Automation of Static and Dynamic FEA Analysis of Bottomhole Assemblies
|
|
- Roderick Johns
- 6 years ago
- Views:
Transcription
1 Automation of Static and Dynamic FEA Analysis of Bottomhole Assemblies Nader E. Abedrabbo, Lev Ring & Raju Gandikota 1 Weatherford International Spencer Road, Houston, TX nader.abedrabbo@weatherford.com Abstract: A lower portion of the drillstring used in drilling for oil and gas is called bottomhole assembly (BHA). Drilling forces and vibrations have a great impact not only on the rate of drilling, but also on the survivability of the equipment. Therefore, it is critical to perform detailed analysis on every BHA system to predict critical dynamic behavior and minimize failures. There are several challenges in applying finite element analysis to such problems. The ratio of the length to the diameter is in the order of Beam elements provide a good approximation and result in acceptable combination of accuracy and solution time. However, each BHA model could consist of hundreds of small parts with different section and profile definitions. Contact definition for beam elements and drillstring instabilities pose another complication. An automated method was developed to assist in creating any BHA system from three files: BHA components, well survey and wellbore IDs. Using these, a complete Abaqus input file can be created for each BHA at any location in the well in a matter of seconds. A complete user interface was also created for specifying multiple input parameters, generating input files and then to run and monitor the analysis. The developed GUI allows engineers who are not familiar with FEA and Abaqus to conduct complex static and dynamic analysis. A Standalone post-processor was also developed to automatically extract required data from the ODB file in order to report and view the results in a manner consistent with industry standards. Keywords: Automation, Bottomhole Assembly, BHA, Bending, Buckling, Drilling, Dynamics, Wellbore, Oil Industry. 1. Introduction A lower portion of the drillstring used in drilling for oil and gas is called bottomhole assembly (BHA). The BHA consists of a combination of very sophisticated and expensive equipment that is designed to stabilize and direct (navigate) the drill bit to a specific target depth and horizontal deviation (directional drilling) while simultaneously performing real time geophysical measurements (logging-while-drilling). A typical BHA ranged between 500 and 600 feet in length. Figure 1 shows a sample BHA and Figure 2 shows the list of components for the same BHA. Drilling forces and vibrations that occur during drilling operations have great impact not only on the rate of drilling, but also on the survivability of the downhole equipment. Therefore, it is essential to perform detailed analysis on every BHA system in order to predict critical dynamic behavior and minimize premature failures.
2 Figure 1. Schematic of a BHA showing the composition of different parts with different sections. Figure 2. Component list of the parts making the sample BHA shown in Figure 1. 2
3 There are several challenges in efficiently applying finite element analysis to such models. The ratio of the model length to the typical diameter is in the order of 10 5 which prohibit using shell and solid elements. Another complication is the presence of multiple and variable areas of contact between drillstring and borehole as well as potential drillstring instabilities (i.e., buckling behavior). Choice of beam elements usually provides a good approximation to the geometry and stress distribution, resulting in acceptable combination of accuracy and solution time. Some modeling challenges are specific to Abaqus [1]. Each BHA model consists of hundreds of small parts with different section and profile definitions. The process of defining contacts in Abaqus using the ITT contact elements (beam-to-beam) is not supported in Abaqus/CAE. Creating a single BHA model using a combination of Abaqus/CAE and manual scripting to prepare the input file could take days to construct. In order to automate and accelerate the analysis, an automated method was developed to assist in creating the BHA systems from three simple input files: BHA component list, well survey and wellbore inner diameter definitions. Using these files, a complete Abaqus input file can be created for each BHA at any location in the well in a matter of seconds. A complete user interface (GUI) was also created for specifying a variety of input parameters, generating Abaqus input files and then running and monitoring the Abaqus analysis. This GUI allows engineers who are not familiar with FEA and Abaqus to conduct complex static and dynamic analysis during pre-job planning and identify root causes of potential field problems. A Standalone post-processor was also developed to extract the required data directly from the ODB file in order to report and view the results in a manner consistent with industry standards. 2. BHA Development in Abaqus/CAE In a drilling procedure, the drilling bit has the largest outer diameter (OD) of all the BHA components. Stabilizers, which have a close-to-gage OD, are added at key locations in the BHA composition in order to provide stability and support for the long BHA. Other components of the BHA (e.g. drill pipes, collars, subs) have varying outer diameters that are usually smaller than the bit and stabilizer OD s. Typically, failures occur due to high bending stresses as well as high vibrations occurring during the drilling procedure. To mitigate these problems, static and dynamic analysis of bottomhole assemblies is frequently conducted before a drilling job is performed to ensure that the drilling forces and vibrations experienced by the BHA components are within acceptable tolerances. If the analysis reveals higher stresses, certain measures can be used to reduce these effects (e.g. installing extra stabilizers, reducing drilling speed). One other factor that affects the BHA s response to static and dynamic forces is the location (i.e. orientation) of the BHA in the well. During drilling, the BHA transitions through different locations based on well planning. As the BHA orientation changes, the static and dynamic forces experienced by the BHA also change. Therefore, it is imperative to perform the required analysis on the BHA in different orientations in the well in order to ensure that a configuration in one orientation that passed the safety limits would not experience higher forces in a different one. Figure 3 shows a side view schematic of a planned well. The dots on the line highlighted by the arrows indicate the positions in the well where static and dynamic analysis must be performed. 3
