Global to Local Model Interface for Deepwater Top Tension Risers

Size: px
Start display at page:

Download "Global to Local Model Interface for Deepwater Top Tension Risers"

Transcription

1 Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching several thousand feet. Deep water risers are pipe structures that extend from the floating vessels to the bottom of the sea. In order to capture the time dependent, geometrically non-linear response of the global system with the complex multicomponent response of local details and properly analyze the riser and its interaction with subsea equipment and vessels it is necessary to use several different models. A global model is used to analyze the global response of the riser to various environmental conditions and local models to analyze the interface between the riser components. Global models usually employ finite elements such as nonlinear (large deflection) beam or pipe elements with highly simplified boundary conditions (fixed, pinned, springs, etc.) Local models are usually built of 3D solid elements with much more detailed boundary conditions, often using contact elements, to realistically predict local response of the particular components. In this paper the methodology of analytical interfacing and data transmission between the local and global models is described. The example of the interface between the global and local model for the deep water top tension risers is included. Introduction The water depths from which oil and gas is being produced are reaching several thousands feet. Deep water risers convey fluids such as oil, gas or water between the seabed and the surface vessel. There are many different configurations that are used, depending on application, vessel type and environmental conditions. The most typical are SCRs (Simple Catenary Risers), TTRs (Top Tension Risers) and free standing risers connected to the vessel with flexible jumpers (Reference 1). At the first sight, the riser appears to be a simple structure, but in reality, its response is very complicated. The global response is time dependant and geometrically nonlinear. To capture the local response of the numerous interfaces, detailed modeling of these areas is necessary. The complexity of both global response and detailed components leads to the approach that employs several models of different level of details for various steps of analysis. Global models are usually modeled using pipe elements with simplified boundary conditions. Global analysis results are then used as the input data for further analysis of the sub-components. The paper describes the multiple steps of the analysis and interfacing between the various models and provides the means to verify the correctness of each step. As an example, the modeling and the analysis of TTRs and their interface with the floating vessel is described. The tension in the TTRs is usually provided by the aircan/stem assembly that is located around the upper portion of the riser string. The tension is transferred through the stem head to the riser casing. The bending moment in the riser due to vessel motions and environmental loading is transferred to the riser primarily by the keel joint that is located at the lower end of the stem and set of centralizers between the stem and the riser. This paper focuses on the analysis methods of the keel joint to stem interface as well as on the analysis of the upper stem section. Procedure Risers are subject to severe loading coming from different sources. The types of loading could by described as: Loading caused by the vessel motions Pressure of contained fluids Environmental loading

2 All of the above loads act together so they need to be considered jointly during any type of analysis. The main objectives of the riser analysis are (Reference 1): To ensure that the maximum stress is below the design allowable To ensure that the fatigue life induced by cycling loading meets the design life of the structure These objectives are achieved by conducting global analysis with riser modeled using pipe or beam elements (Reference 2). The results from the analysis utilizing this model are used to assess the global performance of the structure. Often, there is a need to analyze the structure in a more detailed manner, focusing on local behavior of particular components. Thus, local models are developed using shell and solid finite elements. Simplified global boundary conditions such as pinned or fixed nodes of the beam elements can be modeled more realistically using contact elements on the surfaces of the 3D solid or shell local models. The loading that is applied to the global model are the vessel motions that are transferred by the appropriate boundary conditions and environmental loading in form of the current and waves. However, as the application of the pressure of contained fluids is fairly straightforward and is done virtually the same way for the global and local model, the pressure modeling is excluded from the scope of this study. The application of the boundary conditions and loading to the local model is not that straightforward as the local model is only the cutout from the larger global model. It is necessary to extract the information from the global model in order to appropriately constrain and apply the loads to the local model. The following data can be extracted at each node of the pipe or beam model from the global analysis: Displacements in 6 DOFs for each timestep Internal forces in 6 DOFs for each timestep If the displacements are known for each timestep of the global dynamic analysis, then the following approach can be implemented to conduct the analysis using local model: 1. Build the local beam model that will represent a cut-off from the global model. 2. Apply the boundary conditions extracted from the corresponding nodes of the global model to the local model. 3. Compare the response of the local model with the response of the global model as a quality check. 4. Build the full 3D local model using the solid or shell elements. 5. Apply the same boundary conditions as applied to the local beam model to the 3D local model. 6. Compare the response of the 3D local model with the response of the local beam model as a quality check. 7. Perform the required analysis on the 3D local model, using ANSYS (Reference 2) built-in submodeling procedures if required. The procedure described above is possible only, if all the necessary global analysis data is available for the local analysis. This is not always the case - often the party conducting the detailed FE analysis is provided only limited data. Usually the available data for the analysis is snapshots of the maximum internal forces along the riser. Thus, the methodology specified above needs to be adapted to account for these circumstances. Step two of the approach described above is modified to the following: 2A. Apply the fixed boundary conditions at one end of the model and internal forces resulting from the local model at the other end. Due to differences in the boundary conditions and disregarding of the dynamic forces, the local to global model comparison, usually shows different response. The key issue with this approach is to be able to assess the impact of these differences on the final conclusions. Otherwise, this method is very effective, if used properly.

