 350 N/mm2
Thickness – 1.6 mm
8. SOLUTION AND POST PROCESSING
8.1. Modal Analysis:
Modal analysis is used to determine the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component while it is being designed. It also can be a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. The discrete dynamic equation used in FEA is the following:
Where is the mass matrix, is the damping matrix and the stiffness matrix. All three matrices are constant in linear dynamics.
, and are respectively the acceleration vector, velocity vector and the displacement vector. is the load-vector. All three vectors vary as a function of time.
If we neglect damping for the moment and assume free vibrations, the equation becomes:
Assuming the harmonic solution,
Where is a constant vector, and represents the time-response which is simply a sine wave. is the radial frequency of the sine wave. is obtained by differentiating twice. Using this, we obtain:
Dividing by results in the eigenvalue equation:
In which is the eigenvalue and the eigenvector. The roots of this equation are i2, the eigenvalues, where i ranges from 1 to no. of DOF. Corresponding vectors are i, the eigen vectors.
The square root of the eigen values are i, the structure’s natural circular frequencies. The natural frequencies are then calculated as fi = i / 2π. The Eigen vector, i, represent the mode shape – the shape assumed by the structure when vibrating at the frequency fi
Benefits of modal analysis:
• Allows the design to avoid resonant vibrations or to vibrate at a specified frequency
• Finding loose components in the structure: In static analysis, the structure has to be constrained in such a way that any load in any direction can be countered by a reaction force or moment. If the structure is under-constrained, a static analysis will report an error. Finding these problems is easy with a modal analysis: The analysis will report a 0 Hz (i.e. static) mode for each un-constrained direction. These zero-Hertz modes are often referred to as “rigid-body-modes” or “strain-less modes”. This is because the structure (or a part of the structure) translates or rotates as if it was rigid. The displacement shape for these modes should provide enough information about which component(s) may be loose or which constraints are missing.
• Gives an idea of how the structure will respond to different types of dynamic loads
Modal analysis has been performed after creating the finite element model of the door with all DOF constraints at the door hinges and translation constraints at the latch point.
Figure 26 Boundary Constraints for Modal Analysis
The results have been calculated for the first 15 frequency modes and first 4 are shown in the figures below.
Frequency of Mode 1: 35.66 Hz Frequency of Mode 2: 40.84 Hz
Frequency of Mode 3: 61.49 Hz Frequency of Mode 4: 62.73 Hz
Figure 27 First four Mode Shapes
8.2. Static Analysis:
A static analysis calculates the effects of steady loading conditions on a structure, while ignoring inertia and damping effects, such as those caused by time-varying loads. A static analysis can, however, include steady inertia loads (such as gravity and rotational velocity), and time-varying loads that can be approximated as static equivalent loads (such as the static equivalent wind and seismic loads commonly defined in many building codes). Static analysis is used to determine the displacements, stresses, strains, and forces in structures or components caused by loads that do not induce significant inertia and damping effects. There are two conditions for static analysis:
1. The force is static i.e. there is no variation with respect to time (dead weight)
2. Equilibrium condition Σ forces (Fx, Fy, Fz) and Σ Moments (Mx, My, Mz) = 0.
The complete equation to be solved in a linear static FE solver is
F = K * u.
Where, F is the vector of all applied external forces and moments; K is the stiffness matrix of the model depending on material and geometric properties. In a linear analysis, K is constant; u is the nodal displacement vector.
Stress results are compared with elastic limit of the material of the component. It must be lower than it with a certain factor of safety. Displacement results are used for calculating stiffness of the component at a specified point by dividing the applied force with resulting displacement. The calculated stiffness values are compared to target values. If results of some tests do not match targets, modifications must be suggested to some components such as web addition or component thickness increasing or some related parameters changing. Any suggestions must be thoroughly studied since it may affect other criteria i.e. increase overall car weight or decrease stiffness of some other parts. Test must be performed several times to verify validity of the suggested modifications until matching targets is reached all over the door.
8.2.1. Frame Front and Rear stiffness:
For the door component load case “Door Frame Stiffness” the door is rigidly constrained at the mounting points of the hinges as shown in Fig. All degrees of freedom are constrained. A force of 360 N is applied in transversal direction at the inner side of the upper corner of the door window frame. This force application point is constrained in transversal and in vertical direction in order to suppress a global rotation of the door around the hinge axis. The scalar stiffness value for the load case “Door Frame Stiffness” is calculated by dividing 360 N by the total displacement at the force application point.
Figure 28 Frame Stiffness Loads and Boundary Condition
Sr. No. Load-cases Boundary conditions Force
LC 1 Frame front stiffness. The body side bracket of hinge assembly is restrained in all DOFs and ball joint support is given to latch point. An outboard force of 360N is applied to the frame front. The line of action perpendicular to the frame (as shown by LC1).