4 Horizontal Position (ft) True Vertical Depth (ft) Positions in well to perform analysis Figure 3. Well profile section indicating locations where BHA is to be analyzed. Due to the ratio of the BHA system length to the typical diameter, beam elements offer the best approach of both accuracy and fast solution time. Beam elements are used to define both the BHA components and the well profile geometry. Contact between the BHA and the well is achieved by using the beam-to-beam contact elements (ITT). In order to define a BHA component in Abaqus and maintain cross sectional accuracy, each component making up the BHA is divided into smaller pipe sections representing the different outer diameter differences. Figure 4 shows a sample BHA part (heavy weight drill pipe) where it has been divided into five separate cylindrical sections, each representing a different OD (typically ID s are similar for a single part). Some of the sections are similar, but they are separated by nonsimilar parts. These different sections need to be represented individually in Abaqus. Section 1 Section 2 Section 3 Section 4 Section 5 Figure 4. BHA part (heavy weight drill pipe) divided into its different section representation in Abaqus. Dimensionally equal parts are indicated. 4
5 The process of creating a beam definition of a BHA system in Abaqus/CAE involves the following: 1. Define the geometry of the whole BHA in Abaqus/CAE Sketcher. In this scheme, the BHA is drawn as a single beam with multiple sections. Each beam section length corresponds to that of a section of the parts making the BHA (see Figure 4). Using this scheme eliminates the need to define elements connecting the different components consequently overhead creation costs are reduced. 2. Define beam profiles using one of the predefined cross section definitions (e.g. tube, circle or the general beam definition method). In the definition, assign the OD and ID of each beam section. 3. Define beam section properties and associate material (e.g. Poisson s ratio) to the beam profile. 4. Associate each section of the BHA system to its appropriate beam section definition. A typical BHA could potentially consist of hundreds of subsections for all its parts. For example, one of the BHA systems currently being analyzed has the following definition: 1. Total number of parts: Subsections for all parts: 93 + well section definitions 3. Total beam and cross section definitions required to represent the BHA: well section definitions After defining the BHA and all its components and manually associating the beam sections to the beam elements, the contact definition between the BHA parts and the well needs to be provided. Since the model is being solved using the Dynamic Implicit approach, the only contact definition available in Abaqus/Implicit is the beam-to-beam contact (e.g. ITT31). These beam definitions, however, are not currently supported in Abaqus/CAE. Manual scripting of the input file must be performed instead. The beam-to-beam contact for beam elements simulates the contact between the OD of each BHA part and the ID/s of the well. Since the BHA is composed of multiple parts with unique ODs, each section of the BHA must have its own beam contact definition. For each contact definition, the interface value, which is the difference between the inner radius of the well and the outer radius of the part, must be supplied in addition to other definitions. Figure 5 shows a sample beam-2-beam contact definition for a single section of the BHA. For the sample BHA described above, a total of 75 beam contact definitions were required to be coded manually. A critical issue that affects the manual definition of beam contacts in Abaqus is the node numbering scheme. Abaqus/CAE tends to assign node numbers to the ends of the beam segments composing the BHA first, then, when all major segments of the line have been assigned, node numbers for the inner regions of the sections are assigned. Abaqus/CAE does not provide a method to renumber nodes in a linear progressive fashion. This numbering scheme further complicates the contact definition for beam elements as shown in Figure 5. The user must keep track and manage differing node numbers increasing the likelihood of confusion and errors. Additionally, this node numbering scheme creates problems when post processing the analysis results as it is difficult to track the OD of each node. 5
6 *************************************************************** *** ITT31 - SLIDE LINE INTERACTIONS FOR BHA AND WELL *** *************************************************************** *ELEMENT, TYPE=ITT31, ELSET=TUBE_SL_ , 1 *ELGEN, ELSET=TUBE_SL_ , 6, 1, 1 *SLIDE LINE, ELSET=TUBE_SL_1, TYPE=LINEAR, GENERATE, SMOOTH= , 796, 1 *INTERFACE, ELSET=TUBE_SL_1, NAME=ISL_ , *FRICTION 0.1, *SURFACE BEHAVIOR, PRESSURE-OVERCLOSURE=EXPONENTIAL 0.001, Figure 5. Beam-to-beam contact definition for a single section of the BHA. Another significant issue exists with using the manual method to define beam elements for a BHA in Abaqus/CAE. As described earlier, the BHA must be analyzed at different location in the well. As shown in Figure 3, not all positions in the well conform to a straight line. Analysis locations in the well may include BHA systems that are partially or even completely curved. Creating a curved beam of the BHA components while accounting for the exact lengths of each section or part is nearly impossible to do manually. One solution to this problem is to start each analysis with the BHA in a vertical position, dynamically insert the BHA to the required position, stop the analysis, and finally perform a static analysis in this position. Using this approach, however, is both time consuming, and creates more work load. In the BHA example described previously and illustrated in the last point of Figure 3, the analysis took two days to dynamically insert the BHA to the required position. This solution time is prohibitive especially when the analysis must be conducted for several locations and for multiple BHA configurations. Assuming all the previous manual definition limiting issues were resolved, constructing the input file for Abaqus using a combination of Abaqus/CAE and manual editing would require at least two days for each BHA system and for each test position within those systems (for positions shown in Figure 3). In order to build, test, and analyze multiple configurations rapidly and effectively, an automated method is required to speed up the FEA analysis. 3. Motivation At Weatherford International and in the oil industry in general, bottomhole assembly analysis is currently conducted using proprietary third party programs. These programs, however, suffer from several limitations (as reported by our users and personal testing): 1. Majority of the programs only give limited output results regarding the behavior of the BHA. For example, the deformed shape of the BHA in one plane, usually the lateral 6