3 Analysis In-house Global and Local Dynamic Analysis of the Stem A schematic drawing of the structure analyzed is shown in Figure 1 below. The stem that is modeled as the pipe in the global model is in reality a complex structure made up of several different sections. The objective of the detailed FE analysis is to determine the stress distribution in the tapered section of the stem, where the wall thickness changes from 0.3 to 0.5in. The global pipe model is shown in Figure 2 and Figure 3 below. The stem and the riser are modeled with pipe elements. The interaction between the riser and stem as well as between the stem and the vessel is modeled using friction guides modeled using CONTA178 contact element with cylindrical gap option. Figure 1. Coupled Riser - Stem/Air Can Sketch

4 Figure 2. Coupled Riser-Stem/Air Can Global Model Figure 3. Coupled Riser-Stem/Air Can Global Model Upper Section The objective of the analysis is to assess the stress distribution in a section of the stem under the dynamic loading. As the first step, the global model is analyzed by applying the vessel motions and the current

5 loading to the model. Analysis is performed with 10 year hurricane regular wave loading. The timetraces of the 6 DOFs are extracted at two locations. Further to this, the local beam model is developed. The timetraces of the displacements from the global model are applied to the top and bottom nodes of the local beam model as the boundary conditions. The results comparison between the local and global model is shown in Figure 4. Figure 4. Results Comparison - Global and Local Beam Model The next step is to build the detailed local model using shell elements. In this case, the local model is a simple cylinder meshed with shell elements as shown in Figure 5. Different colors of the elements represent different wall thicknesses.

6 Figure 5. Local Shell Model FE Mesh The top and bottom of the cylinder are constrained using the master-slave constrains as shown in Figure 6. The boundary conditions are applied the same way to the local shell model as to the local beam model. The dynamic analysis is performed for 40 sec. The timetrace of stresses for the local beam model and the detailed shell local model are shown in Figure 7. The comparison of the response of both models indicates the correctness of the analysis process. Figure 6. Master - Slave Boundary Conditions

7 Figure 7. Stress in Local Beam and 3D Shell Model Further steps may be taken using Ansys built-in sub-modeling functions. In this particular case the detailed analysis of the transitions between two wall thicknesses is conducted using a 3D solid sub-model. The section along the 3D solid sub-model is shown in Figure 8. The boundaries of the sub-model are defined as specified in Figure 9. Figure 8. FE Mesh along the Mid Taper Section of Stem 3D Solid Sub-Model

8 Figure 9. Stress in 3D Solid Model with Sub-modeling Boundary Conditions Ansys sub-modeling allows transferring the resultant deformation along the boundary line from one model and applying it to a different model as boundary conditions. This enables further more detail analysis of the particular components. This function is very efficient with optimization analysis. However, it is necessary to proceed with caution when using sub-modeling and ensure that the changes made to the submodel do not impact the global model response. In this case it is necessary to rerun the analysis with the updated model. Detailed Finite Element Analysis of Keel Joint This section discusses another example that illustrates the interface between a global and local model. The problem involves using ANSYS to perform the detailed local finite element analysis of a keel joint in a top tensioned riser (TTR). The global results for the TTR are obtained using a pipe element model. The details of a top tensioned riser are shown in Figure 1. The top tensioned riser in this example is a pipein-pipe type i.e. it has an outer casing and inner casing. The keel joint is used to locally stiffen the fatigue critical region of the outer casing. The keel joint is centralized within the stem using a wheel/ball, which is shrunk-fit around the keel joint. The keel joint is attached to the riser pipe using flanges. The objective of the local analysis is to verify the strength of the keel joint under extreme hurricane loads. The stress concentration factors (SCFs) (Reference 3) along the keel joint length are also required to confirm that the geometry of the joint is suitable for the fatigue requirements of the riser system. Model Details The entire riser is modeled using pipe elements. This problem differs from the previous example as the entire global analysis results are not available for the local analysis. The maximum bending moment, effective tension and shear force distribution snapshots obtained from the global dynamic analysis are provided along the critical region in the riser.

9 Detailed FEA of the keel joint is performed in ANSYS. Two FE models - the stepped beam model and the 3D solid model - are developed for the local analysis. A stepped beam model is used to make a comparison with the global model results and to obtain the nominal stress distribution along the keel joint length. BEAM3 elements are used for this model. The upper end of the model is fixed in all six degrees of freedom and the bending moment, tension and shear as well as reaction between the stem and the keel ball are applied as concentrated forces. The center of the keel ball is constrained only by the reaction force with no geometric boundary conditions in order to ensure that the local model assumes the correct displaced shape. A solid half model of the keel joint, the keel ball, the upper and lower crossover joints and nominal riser joint is used for keel strength analysis and determining the SCF. SOLID95 3D elements (Reference 2) are used for the model. Contact between the ball and the keel is modeled using CONTA174 and TARGE170 elements (Reference 2). The mesh at the keel ball is shown in Figure 10. The boundary conditions are applied at a distance of 5 times the nominal diameter from the region of interest. This is done to ensure that discontinuities due to the application of boundary conditions are at a sufficient distance from the regions of interest and do not affect the results of the analysis. For determining the SCF and strength analysis, the model is assumed fixed at the upper end. As shown in Figure 11, bending, tension and shear forces are applied as equivalent nodal forces at the lower end of the model. Reaction from the stem is applied at the center of the keel ball as a point load. Vertical friction between the stem and the ball is also included in the 3D model. The friction coefficient between the stem and the ball is assumed to be 0.5. The shrink fit is represented by initial penetration of the ball into the keel. The flange is modeled as a solid block, resulting in a slightly higher stiffness for this component. Figure 10. 3D Mesh Details at the Keel Ball