LC 2 Frame rear stiffness. An outboard force of 360N is applied to the frame rear. The line of action perpendicular to the frame (as shown by LC2).
Table 3 Frame Stiffness Loads and Boundary Condition
Stiffness Calculation:
Figure 29 Frame Front Displacement in Hyperview
Figure 30 Frame Rear Displacements in Hyperview
Results:
• Frame Front stiffness of the Door = 49.81 N/mm
• Frame Rear Stiffness of the Door = 43.94 N/mm
8.2.2. Overall Stiffness:
For the door component load case “Door Overall Stiffness” the door is rigidly constrained at the mounting points of the hinges as shown in Fig. All degrees of freedom are constrained. A force of 360 N is applied in vertically downward direction at the latch point. This force application point is constrained in transversal and in vertical direction in order to suppress a global rotation of the door around the hinge axis. The scalar stiffness value for the load case “Door Frame Stiffness” is calculated by dividing 360 N by the total displacement at the force application point.
Figure 31 Overall Stiffness Loads and Boundary Conditions
Sr. No. Load-cases Boundary conditions Force
LC 3 Overall (Vertical) The body side bracket of hinge assembly is restrained in all DOFs and latch point in Y direction (2). Vertically downward force of 900N is applied at the latch.
Table 4 Overall Stiffness Loads and Boundary Conditions
Stiffness Calculation:
Figure 32 Displacement results in Hyperview
Results:
• The Overall Stiffness of the door = 110.93 N/mm
8.2.3. Torsional Rigidity Top and Bottom Stiffness:
For the door component load case “Door Overall Stiffness” the door is rigidly constrained at the mounting points of the hinges as shown in Fig. All degrees of freedom are constrained. An outboard force of 900N is applied to the door inner and outer corner top. This force application point is constrained in transversal and in vertical direction in order to suppress a global rotation of the door around the hinge axis. The scalar stiffness value for the load case “Door torsion rigidity Stiffness” is calculated by dividing 900 N by the total displacement at the force application point.
Figure 33 Torsional Rigidity Stiffness Loads and Boundary Conditions
Sr. No. Load-cases Boundary conditions Force
LC 4 Torsional rigidity top The body side bracket of hinge assembly is restrained in all DOFs. Latch point in Y direction. An outboard force of 900N is applied to the door inner corner top. (As shown by LC4).
LC 5 Torsional rigidity bottom. An outboard force of 900N is applied to the door inner corner bottom. (As shown by LC5).
Table 5 Torsional Rigidity Stiffness Loads and Boundary Conditions
Stiffness Calculation:
Figure 34 Torsion Rigidity Displacement in Hyperview
Figure 35 Torsion Rigidity bottom displacement in Hyperview
Results:
• Torsional Rigidity Top Stiffness of the Door = 188.28 N/mm
• Torsional Bottom Rigidity Stiffness of the Door = 237.091 N/mm
8.2.4. Inner and Outer Beltline Stiffness:
For the door component load case “Door Beltline Stiffness” the door is rigidly constrained at the mounting points of the hinges as shown in Fig. All degrees of freedom are constrained. A force of 540 N is applied to the beltline reinforcement at the midpoint of the window opening. This force application point is constrained in transversal and in vertical direction in order to suppress a global rotation of the door around the hinge axis. The scalar stiffness value for the load case “Door beltline Stiffness” is calculated by dividing 540 N by the total displacement at the force application point.
Figure 36 Beltline Stiffness Loads and Boundary condition
Sr. No. Load-cases Boundary conditions Force
LC 6 Beltline inner. The body side bracket of hinge assembly is restrained in all DOFs and ball joint support is given to latch point. A lateral force of 540N is applied to the beltline reinforcement at the midpoint of the window opening inner (as shown by LC6).
LC 7 Beltline outer. A lateral force of 540N is applied to the beltline reinforcement at the midpoint of the window opening outer (as shown by LC7).
Table 6 Beltline Stiffness Loads and Boundary condition
Stiffness Calculation:
Figure 37 Inner Beltline Displacement in Hyperview
Figure 38 Outer Beltline Displacement in Hyperview
Results:
• Inner Beltline Stiffness of the Door = 107.18 N/mm
• Outer Beltline Stiffness of the Door = 77.854 N/mm
Summary:
1. Frame Front stiffness of the Door = 49.81 N/mm
2. Frame Rear Stiffness of the Door = 43.94 N/mm
3. The Overall Stiffness of the door = 110.93 N/mm
4. Torsional Rigidity Top Stiffness of the Door = 188.28 N/mm
5. Torsional Bottom Rigidity Stiffness of the Door = 237.091 N/mm
6. Inner Beltline Stiffness of the Door = 107.18 N/mm
7. Outer Beltline Stiffness of the Door = 77.854 N/mm
9. CONCLUSION AND RECOMMENDATIONS
Car Door geometry was imported into the preprocessor tool Hypermesh. The geometry was modeled in the tool and material properties and