7 axes, is only supplied. In order to accurately predict helical and sinusoidal buckling, however, viewing the out-of-plane deformed shape of the BHA is a necessity. 2. The ability to extract the analysis results in text or CSV file formats is limited. 3. One of the major problems with these programs is that they limit the length (or divisions) of the BHA being analyzed. For example, one of the programs currently in use relies on a student version of ANSYS as a solver. Due to this fact, the user is limited to a small number of nodes that can be used to describe the BHA and the well (500 node limit). Because of this limitation, the users are forced to reduce both the length and complexity of the BHA system being analyzed by limiting the number of varying OD and ID sections. The more complex the system being studied, the shorter the length of the BHA must be for the analysis to run. The reduction in BHA complexity limits the amount of useful information available to accurately analyze BHA systems. 4. Some of these programs suffer from major bugs and crash incidents. One of the programs currently in use suffers from a crash rate of 50%. 5. As mentioned earlier, every BHA must be analyzed at different locations in the well as shown in Figure 3. However, most the programs currently in use do not use the real well trajectory to position the BHA for the analysis. Instead, they rely on a very short description of the well. In this description, the BHA is either in the vertical, horizontal or completely curved (i.e., arc) position. This description, although useful, does not accurately describe the actual well in use, especially for conditions where the BHA is in a non-uniform well. 4. Development Requirements With these shortcomings of current BHA analysis programs in mind, future developed procedures for analyzing BHA s using Abaqus FEA should satisfy the following criteria: 1. FEA (and Abaqus) Knowledge: Users with limited to no knowledge of the FEA process or Abaqus should be able to use the program with ease. 2. Usability: The BHA and all its complex components must be created with ease and with minimum user effort. Also, no limitations on BHA lengths being analyzed should be imposed. 3. Flexibility: The developed methods must have the ability to apply different boundary conditions based on the analysis type and create different test scenarios quickly (e.g. static analysis at different locations in the well). 4. Accuracy: The FEA analysis must be able to run to completion with minimal code crashes and produce accurate results. 5. Post-Processing: The user should have the ability to extract the desired results from the analysis ODB file and plot them in a fashion close to other programs for easy comparison. 7
8 5. Developed Solution Based on the requirements stated above, a standalone program (GUI) was developed for the creation and analysis of bottomhole assemblies which uses Abaqus FEA as a solver engine. The developed program with its standalone GUI was developed using the Python programing language [2]. Also, a post-processor was developed where the required output results are extracted directly from the Abaqus ODB results file using a Python script. The extracted data is then manipulated and the post-processor is used to display the analysis results in the required format. After generating the required input files for Abaqus, the developed program then calls the Abaqus FEA solver to perform the required analysis from within the GUI. Monitoring of the progress of the analysis is also provided. In the developed program, a complete input file for Abaqus can be generated for any BHA system at any position in the well (e.g. horizontal, vertical, curved or in-between) in less than two seconds, compared to more than two days using a combination of Abaqus/CAE and manual editing (if feasible). Running the analysis to solve the BHA problem (Implicit Dynamic step followed by a Static step) takes between 10 to 45 minutes, depending on the location of the BHA in the well. 5.1 Procedures The developed procedure for generating the required BHA input files for Abaqus in any location in the well and also for post-processing of the results is as follows: 1. General Settings: In this window (as shown in Figure 6), the user specifies all the necessary information and boundary conditions for the analysis: a. Solution directory; b. Project name which is used in naming of the (*.inp) files for easy identification. c. Analysis type: i. Static Analysis: This is used to perform the static analysis of the BHA. The analysis is achieved using a multiple step procedure combining an Implicit/Dynamic step followed by an Implicit/Static step. ii. Buckle Analysis: This is used to generate imperfections to be included in the Static Analysis step in order to improve buckling predictions. iii. Frequency Analysis: This is used to extract the eigenvalues and modes of the model. Contact between BHA parts and the wellbore are enforced using BC definitions. d. Boundary conditions: The user can specify all the necessary boundary conditions for the analysis. For example: i. Fix top of BHA: The drill bit is usually fixed to the centerline of the wellbore. The user can also choose to fix the top of the BHA to the centerline, in which case only lateral movement will be allowed. 8
9 ii. Test MD: As shown in Figure 3, this is the position in the well where the analysis is to be performed. iii. WOB: This is the weight on bit that is to be applied as an axial force to the top of the BHA. iv. Other boundary conditions Figure 6. General setting window of the developed GUI. 2. Well Survey: In this window, the user supplies the well survey information in the spherical coordinate system: Measured Depth, Inclination and Azimuth. In order for the well survey data to be used in the finite element method, the spherical coordinate data must be converted into the Cartesian coordinate system. This is achieved internally in the program using the Minimum Curvature Method [3]. After conversion, several plots are provided of the well survey for better visualization (e.g. 3D, side view, planar view). Figure 7 shows a 3D plot of a sample well. 9
10 Figure 7. 3D plot a sample survey data after being converted into real coordinates. 3. Well Intervals: In this window, the user supplies the well inner diameters. Some wellbores can have multiple inner diameters; therefore, the inner diameter of the well is supplied as a function of measured depth. A plot is also provided to the user for better visualization of the well inner diameters as shown in Figure 8. Figure 8. Well intervals input showing inner diameter as a function of depth. 10