10 Figure 11. Boundary Conditions Applied to 3D Model Discussion of Results The stepped beam model is used to verify whether the resulting force and stress distributions, obtained using the intended method of applying the boundary conditions, match with the global analysis results and to determine the discrepancies. The bending moment distribution along the model length obtained using the two models is presented in Figure 12. The bending moment from the ANSYS stepped beam model is higher than that predicted by the global model by 7.3% at the keel joint center. All six degrees of freedom are constrained at the upper end of the beam model. The tension, bending moment and shear loads are applied at the lower end. In the global model, the displacements at the location of the upper end of the stepped beam model are limited by the stiffness of the pipe above and by the arrangement of the stem-riser centralizers. Therefore, the fixed end boundary condition in the beam model causes a higher bending moment distribution along the model length. The exclusion of the inner casing in the ANSYS model also affects the bending moment. The bending moment in the inner casing is approximately 10% of the bending moment in the outer casing for the 1-year winter storm loading condition.

11 Figure 12. Comparison of Bending Moment from ANSYS Beam Model with Global Analysis Results The differences between the global analysis and beam model results do not affect the determination of the SCF as the nominal stresses are derived by applying the loading and boundary conditions identical with the 3D model to the beam model. For the strength analysis, the higher bending moment obtained using the beam model implies that applying the same load to the 3D model provides a conservative result. The SCFs are calculated as the change in the first principal stress due to bending fluctuations divided by the change in the nominal stress due to bending. The plot for the principal bending stress from the 3D model and the bending stress from the beam model for a typical loading condition is shown in Figure 13.

12 Figure 13. Principal Stress (3D Model) and Nominal Bending Stress (Beam Model) along Keel Joint Conclusion The paper presents a detailed methodology for interfacing between global and local finite element models in order to capture the time dependent geometrically non-linear response of the global system with the complex multi-component response of local details. Two examples illustrating the procedure are presented. The first example shows how displacement timetraces can be used to interface between global and local models. The second example shows how the snapshot of the maximum global loads can be used to perform local component analysis. The use of the timetrace approach is more straightforward and reliable. Performing both the global and local analysis ensures that a one-to-one correspondence between the global and local models can be maintained whilst avoiding undue complexity in both the global and local models. This facilitates the easy transfer of boundary conditions from one model to another. However, the limited access to the results of global analysis conducted by a different party can be a constraint and the second example demonstrates a way to get around the problem. The results obtained in the second problem are shown to be conservative and accurate within 10% of the expected results. References 1) American Petroleum Institute, Recommended Practice for Design of Risers for Floating Production Systems and TLP's, API-RP-2RD, API, June ) Swanson Analysis Systems Inc, ANSYS/Structural Finite Element Analysis Software, Version 6.0, April ) R. J. Roark, W. C. Young, Formulas for Stress and Strain, McGraw-Hill, 1984, Singapore.

ANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.

ANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best

More information

A05 Steel Catenary Riser Systems

A05 Steel Catenary Riser Systems A05 Steel Catenary Riser Systems Introduction This example contains three examples of steel catenary risers (SCRs). These are: Catenary with Spar Catenary with SemiSub Lazy Wave with FPSO The example also

More information

D04 J-Tube Pull-In. Orcina. 1. Introduction

D04 J-Tube Pull-In. Orcina. 1. Introduction D04 J-Tube Pull-In 1. Introduction This example shows how to model a typical J-tube pull-in operation. It includes pulling a line (a riser) out from a vessel over a chute whilst simultaneously pulling

More information

Revised Sheet Metal Simulation, J.E. Akin, Rice University

Revised Sheet Metal Simulation, J.E. Akin, Rice University Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.