11 4. BHA Breakdown: In this window the user defines the composition of each component of the BHA. Each BHA part is divided into its subsections based on outer diameter as described in Figure 4. For some parts (e.g. drill pipe, heavy weight drill pipes), a built-in database has been developed such that the user only needs to specify the part name and nominal outer diameter to identify the part. Two plots are also supplied for the user in order to review the composition of the BHA: 2D sectional view and 3D view. Figure 9 shows the BHA breakdown of a sample BHA system. A plot of the cross section of the parts is also shown. Figure 9. Breakdown of BHA components into subsections. 5. Generate Abaqus Input Files: After the user supplies all the necessary information about the well, BHA components, required analysis type and boundary conditions, the Abaqus input files can be generated. As seen in Figure 10, generation of the input files for the system illustrated in Figure 9 based was accomplished in 1.25 seconds. 6. Run Abaqus Analysis: When the input files have been generated based on the supplied data, the user can run the Abaqus analysis from within the GUI. The user has the ability also to select the number of CPUs to use for the Analysis. The state and progress of the analysis can be monitored using the Event Log window and also through the utilization of progress bars. Figure 11 shows an example of a case being solved using Abaqus solver and the solution monitored within the GUI. 11
12 Figure 10. Generation of Abaqus input files based on supplied data. Building complete Abaqus input files for the model was accomplished in 1.25 sec. Figure 11. Running of Abaqus analysis and monitoring of the analysis is done from within the GUI. 12
13 7. Post-Processing: After the model is analyzed using Abaqus solver, post-processing of the data in a format that is easy to understand by the users is necessary. Due to the fact that the ratio of the model length to the typical diameter is in the order of 10 5, viewing of a model that is 500ft long in Abaqus/CAE does not produce useful viewable information. Figure 12 shows the result from a sample BHA analysis using Abaqus/CAE. The beam profile rendering was activated with a magnification scale factor of 10. Figure 12 clearly illustrates that even with the magnification, the BHA deformations are not easy to visualize in the current format. Figure 12. BHA analysis result of the sample BHA in Figure 1 as viewed in Abaqus/CAE. The beam profile is magnified by a scale factor of 10. Furthermore, the extraction of several required variables in the Abaqus/CAE postprocessor, while possible, is time-consuming. In order to extract the results of the analysis and view them in a usable format, a standalone post-processor was developed. All required analysis results are extracted from the ODB file using a specially written Python script file. When the analysis is completed, the user then calls the analysis extraction module where the ODB file is supplied. The data from the ODB file is extracted and saved to a special file. The extracted analysis results is then viewed in the post-processor. In order to view the long BHA in a useful format, the post-processor automatically manipulates the BHA from its original curved or vertical position to a straight, horizontal 13
14 orientation. This allows the deformations in the BHA to be viewed in a much clearer format than shown in Figure 12. Two views are shown for the BHA: front cross-section view and top cross section view. In this format, sinusoidal and helical buckling in the BHA can be easily visualized. Also, the ability to project the von Mises stresses in contour format can be projected on the cross section as shown in Figure 13. The post-processor displays a list of data values that can be viewed alongside the deformed BHA shape. The user can also extract the name of each part in the list by mouse clicking on the plots for easy identification of parts. Figure 13 shows a sample result for the BHA as illustrated in Figure 9. Only the first 250 feet of the BHA is shown. Figure 12. BHA analysis result of the sample BHA in Figure 9 as viewed in Abaqus/CAE. The beam profile is magnified by a scale factor of 10. For the frequency analysis capability, the post-processor shows the natural modes of the solved system in multiple formats. One of the more useful views is the 3D plot, which has the ability to apply the beam profile rendering as well as a scale factor for the deformation intensity of the modes. Figure 13 shows a sample natural mode (mode #14) for the previous system with a deformation scale factor of 30. The post-processor also offers the ability to export all plot data to CSV files if required by the user. 14
15 Figure 13. Natural modes of the sample BHA shown in Figure 9 for mode # Conclusion A standalone user interface was developed that allows an engineer, even one with little or no knowledge of Abaqus or FEA, to perform detailed FEA analysis of a bottomhole assembly. By supplying the program with required input data, the GUI builds complete input files for a BHA, including nodes, elements, contacts and step definitions. The program further allows the user to run the analysis using Abaqus as a solver. When the analysis is completed, the program automatically extracts all the required results from the ODB file. Finally, a standalone postprocessor was also developed to view the analysis results in a usable format. The developed user interface, analysis procedure, and post-processor described in this paper will result in increased speed, efficiency, and accuracy in analyzing bottomhole assemblies with efficiency. 7. References [1] Abaqus is a product of Dassault Systèmes Simulia Corp., Providence, RI, USA. [2] [3] 15
Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE
Getting Started with Abaqus: Interactive Edition Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE The following section is a basic tutorial for the experienced Abaqus user. It leads you
More informationME 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 informationTorsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10
Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10 This document contains an Abaqus tutorial for performing a buckling analysis using the finite element program
More informationCreating and Analyzing a Simple Model in Abaqus/CAE
Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE The following section is a basic tutorial for the experienced Abaqus user. It leads you through the Abaqus/CAE modeling process by visiting
More informationProceedings of the ASME th Biennial Conference On Engineering Systems Design And Analysis ESDA2012 July 2-4, 2012, Nantes, France
Proceedings of the ASME 2012 11th Biennial Conference On Engineering Systems Design And Analysis ESDA2012 July 2-4 2012 Nantes France ESDA2012-82316 A MULTIBODY SYSTEM APPROACH TO DRILL STRING DYNAMICS
More informationWorkshop 15. Single Pass Rolling of a Thick Plate
Introduction Workshop 15 Single Pass Rolling of a Thick Plate Rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. The rolling process
More informationAnalysis Steps 1. Start Abaqus and choose to create a new model database
Source: Online tutorials for ABAQUS Problem Description The two dimensional bridge structure, which consists of steel T sections (b=0.25, h=0.25, I=0.125, t f =t w =0.05), is simply supported at its lower
More informationAbaqus/CAE Axisymmetric Tutorial (Version 2016)
Abaqus/CAE Axisymmetric Tutorial (Version 2016) Problem Description A round bar with tapered diameter has a total load of 1000 N applied to its top face. The bottom of the bar is completely fixed. Determine
More informationEN1740 Computer Aided Visualization and Design Spring /26/2012 Brian C. P. Burke
EN1740 Computer Aided Visualization and Design Spring 2012 4/26/2012 Brian C. P. Burke Last time: More motion analysis with Pro/E Tonight: Introduction to external analysis products ABAQUS External Analysis
More informationInstallation Guide. Beginners guide to structural analysis
Installation Guide To install Abaqus, students at the School of Civil Engineering, Sohngaardsholmsvej 57, should log on to \\studserver, whereas the staff at the Department of Civil Engineering should
More informationSIMULATING PERFORATING SHOCK ON AN INTELLIGENT COMPLETIONS INTERVAL CONTROL VALVE
2016 INTERNATIONAL PERFORATING SYMPOSIUM GALVESTON SIMULATING PERFORATING SHOCK ON AN INTELLIGENT COMPLETIONS INTERVAL CONTROL VALVE May 10TH, 2016 AUTHOR: Jim Wight Halliburton 2016 Halliburton. All Rights
More information2. MODELING A MIXING ELBOW (2-D)
MODELING A MIXING ELBOW (2-D) 2. MODELING A MIXING ELBOW (2-D) In this tutorial, you will use GAMBIT to create the geometry for a mixing elbow and then generate a mesh. The mixing elbow configuration is
More informationFinite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam
Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam Consider the beam in the figure below. It is clamped on the left side and has a point force of 8kN acting
More informationCoupled 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 informationGlobal to Local Model Interface for Deepwater Top Tension Risers
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
More informationAbaqus/CAE (ver. 6.11) Nonlinear Buckling Tutorial
Abaqus/CAE (ver. 6.11) Nonlinear Buckling Tutorial Problem Description This is the NAFEMS 1 proposed benchmark (Lee s frame buckling) problem. The applied load is based on the normalized (EI/L 2 ) value
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
Problem Description: FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Dimitri Soteropoulos Programs Utilized: Abaqus/CAE 6.11-2 This tutorial explains how to build
More informationThis tutorial will take you all the steps required to set up and run a basic simulation using ABAQUS/CAE and visualize the results;
ENGN 1750: Advanced Mechanics of Solids ABAQUS TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to set up and run a basic simulation using ABAQUS/CAE and
More informationTRINITAS. a Finite Element stand-alone tool for Conceptual design, Optimization and General finite element analysis. Introductional Manual
TRINITAS a Finite Element stand-alone tool for Conceptual design, Optimization and General finite element analysis Introductional Manual Bo Torstenfelt Contents 1 Introduction 1 2 Starting the Program
More informationAbaqus/CAE (ver. 6.9) Vibrations Tutorial
Abaqus/CAE (ver. 6.9) Vibrations Tutorial Problem Description The two dimensional bridge structure, which consists of steel T sections, is simply supported at its lower corners. Determine the first 10
More informationAbaqus/CAE (ver. 6.12) Vibrations Tutorial
Abaqus/CAE (ver. 6.12) Vibrations Tutorial Problem Description The two dimensional bridge structure, which consists of steel T sections, is simply supported at its lower corners. Determine the first 10
More informationCam makes a higher kinematic pair with follower. Cam mechanisms are widely used because with them, different types of motion can be possible.
CAM MECHANISMS Cam makes a higher kinematic pair with follower. Cam mechanisms are widely used because with them, different types of motion can be possible. Cams can provide unusual and irregular motions
More informationStructural Analysis of an Aluminum Spiral Staircase. EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen
Structural Analysis of an Aluminum Spiral Staircase EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen Abstract An old aluminum spiral staircase at Marcos home has been feeling really
More informationSliding Split Tube Telescope
LESSON 15 Sliding Split Tube Telescope Objectives: Shell-to-shell contact -accounting for shell thickness. Creating boundary conditions and loads by way of rigid surfaces. Simulate large displacements,
More informationSimLab 14.3 Release Notes
SimLab 14.3 Release Notes Highlights SimLab 14.0 introduced new graphical user interface and since then this has evolved continuously in subsequent versions. In addition, many new core features have been
More informationThis tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
ENGN 1750: Advanced Mechanics of Solids ABAQUS CAD INTERFACE TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
More informationIntroduction to Solid Modeling Parametric Modeling. Mechanical Engineering Dept.
Introduction to Solid Modeling Parametric Modeling 1 Why draw 3D Models? 3D models are easier to interpret. Simulation under real-life conditions. Less expensive than building a physical model. 3D models
More informationExercise 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 information3. MODELING A THREE-PIPE INTERSECTION (3-D)
3. MODELING A THREE-PIPE INTERSECTION (3-D) This tutorial employs primitives that is, predefined GAMBIT modeling components and procedures. There are two types of GAMBIT primitives: Geometry Mesh Geometry
More informationAbaqus 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 informationSimulation of Laminar Pipe Flows
Simulation of Laminar Pipe Flows 57:020 Mechanics of Fluids and Transport Processes CFD PRELAB 1 By Timur Dogan, Michael Conger, Maysam Mousaviraad, Tao Xing and Fred Stern IIHR-Hydroscience & Engineering
More informationDevelopment of a Durable Automotive Bushing with fe-safe/rubber
Development of a Durable Automotive Bushing with fe-safe/rubber Jing Bi, Gergana Dimitrova, Sandy Eyl Dassault Systemes Simulia Corp 1301 Atwood Ave, Suite 101W, Johnston RI 02919 Abstract Fatigue life
More informationTutorial 1. A the end of the tutorial you should be able to
CUFSM 2.5 Tutorial 1 Default Cee section in bending Objective To introduce CUFSM and the finite strip method and gain a rudimentary understanding of how to perform an analysis and interpret the results.