More information

Stress Concentration Factors

Stress Concentration Factors CONSEIL INTERNATIONAL DES MACHINES A COMBUSTION INTERNATIONAL COUNCIL ON COMBUSTION ENGINES CO-ORDINATING WORKING GROUP "CLASSIFICATION SOCIETIES DIESEL" (WG2) Proposal by CIMAC WG4 11th May 2012 IACS

More information

Technical Report Example (1) Chartered (CEng) Membership

Technical Report Example (1) Chartered (CEng) Membership Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION

More information

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake

More information

Chapter 3 Analysis of Original Steel Post

Chapter 3 Analysis of Original Steel Post Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part

More information

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to

More information

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they

More information

MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, From your book and other

MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, From your book and other MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, 2016 1.0 From your book and other sources, write a paragraph explaining CFD and finite element

More information

Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA

Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA Andrew Smyth, P.E. LPI, Inc., New York, NY, USA Abstract Overhead crane wire ropes utilized within manufacturing plants are subject to extensive

More information

SOLIDWORKS Simulation

SOLIDWORKS Simulation SOLIDWORKS Simulation Length: 3 days Prerequisite: SOLIDWORKS Essentials Description: SOLIDWORKS Simulation is designed to make SOLIDWORKS users more productive with the SOLIDWORKS Simulation Bundle. This

More information

Manual. Ansys Exercise. Offshore Wind Farm Design

Manual. Ansys Exercise. Offshore Wind Farm Design Manual for the Ansys Exercise Accompanying the Offshore Wind Farm Design Assignment Contents Contents... i 1. Introduction... 1 2. Brief Overview of ANSYS... 2 3. Overview of the input files for the ANSYS

More information

MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1

MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1 Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress

More information

Lesson 6: Assembly Structural Analysis

Lesson 6: Assembly Structural Analysis Lesson 6: Assembly Structural Analysis In this lesson you will learn different approaches to analyze the assembly using assembly analysis connection properties between assembly components. In addition

More information

ME Optimization of a Frame

ME Optimization of a Frame ME 475 - Optimization of a Frame Analysis Problem Statement: The following problem will be analyzed using Abaqus. 4 7 7 5,000 N 5,000 N 0,000 N 6 6 4 3 5 5 4 4 3 3 Figure. Full frame geometry and loading

More information

The part to be analyzed is the bracket from the tutorial of Chapter 3.

The part to be analyzed is the bracket from the tutorial of Chapter 3. Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component

More information

Step Change in Design: Exploring Sixty Stent Design Variations Overnight

Step Change in Design: Exploring Sixty Stent Design Variations Overnight Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com

More information

CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION

CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION 68 CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION 4.1 INTRODUCTION There is a demand for the gears with higher load carrying capacity and increased fatigue life. Researchers in the

More information

Offshore Platform Fluid Structure Interaction (FSI) Simulation

Offshore Platform Fluid Structure Interaction (FSI) Simulation Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,

More information

SolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs

SolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs An Overview of SolidWorks and Its Associated Analysis Programs prepared by Prof. D. Xue University of Calgary SolidWorks - a solid modeling CAD tool. COSMOSWorks - a design analysis system fully integrated

More information

Exercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method

Exercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method Exercise 1 3-Point Bending Using the GUI and the Bottom-up-Method Contents Learn how to... 1 Given... 2 Questions... 2 Taking advantage of symmetries... 2 A. Preprocessor (Setting up the Model)... 3 A.1

More information

OTC are critical locations that exhibit complex response having the lowest predicted fatigue life.

OTC are critical locations that exhibit complex response having the lowest predicted fatigue life. OTC 17248 A Fatigue Monitoring Strategy & Implementation on a Deepwater Top Tensioned Riser Ricky Thethi, 2H Offshore Inc.; Hugh Howells, 2H Offshore Engineering Limited; Shreenaath Natarajan, 2H Offshore

More information

What makes Bolt Self-loosening Predictable?

What makes Bolt Self-loosening Predictable? What makes Bolt Self-loosening Predictable? Abstract Dr.-Ing. R. Helfrich, Dr.-Ing. M. Klein (INTES GmbH, Germany) In mechanical engineering, bolts are frequently used as standard fastening elements, which

More information

Future Trends Part - 1 A New CAD & CAE AIES Ltd

Future Trends Part - 1 A New CAD & CAE AIES Ltd Future Trends Part - 1 A New CAD & CAE Process @ AIES Ltd Dr Ian McLuckie April 2016 ian.mcluckie@aiesl.co.uk 1 Future Trends - CAD & CAE There is a lot of discussion about how we need bigger and faster

More information

Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections

Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections October 25, 2000 Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections Tommi Vanhala Helsinki Institute of Physics 1. INTRODUCTION...2 2. STIFFNESS ANALYSES...2 2.1 ENVELOPE...2 2.2

More information

THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD

THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD Haval Kamal Asker Department of Mechanical Engineering, Faculty of Agriculture and Forestry, Duhok University, Duhok,

More information

Coupled Analysis of FSI

Coupled Analysis of FSI Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA

More information

Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet

Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Mahesha J 1, Prashanth A S 2 M.Tech Student, Machine Design, Dr. A.I.T, Bangalore, India 1 Asst. Professor, Department of Mechanical

More information

Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses

Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses Goals In this exercise, we will explore the strengths and weaknesses of different element types (tetrahedrons vs. hexahedrons,

More information

Introduction to FEM Modeling

Introduction to FEM Modeling Total Analysis Solution for Multi-disciplinary Optimum Design Apoorv Sharma midas NFX CAE Consultant 1 1. Introduction 2. Element Types 3. Sample Exercise: 1D Modeling 4. Meshing Tools 5. Loads and Boundary

More information

Module 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis

Module 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis 25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load

More information

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Outcome 1 The learner can: CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Calculate stresses, strain and deflections in a range of components under

More information

ME 475 FEA of a Composite Panel

ME 475 FEA of a Composite Panel ME 475 FEA of a Composite Panel Objectives: To determine the deflection and stress state of a composite panel subjected to asymmetric loading. Introduction: Composite laminates are composed of thin layers

More information

Visit the following websites to learn more about this book:

Visit the following websites to learn more about this book: Visit the following websites to learn more about this book: 6 Introduction to Finite Element Simulation Historically, finite element modeling tools were only capable of solving the simplest engineering

More information

Stress Analysis of Cross Groove Type Constant Velocity Joint

Stress Analysis of Cross Groove Type Constant Velocity Joint TECHNICAL REPORT Stress Analysis of Cross Groove Type Constant Velocity Joint H. SAITO T. MAEDA The driveshaft is the part that transmits the vehicle's engine torque and rotation to the tires, and predicting

More information

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0 Exercise 1 3-Point Bending Using the Static Structural Module of Contents Ansys Workbench 14.0 Learn how to...1 Given...2 Questions...2 Taking advantage of symmetries...2 A. Getting started...3 A.1 Choose

More information

A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov

A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue. Alan Mueller & Oleg Voronkov A study of Jumper FIV due to multiphase internal flow: understanding life-cycle fatigue Alan Mueller & Oleg Voronkov Case description Main structural dimensions [1]: deformable jumper [2] in Mixture on

More information

TABLE OF CONTENTS SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 SECTION 3 WAVE REFLECTION AND TRANSMISSION IN RODS Introduction...

TABLE OF CONTENTS SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 SECTION 3 WAVE REFLECTION AND TRANSMISSION IN RODS Introduction... TABLE OF CONTENTS SECTION 1 INTRODUCTION... 1 1.1 Introduction... 1 1.2 Objectives... 1 1.3 Report organization... 2 SECTION 2 BACKGROUND AND LITERATURE REVIEW... 3 2.1 Introduction... 3 2.2 Wave propagation

More information

Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004

Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004 Structural stability of shelf probe cards Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004 Presentation Outline Introduction Objectives Multi die applications

More information

WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14

WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14 WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.

More information

VALIDATE SIMULATION TECHNIQUES OF A MOBILE EXPLOSIVE CONTAINMENT VESSEL

VALIDATE SIMULATION TECHNIQUES OF A MOBILE EXPLOSIVE CONTAINMENT VESSEL VALIDATE SIMULATION TECHNIQUES OF A MOBILE EXPLOSIVE CONTAINMENT VESSEL David Karlsson DYNAmore Nordic AB, Sweden KEYWORDS Hexa, Map, Explosive, LS-DYNA ABSTRACT A Mobile Explosive Containment Vessel (MECV)

More information

B01 Drilling Riser. Orcina. 1. Building the model

B01 Drilling Riser. Orcina. 1. Building the model B01 Drilling Riser A tensioned drilling riser descends from a semi-submersible drilling vessel to a BOP (blow out preventer) on the seabed. A drill string is modelled running inside the riser down to the

More information

Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing

Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Kasetsart J. (Nat. Sci.) 42 : 165-176 (2008) Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Chakrit Suvanjumrat*, Tumrong Puttapitukporn and Satjarthip Thusneyapan

More information

Analysis of Crank End of Connecting Rod using Finite Element Method

Analysis of Crank End of Connecting Rod using Finite Element Method Analysis of Crank End of Connecting Rod using Finite Element Method Mohammad Umair Zaki Faculty of Mechanical Engineering Noida International University Greater Noida, India e-mail-umairzaki@yahoo.com

More information

Development of the Compliant Mooring Line Model for FLOW-3D

Development of the Compliant Mooring Line Model for FLOW-3D Flow Science Report 08-15 Development of the Compliant Mooring Line Model for FLOW-3D Gengsheng Wei Flow Science, Inc. October 2015 1. Introduction Mooring systems are common in offshore structures, ship

More information

Abstract. Introduction:

Abstract. Introduction: Abstract This project analyzed a lifecycle test fixture for stress under generic test loading. The maximum stress is expected to occur near the shrink fit pin on the lever arm. The model was constructed

More information

LIGO Scissors Table Static Test and Analysis Results

LIGO Scissors Table Static Test and Analysis Results LIGO-T980125-00-D HYTEC-TN-LIGO-31 LIGO Scissors Table Static Test and Analysis Results Eric Swensen and Franz Biehl August 30, 1998 Abstract Static structural tests were conducted on the LIGO scissors

More information

Mixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube

Mixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube Journal of Materials Science & Surface Engineering Vol. 3 (4), 2015, pp 298-302 Contents lists available at http://www.jmsse.org/ Journal of Materials Science & Surface Engineering Mixed Mode Fracture

More information

Using MSC.Nastran for Explicit FEM Simulations

Using MSC.Nastran for Explicit FEM Simulations 3. LS-DYNA Anwenderforum, Bamberg 2004 CAE / IT III Using MSC.Nastran for Explicit FEM Simulations Patrick Doelfs, Dr. Ingo Neubauer MSC.Software GmbH, D-81829 München, Patrick.Doelfs@mscsoftware.com Abstract:

More information

Finite Element Analysis Using Creo Simulate 4.0

Finite Element Analysis Using Creo Simulate 4.0 Introduction to Finite Element Analysis Using Creo Simulate 4.0 Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

Quarter Symmetry Tank Stress (Draft 4 Oct 24 06)

Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of

More information

PTC Newsletter January 14th, 2002

PTC  Newsletter January 14th, 2002 PTC Email Newsletter January 14th, 2002 PTC Product Focus: Pro/MECHANICA (Structure) Tip of the Week: Creating and using Rigid Connections Upcoming Events and Training Class Schedules PTC Product Focus:

More information

Analysis of Detroit Seismic Joint System

Analysis of Detroit Seismic Joint System Analysis of Detroit Seismic Joint System for EMSEAL Corporation Prepared by Haig Saadetian, P.Eng. Senior Consultant ROI Engineering Inc. 50 Ronson Drive, Suite 120 Toronto ON M9W 1B3 26-April-2009 1 Contents

More information

Eng Ship Structures 1 L E C T U R E 1 0 : F I N I T E E L E M E N T T E C H N I Q U E S I N S H I P S T R U C T U R A L D E S I G N

Eng Ship Structures 1 L E C T U R E 1 0 : F I N I T E E L E M E N T T E C H N I Q U E S I N S H I P S T R U C T U R A L D E S I G N Eng. 6002 Ship Structures 1 L E C T U R E 1 0 : F I N I T E E L E M E N T T E C H N I Q U E S I N S H I P S T R U C T U R A L D E S I G N Contents Introduction Linear Analysis Static Non-linear Analysis

More information

COMPUTER AIDED ENGINEERING. Part-1

COMPUTER AIDED ENGINEERING. Part-1 COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.

More information

Week 12 - Lecture Mechanical Event Simulation. ME Introduction to CAD/CAE Tools

Week 12 - Lecture Mechanical Event Simulation. ME Introduction to CAD/CAE Tools Week 12 - Lecture Mechanical Event Simulation Lecture Topics Mechanical Event Simulation Overview Additional Element Types Joint Component Description General Constraint Refresh Mesh Control Force Estimation

More information

Creo Simulate 3.0 Tutorial

Creo Simulate 3.0 Tutorial Creo Simulate 3.0 Tutorial Structure and Thermal Roger Toogood, Ph.D., P. Eng. SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

Appendix B Submodeling Technique

Appendix B Submodeling Technique Appendix B Submodeling Technique 16.0 Release Introduction to ANSYS Mechanical 1 2015 ANSYS, Inc. February 27, 2015 Chapter Overview In this chapter controlling meshing operations is described. Topics:

More information

Computer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks

Computer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University

More information

Slug Induced Vibrations in Pipeline and Jumper Spans Enhanced industry design and analysis methods enabled by the SLARP JIP

Slug Induced Vibrations in Pipeline and Jumper Spans Enhanced industry design and analysis methods enabled by the SLARP JIP Slugfest Slug Induced Vibrations in Pipeline and Jumper Spans Enhanced industry design and analysis methods enabled by the SLARP JIP Kieran Kavanagh Technology & Engineering Director, Wood Group Kenny

More information

inter.noise 2000 The 29th International Congress and Exhibition on Noise Control Engineering August 2000, Nice, FRANCE

inter.noise 2000 The 29th International Congress and Exhibition on Noise Control Engineering August 2000, Nice, FRANCE Copyright SFA - InterNoise 2000 1 inter.noise 2000 The 29th International Congress and Exhibition on Noise Control Engineering 27-30 August 2000, Nice, FRANCE I-INCE Classification: 7.6 CHARACTERIZING

More information

Element Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can

Element Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be

More information

An Overview of Computer Aided Design and Finite Element Analysis

An Overview of Computer Aided Design and Finite Element Analysis An Overview of Computer Aided Design and Finite Element Analysis by James Doane, PhD, PE Contents 1.0 Course Overview... 4 2.0 General Concepts... 4 2.1 What is Computer Aided Design... 4 2.1.1 2D verses

More information

Lateral Loading of Suction Pile in 3D

Lateral Loading of Suction Pile in 3D Lateral Loading of Suction Pile in 3D Buoy Chain Sea Bed Suction Pile Integrated Solver Optimized for the next generation 64-bit platform Finite Element Solutions for Geotechnical Engineering 00 Overview

More information

2008 International ANSYS Conference

2008 International ANSYS Conference 2008 International ANSYS Conference FEM AND FSI SIMULATIONS OF IMPACT LOADS ON GRP SUBSEA COMPOSITE COVERS Kjetil Rognlien, MSc Technical Consultant EDR AS, Norway 2008 ANSYS, Inc. All rights reserved.