More informationIntroduction to Abaqus. About this Course
Introduction to Abaqus R 6.12 About this Course Course objectives Upon completion of this course you will be able to: Use Abaqus/CAE to create complete finite element models. Use Abaqus/CAE to submit and
More informationDMU Engineering Analysis Review
Page 1 DMU Engineering Analysis Review Preface Using This Guide Where to Find More Information Conventions What's New? Getting Started Inserting a CATAnalysis Document Using DMU Space Analysis From CATAnalysis
More informationFOUNDATION IN OVERCONSOLIDATED CLAY
1 FOUNDATION IN OVERCONSOLIDATED CLAY In this chapter a first application of PLAXIS 3D is considered, namely the settlement of a foundation in clay. This is the first step in becoming familiar with the
More informationAXIAL OF OF THE. M. W. Hyer. To mitigate the. Virginia. SUMMARY. the buckling. circumference, Because of their. could.
IMPROVEMENT OF THE AXIAL BUCKLING CAPACITY OF COMPOSITE ELLIPTICAL CYLINDRICAL SHELLS M. W. Hyer Department of Engineering Science and Mechanics (0219) Virginia Polytechnic Institute and State University
More informationABAQUS/CAE Workshops
ABAQUS/CAE Workshops University of Birmingham ABAQUS Training 27 th / 28 th October 2009 Workshop 1a: Create 3D Part Type: abaqus cae at the command prompt or select abaqus V6.9-1 from the start menu.
More informationIntroduction to Abaqus/CAE. About this Course. Course objectives. Target audience. Prerequisites
Introduction to Abaqus/CAE R 6.12 About this Course Course objectives Upon completion of this course you will be able to: Use Abaqus/CAE to create complete finite element models. Use Abaqus/CAE to submit
More informationCoke Drum Laser Profiling
International Workshop on SMART MATERIALS, STRUCTURES NDT in Canada 2013Conference & NDT for the Energy Industry October 7-10, 2013 Calgary, Alberta, CANADA Coke Drum Laser Profiling Mike Bazzi 1, Gilbert
More informationAADE-05-NTCE-67. A Gravity-Based Measurement-While-Drilling Technique Determines Borehole Azimuth From Toolface and Inclination Measurements
AADE-05-NTCE-67 A Gravity-Based Measurement-While-Drilling Technique Determines Borehole Azimuth From Toolface and Inclination Measurements Herbert Illfelder, Ken Hamlin, Graham McElhinney - PathFinder
More informationSIMULATION CAPABILITIES IN CREO
SIMULATION CAPABILITIES IN CREO Enhance Your Product Design with Simulation & Using digital prototypes to understand how your designs perform in real-world conditions is vital to your product development
More information2: Static analysis of a plate
2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors
More informationABAQUS for CATIA V5 Tutorials
ABAQUS for CATIA V5 Tutorials AFC V2.5 Nader G. Zamani University of Windsor Shuvra Das University of Detroit Mercy SDC PUBLICATIONS Schroff Development Corporation www.schroff.com ABAQUS for CATIA V5,
More informationAbaqus 6.9SE Handout
MANE 4240/ CIVL 4240: Introduction to Finite Elements Abaqus 6.9SE Handout Professor Suvranu De Department of Mechanical, Aerospace and Nuclear Engineering Rensselaer Polytechnic Institute Table of Contents
More informationApplication of Predictive Engineering Tool (ABAQUS) to Determine Optimize Rubber Door Harness Grommet Design
Application of Predictive Engineering Tool (ABAQUS) to Determine Optimize Rubber Door Harness Grommet Design Praveen Mishra, Dayananda Gowda Mercedes Benz R & D India, Bangalore, Karnataka, India Abstract:
More information3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
More informationRecent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper
More informationCATIA V5 FEA Tutorials Release 14
CATIA V5 FEA Tutorials Release 14 Nader G. Zamani University of Windsor SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com CATIA V5 FEA Tutorials 2-1 Chapter 2 Analysis
More informationME Optimization of a Truss
ME 475 - Optimization of a Truss Analysis Problem Statement: The following problem will be analyzed using Abaqus and optimized using HEEDS. 4 5 8 2 11 3 10 6 9 1 7 12 6 m 300 kn 300 kn 22 m 35 m Figure
More informationCE366/ME380 Finite Elements in Applied Mechanics I Fall 2007
CE366/ME380 Finite Elements in Applied Mechanics I Fall 2007 FE Project 1: 2D Plane Stress Analysis of acantilever Beam (Due date =TBD) Figure 1 shows a cantilever beam that is subjected to a concentrated
More informationMASTA 9.0 Release Notes
November 2018 2018 Smart Manufacturing Technology Ltd. Commercial in Confidence Page 1 of 33 MASTA 9.0 Contents and Summary See next section for additional details The 9.0 release of MASTA contains all
More informationIntroduction to Nastran SOL 200 Design Sensitivity and Optimization
Introduction to Nastran SOL 200 Design Sensitivity and Optimization PRESENTED BY: CHRISTIAN APARICIO The Nastran Engineering SOL 200 questions? Lab Email me: christian@ the-engineering-lab.com Motivation
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More informationShape and parameter optimization with ANSA and LS-OPT using a new flexible interface
IT / CAE Prozesse I Shape and parameter optimization with ANSA and LS-OPT using a new flexible interface Korbetis Georgios BETA CAE Systems S.A., Thessaloniki, Greece Summary: Optimization techniques becomes
More informationModeling Submerged Structures Loaded by Underwater Explosions with ABAQUS/Explicit
Modeling Submerged Structures Loaded by Underwater Explosions with ABAQUS/Explicit David B. Woyak ABAQUS Solutions Northeast, LLC Abstract: Finite element analysis can be used to predict the transient
More informationSelective Space Structures Manual
Selective Space Structures Manual February 2017 CONTENTS 1 Contents 1 Overview and Concept 4 1.1 General Concept........................... 4 1.2 Modules................................ 6 2 The 3S Generator
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationLinear Bifurcation Buckling Analysis of Thin Plate
LESSON 13a Linear Bifurcation Buckling Analysis of Thin Plate Objectives: Construct a quarter model of a simply supported plate. Place an edge load on the plate. Run an Advanced FEA bifurcation buckling
More informationAbaqus/CAE (ver. 6.10) Stringer Tutorial
Abaqus/CAE (ver. 6.10) Stringer Tutorial Problem Description A table made of steel tubing with a solid steel top and shelf is loaded with an oblique impulse load. Determine the transient response of the
More informationLive Classroom Curriculum Guide
Curriculum Guide Live Classroom Curriculum Guide Milling using Pro/ENGINEER Wildfire 4.0 Pro/ENGINEER Mechanica Simulation using Pro/ENGINEER Wildfire 4.0 Introduction to Pro/ENGINEER Wildfire 4.0 Pro/ENGINEER
More informationModule 1.6: Distributed Loading of a 2D Cantilever Beam
Module 1.6: Distributed Loading of a 2D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing
More informationPTC 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 informationModelling Tube-to-Tube contact in Abaqus using Part and Instance
Modelling Tube-to-Tube contact in Abaqus using Part and Instance Key Words: Abaqus, ITT21 or ITT31, *Interface, *Slide Line, Tube-to-Tube, Tube in Tube contact When using Abaqus CAE, and especially Native
More informationChapter 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 informationFinite element representations of crash
Optimization of Material Parameters for Crash Test Dummies George Scarlat Sridhar Sankar Simulia Corp. Providence, R.I. process automation and design optimization software makes it easier to identify optimal
More informationNon-Parametric Optimization in Abaqus
Non-Parametric Optimization in Abaqus 2016 About this Course Course objectives Upon completion of this course you will be able to: Apply topology, shape, sizing and bead optimization techniques to your
More informationpre- & post-processing f o r p o w e r t r a i n
pre- & post-processing f o r p o w e r t r a i n www.beta-cae.com With its complete solutions for meshing, assembly, contacts definition and boundary conditions setup, ANSA becomes the most efficient and
More informationTrajectory and Window Width Prediction for a Cased Hole Sidetrack using a Whipstock
AADE-05-NTCE-52 Trajectory and Window Width Prediction for a Cased Hole Sidetrack using a Whipstock Harshad Patil, Smith Services Smith International, Inc. Dr. John Rogers Smith, Louisiana State University
More informationUsing three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model
Boundary Elements XXVII 245 Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model J. J. Rencis & S. R. Pisani Department of Mechanical Engineering,
More informationME 442. Marc/Mentat-2011 Tutorial-1
ME 442 Overview Marc/Mentat-2011 Tutorial-1 The purpose of this tutorial is to introduce the new user to the MSC/MARC/MENTAT finite element program. It should take about one hour to complete. The MARC/MENTAT
More informationSimilar Pulley Wheel Description J.E. Akin, Rice University
Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated
More informationClick here to be a Dips 7.0 Beta Tester! 3D Stereosphere. Contour Arbitrary Data on Stereonet. Curved Boreholes. Intersection Calculator
DIPS7.0 It s been 3 years since the release of Dips 6.0, so it s time for an upgrade! The latest version of our popular stereonet program - Dips 7.0 - is scheduled for release in early 2016. If you would
More informationPiping Design. Site Map Preface Getting Started Basic Tasks Advanced Tasks Customizing Workbench Description Index
Piping Design Site Map Preface Getting Started Basic Tasks Advanced Tasks Customizing Workbench Description Index Dassault Systèmes 1994-2001. All rights reserved. Site Map Piping Design member member
More informationVerification of Laminar and Validation of Turbulent Pipe Flows
1 Verification of Laminar and Validation of Turbulent Pipe Flows 1. Purpose ME:5160 Intermediate Mechanics of Fluids CFD LAB 1 (ANSYS 18.1; Last Updated: Aug. 1, 2017) By Timur Dogan, Michael Conger, Dong-Hwan
More informationMAE 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 informationTopology Optimization and Analysis of Crane Hook Model
RESEARCH ARTICLE Topology Optimization and Analysis of Crane Hook Model Thejomurthy M.C 1, D.S Ramakrishn 2 1 Dept. of Mechanical engineering, CIT, Gubbi, 572216, India 2 Dept. of Mechanical engineering,
More informationLatch Spring. Problem:
Problem: Shown in the figure is a 12-gauge (0.1094 in) by 3/4 in latching spring which supports a load of F = 3 lb. The inside radius of the bend is 1/8 in. Estimate the stresses at the inner and outer
More informationOverview of ABAQUS II. Working with Geometry in ABAQUS III. Working with models Created Outside ABAQUS IV. Material and Section Properties
ABAQUS TRAINING I. Overview of ABAQUS II. Working with Geometry in ABAQUS III. Working with models Created Outside ABAQUS IV. Material and Section Properties V. Assemblies in ABAQUS VI. Steps, Output,
More informationIntroduction to Electrostatic FEA with BELA
Introduction to Electrostatic FEA with BELA David Meeker dmeeker@ieee.org Updated October 31, 2004 Introduction BELA ( Basic Electrostatic Analysis ) is a software package for the finite element analysis
More informationBell Crank. Problem: Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed (New York: McGraw Hill, May 2002) page 87.