More information

Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields

Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields David Woyak 1, Brian Baillargeon, Ramesh Marrey, and Randy Grishaber 2 1 Dassault Systemés SIMULIA Corporation &

More information

LATERALLY LOADED PILE GROUPS

LATERALLY LOADED PILE GROUPS LATERALLY LOADED PILE GROUPS Pedro Meneses Key words: Group Interaction, Lateral Response, Piles, p-multipliers, p-y Curves. Introduction The lateral resistance of pile foundations is a particularly important

More information

CHAPTER 4 CFD AND FEA ANALYSIS OF DEEP DRAWING PROCESS

CHAPTER 4 CFD AND FEA ANALYSIS OF DEEP DRAWING PROCESS 54 CHAPTER 4 CFD AND FEA ANALYSIS OF DEEP DRAWING PROCESS 4.1 INTRODUCTION In Fluid assisted deep drawing process the punch moves in the fluid chamber, the pressure is generated in the fluid. This fluid

More information

General modeling guidelines

General modeling guidelines General modeling guidelines Some quotes from industry FEA experts: Finite element analysis is a very powerful tool with which to design products of superior quality. Like all tools, it can be used properly,

More information

Non-Linear Analysis of Base Plates in Automated Storage Systems

Non-Linear Analysis of Base Plates in Automated Storage Systems Non-Linear Analysis of Base Plates in Automated Storage Systems Ph.D. Juan José del Coz Díaz, Fco. Suarez Domínguez, Paulino J.Garcia Nieto University of Oviedo. Construction and Applied Mathematics Area.

More information

DESIGNING FIBER OPTIC DYNAMIC RISER CABLES FOR OFFSHORE APPLICATIONS

DESIGNING FIBER OPTIC DYNAMIC RISER CABLES FOR OFFSHORE APPLICATIONS DESIGNING FIBER OPTIC DYNAMIC RISER CABLES FOR OFFSHORE APPLICATIONS Jon Steinar Andreassen (Nexans Norway) Email: Nexans Norway AS, P.O Box 645 Etterstad, N-65 Oslo,

More information

WP1 NUMERICAL BENCHMARK INVESTIGATION

WP1 NUMERICAL BENCHMARK INVESTIGATION WP1 NUMERICAL BENCHMARK INVESTIGATION 1 Table of contents 1 Introduction... 3 2 1 st example: beam under pure bending... 3 2.1 Definition of load application and boundary conditions... 4 2.2 Definition

More information

WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14

WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14 WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.

More information

Finite element modelling techniques and testing methods of submerged pipes

Finite element modelling techniques and testing methods of submerged pipes Visit the SIMULIA Resource Center for more customer examples. Finite element modelling techniques and testing methods of submerged pipes A. Giordano 1, A.C. Walker 2 and F. Guarracino 1 1 Dipartimento

More information

Bridge Software Institute 2

Bridge Software Institute 2 EXECUTIVE SUMMARY This report summarizes six API soil models that have been implemented into the FB- MultiPier computer program according to the American Petroleum Institute Recommended Practice 2A LRFD

More information

Set No. 1 IV B.Tech. I Semester Regular Examinations, November 2010 FINITE ELEMENT METHODS (Mechanical Engineering) Time: 3 Hours Max Marks: 80 Answer any FIVE Questions All Questions carry equal marks

More information

Force Model & Solid Model Report. MIE 313 Design of Mechanical Components. Amado, Juliana A. Nestor, Charlene Walsh, Peter J.

Force Model & Solid Model Report. MIE 313 Design of Mechanical Components. Amado, Juliana A. Nestor, Charlene Walsh, Peter J. Force Model & Solid Model Report MIE 313 Design of Mechanical Components. Amado, Juliana A. Nestor, Charlene Walsh, Peter J. Table of Contents Force Model & Solid Model Report... i Abstract:... iv Introduction:...

More information

Abaqus CAE Tutorial 6: Contact Problem

Abaqus CAE Tutorial 6: Contact Problem ENGI 7706/7934: Finite Element Analysis Abaqus CAE Tutorial 6: Contact Problem Problem Description In this problem, a segment of an electrical contact switch (steel) is modeled by displacing the upper

More information

1.2 Connection configurations:

1.2 Connection configurations: 1.2 Connection configurations: 1.2.1 Simple connections: Simple connections are assumed to transfer shear only shear at some nominal eccentricity. Therefore such connections can be used only in non-sway

More information

Introduction to ANSYS Mechanical

Introduction to ANSYS Mechanical Lecture 6 Modeling Connections 15.0 Release Introduction to ANSYS Mechanical 1 2012 ANSYS, Inc. February 12, 2014 Chapter Overview In this chapter, we will extend the discussion of contact control begun

More information

Matching Real World Results

Matching Real World Results Matching Real World Results Randy Dreher FFE Minerals Inc. Jan Janssen, Doug Farnell, Stephen Thompson Farnell-Thompson Applied Technologies Inc Abstract Comparing measured results to those generated by

More information

Workbench-Mechanical Structural Nonlinearities

Workbench-Mechanical Structural Nonlinearities Workshop 2B Assembly Contact Workbench-Mechanical Structural Nonlinearities WS2B-1 Workshop 2B Assembly Contact Goal: In this workshop our goal is to investigate the behavior of the pipe clamp assembly