Problem: A cast-iron bell-crank lever, depicted in the figure below is acted upon by forces F 1 of 250 lb and F 2 of 333 lb. The section A-A at the central pivot has a curved inner surface with a radius
More informationManual for Computational Exercises
Manual for the computational exercise in TMM4160 Fracture Mechanics Page 1 of 32 TMM4160 Fracture Mechanics Manual for Computational Exercises Version 3.0 Zhiliang Zhang Dept. of Structural Engineering
More informationModule 1.7: Point Loading of a 3D Cantilever Beam
Module 1.7: Point Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 6 Element Type 6 Material Properties 7 Meshing 8 Loads 9 Solution 15 General
More informationME 475 Modal Analysis and Optimization of a Tapered Beam
ME 475 Modal Analysis and Optimization of a Tapered Beam Objectives: To optimize the shape of a tapered beam to minimize the mass, while holding the first three natural frequencies above those of the baseline
More informationImpact of 3D Laser Data Resolution and Accuracy on Pipeline Dents Strain Analysis
More Info at Open Access Database www.ndt.net/?id=15137 Impact of 3D Laser Data Resolution and Accuracy on Pipeline Dents Strain Analysis Jean-Simon Fraser, Pierre-Hugues Allard Creaform, 5825 rue St-Georges,
More informationSIMULATION CAPABILITIES IN CREO. Enhance Your Product Design with Simulation & Analysis
SIMULATION CAPABILITIES IN CREO Enhance Your Product Design with Simulation & Using digital prototypes to understand how your designs perform in real-world conditions is vital to your product development
More information(Based on a paper presented at the 8th International Modal Analysis Conference, Kissimmee, EL 1990.)
Design Optimization of a Vibration Exciter Head Expander Robert S. Ballinger, Anatrol Corporation, Cincinnati, Ohio Edward L. Peterson, MB Dynamics, Inc., Cleveland, Ohio David L Brown, University of Cincinnati,
More informationFinite 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 informationCAE 3D A Computer-Aided Engineering Software Package for Engineering Education
CAE 3D A Computer-Aided Engineering Software Package for Engineering Education S. Otarawanna 1,*, K. Ngiamsoongnirn 1, A. Malatip 1, and P. Eiamaram 2 1 National Metal and Materials Technology Center (MTEC),
More informationCase Study 2: Piezoelectric Circular Plate
Case Study 2: Piezoelectric Circular Plate PROBLEM - 3D Circular Plate, kp Mode, PZT4, D=50mm x h=1mm GOAL Evaluate the operation of a piezoelectric circular plate having electrodes in the top and bottom
More informationTrajectory and window width predictions for a cased hole sidetrack using a whipstock
Louisiana State University LSU Digital Commons LSU Master's Theses Graduate School 004 Trajectory and window width predictions for a cased hole sidetrack using a whipstock Harshad Prakash Patil Louisiana
More informationWhat s new in Femap 9.3
What s new in Femap 9.3 fact sheet www.ugs.com/femap Summary Femap version 9.3 is the latest release of UGS robust pre and post processor for engineering finite element analysis (FEA). Femap software is
More informationFemap Version
Femap Version 11.3 Benefits Easier model viewing and handling Faster connection definition and setup Faster and easier mesh refinement process More accurate meshes with minimal triangle element creation
More informationFinite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench
Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench Course Curriculum (Duration: 120 Hrs.) Section I: ANSYS Mechanical APDL Chapter 1: Before you start using ANSYS a. Introduction to
More informationEnhanced Performance of a Slider Mechanism Through Improved Design Using ADAMS
Enhanced Performance of a Slider Mechanism Through Improved Design Using ADAMS (Nazeer Shareef, Sr. R&D Engr., BAYER CORP., Elkhart, IN) Introduction Understanding of the influence of critical parameters
More informationASME Verification and Validation Symposium May 13-15, 2015 Las Vegas, Nevada. Phillip E. Prueter, P.E.
VVS2015-8015: Comparing Closed-Form Solutions to Computational Methods for Predicting and Validating Stresses at Nozzle-to-Shell Junctions on Pressure Vessels Subjected to Piping Loads ASME Verification
More informationStress 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 informationThe New Generation of Rotary Systems May be Closer Than You Think Frank J. Schuh, Pat Herbert, John Harrell, The Validus International Company, LLC
1 AADE-03-NTCE-02 The New Generation of Rotary Systems May be Closer Than You Think Frank J. Schuh, Pat Herbert, John Harrell, The Validus International Company, LLC Copyright 2003 AADE Technical Conference
More informationWeld Strength Extension
Weld Strength Extension DOCUMENTATION Extension version 170.7 Release date 07-Feb-17 Compatible ANSYS version 17.X, 18.0 www.edrmedeso.com Table of Contents Weld Strength toolbar... 3 Weld Strength Help...
More informationFinite Element Analysis Using Pro/Engineer
Appendix A Finite Element Analysis Using Pro/Engineer A.1 INTRODUCTION Pro/ENGINEER is a three-dimensional product design tool that promotes practices in design while ensuring compliance with industry
More information