More information

The Role of Finite Element Analysis in Light Aircraft Design and Certification

The Role of Finite Element Analysis in Light Aircraft Design and Certification The Role of Finite Element Analysis in Light Aircraft Design and Certification Nigel Bamber Wey Valley Aeronautics Ltd www.weyvalleyaero.co.uk Engineering Consultancy Civil and Military Aerospace and Motorsport

More information

ANSYS AIM Tutorial Stepped Shaft in Axial Tension

ANSYS AIM Tutorial Stepped Shaft in Axial Tension ANSYS AIM Tutorial Stepped Shaft in Axial Tension Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Contents: Problem Specification 3 Learning Goals 4 Pre-Analysis & Start Up 5 Calculation

More information

Introduction to the Finite Element Method (3)

Introduction to the Finite Element Method (3) Introduction to the Finite Element Method (3) Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic petr.kabele@fsv.cvut.cz people.fsv.cvut.cz/~pkabele 1 Outline

More information

Chapter 5 Modeling and Simulation of Mechanism

Chapter 5 Modeling and Simulation of Mechanism Chapter 5 Modeling and Simulation of Mechanism In the present study, KED analysis of four bar planar mechanism using MATLAB program and ANSYS software has been carried out. The analysis has also been carried

More information

Lecture 5 Modeling Connections

Lecture 5 Modeling Connections Lecture 5 Modeling Connections 16.0 Release Introduction to ANSYS Mechanical 1 2015 ANSYS, Inc. February 27, 2015 Chapter Overview In this chapter, we will extend the discussion of contact control begun

More information

Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint

Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Jose M. Cabrero Assistant Professor University of Navarra, Department of Structural Analysis and Design,

More information

Solid design. Reliable pipelines. Simulation results can be viewed and printed in different formats in tables, graphs and in 3D illustrations.

Solid design. Reliable pipelines. Simulation results can be viewed and printed in different formats in tables, graphs and in 3D illustrations. Bringing added value to pipeline engineers worldwide SAGE Profile has been specifically designed to assist pipeline engineers in the design, installation and analysis of offshore pipelines. The powerful

More information

Efficient Shape Optimisation of an Aircraft Landing Gear Door Locking Mechanism by Coupling Abaqus to GENESIS

Efficient Shape Optimisation of an Aircraft Landing Gear Door Locking Mechanism by Coupling Abaqus to GENESIS Efficient Shape Optimisation of an Aircraft Landing Gear Door Locking Mechanism by Coupling Abaqus to GENESIS Mark Arnold and Martin Gambling Penso Consulting Ltd GRM Consulting Ltd Abstract: The objective

More information

TOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION

TOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION TOPOLOGY OPTIMIZATION OF WING RIBS IN CESSNA CITATION [1],Sathiyavani S [2], Arun K K [3] 1,2 student, 3 Assistant professor Kumaraguru College of technology, Coimbatore Abstract Structural design optimization

More information

midas NFX 2017R1 Release Note

midas NFX 2017R1 Release Note Total Solution for True Analysis-driven Design midas NFX 2017R1 Release Note 1 midas NFX R E L E A S E N O T E 2 0 1 7 R 1 Major Improvements Midas NFX is an integrated finite element analysis program

More information

FB-MULTIPIER vs ADINA VALIDATION MODELING

FB-MULTIPIER vs ADINA VALIDATION MODELING FB-MULTIPIER vs ADINA VALIDATION MODELING 1. INTRODUCTION 1.1 Purpose of FB-MultiPier Validation testing Performing validation of structural analysis software delineates the capabilities and limitations

More information

Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading

Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading IUST International Journal of Engineering Science, Vol. 17, No.3-4, 2006, Page 21-28 Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading M. Haghpanahi and H. Pirali

More information

Nerf Blaster Redesign

Nerf Blaster Redesign Nerf Blaster Redesign ME4041 Computer Graphics and CAD April 0, 010 Submitted By: Michael Schulman Greg Mann Table of Contents Introduction. Objectives Modeling. 4 External Components 4 Internal Components.

More information

Beams. Lesson Objectives:

Beams. Lesson Objectives: Beams Lesson Objectives: 1) Derive the member local stiffness values for two-dimensional beam members. 2) Assemble the local stiffness matrix into global coordinates. 3) Assemble the structural stiffness

More information

Automation of Static and Dynamic FEA Analysis of Bottomhole Assemblies

Automation of Static and Dynamic FEA Analysis of Bottomhole Assemblies Automation of Static and Dynamic FEA Analysis of Bottomhole Assemblies Nader E. Abedrabbo, Lev Ring & Raju Gandikota 1 Weatherford International 11909 Spencer Road, Houston, TX nader.abedrabbo@weatherford.com

More information

Structural Design Code Verifier. Be an analyst not an admin

Structural Design Code Verifier. Be an analyst not an admin Structural Design Code Verifier Be an analyst not an admin SDC Verifier Embedded 2 Separate GUI What is SDC Verifier? The goal of SDC Verifier is checking structures according to standards and report generation.

More information