This workshop involves a thermal-stress analysis of intersecting pipes using ABAQUS. A quarter symmetry model is created and meshed. A thermal analysis is performed to determine the temperature distribution. This is followed by two static stress analyses - the first applies an internal pressure, and the second uses the temperatures from the thermal analysis as loading. A restart analysis is then used to illustrate ABAQUS' restart capability. Finally, an explicit dynamics analysis is performed to simulate the fully coupled thermal-stress response.
This document provides an overview of continuously variable transmissions (CVTs) and hybrid electric vehicles (HEVs). It discusses the history and development of CVTs, including early inventions. The key components of CVTs are described, including the primary and secondary clutches and different types of belts. The document explains how CVTs work by varying the gear ratio through movement of the sheaves. Research and applications of CVTs are expanding, and they are beginning to be used more widely in vehicles. Hybrid vehicles combine an internal combustion engine with electric motors and batteries, and can have parallel or series configurations. CVTs may be beneficial for improving fuel efficiency in vehicles.
The document summarizes side impact crash test simulations conducted on a 1993 Ford Taurus finite element model according to FMVSS 214, NCAP, and IIHS testing protocols. The simulations showed injury metrics like TTI(d) and pelvis acceleration within acceptable limits for FMVSS 214. Velocity curves for the NCAP test matched well with actual data. B-pillar deformation for the IIHS test was acceptable. Overall, the simulations produced results comparable to real crash tests.
This document discusses the challenges for materials used in electric motors as the demands of electric vehicles increase. It notes trends toward higher power, torque, and voltage as well as increased motor speeds. These trends place new demands on motor materials, including the need for insulation that can withstand higher voltages and temperatures. Electrical steel must reduce losses at higher frequencies while maintaining strength. Permanent magnets must operate at higher temperatures while providing increased flux. The document argues that cooperation between motor and material suppliers will be important to develop new materials that allow improvements in motor design and help accelerate electric vehicle adoption.
Study on Bogie and Suspension System of an Electric Locomotive (Wap-4) IJMER
This document summarizes a study on the bogie and suspension system of the Indian Railways' WAP-4 electric locomotive. Some key points:
- The WAP-4 locomotive was introduced in 1994 to haul heavier passenger trains at higher speeds of up to 140 km/h. It has a more powerful electrical system compared to the earlier WAP-1.
- The bogie uses a conventional Flexicoil design with a cast steel frame and bolster. It has a two-stage suspension system using helical springs between the axle boxes and bogie frame, and between the bogie frame and bolster.
- The bogie supports the locomotive body through a center pivot
This document discusses vehicle aerodynamics and the various road loads that affect a vehicle's performance and fuel efficiency. It covers topics such as aerodynamic drag, lift forces, pressure distributions, rolling resistance, and how factors like air density, drag coefficients, tire design and crosswinds influence a vehicle's handling and energy usage. The goal of vehicle aerodynamics is to optimize these elements to reduce wind resistance, improve stability, and minimize fuel consumption during driving.
This presentation defines hybrid vehicles as those that use two distinct energy sources, such as gasoline and electricity, to power the vehicle. It describes the three main types of hybrids: parallel, series, and a combination of the two. Parallel hybrids have both an internal combustion engine and electric motor connected directly to the transmission, while series hybrids use only the electric motor to power the vehicle. Combination hybrids use both a mechanical and electrical connection between the engine and drive axle. The presentation outlines the advantages and disadvantages of each system and discusses degrees of hybridization from mild to plug-in hybrids.
“MATERIAL AND STRUCTURE OPTIMIZATION AND VALUE ENGINEERING APPLIED TO CAR DOO...Jayesh Sarode
In this project automobile window regulator is selected as a case study for the use of optimization technique in engineering design. This is a project of the work performed towards the stiffness optimization of an automobile window regulator.
The aim of the project is to analyze the car window regulator with presently used material steel and replacing with Plastic if Possible. Also we are going to reduce weight of the window by using Plastic materials replacing with steel. The aim is to achieve the essential function at the lowest overall cost while maintaining optimum value assurance. In this project, the Car window regulator modeled using software CATIA.
This project intends to explore the adoption of Value Engineering (VE) as a value creation tool. This project presents the basics of Value Engineering and its different phases that can be implemented to a window regulator for its optimization. Value Engineering can improve the product cost by reducing the unnecessary costs associated with the product.
My long term goal is to postulate and validate design metrics which effectively and efficiently measure the remanufacturability of given designs. As well as identifying existing re manufacturing guidelines, philosophies, and practices.
This document provides an overview of continuously variable transmissions (CVTs) and hybrid electric vehicles (HEVs). It discusses the history and development of CVTs, including early inventions. The key components of CVTs are described, including the primary and secondary clutches and different types of belts. The document explains how CVTs work by varying the gear ratio through movement of the sheaves. Research and applications of CVTs are expanding, and they are beginning to be used more widely in vehicles. Hybrid vehicles combine an internal combustion engine with electric motors and batteries, and can have parallel or series configurations. CVTs may be beneficial for improving fuel efficiency in vehicles.
The document summarizes side impact crash test simulations conducted on a 1993 Ford Taurus finite element model according to FMVSS 214, NCAP, and IIHS testing protocols. The simulations showed injury metrics like TTI(d) and pelvis acceleration within acceptable limits for FMVSS 214. Velocity curves for the NCAP test matched well with actual data. B-pillar deformation for the IIHS test was acceptable. Overall, the simulations produced results comparable to real crash tests.
This document discusses the challenges for materials used in electric motors as the demands of electric vehicles increase. It notes trends toward higher power, torque, and voltage as well as increased motor speeds. These trends place new demands on motor materials, including the need for insulation that can withstand higher voltages and temperatures. Electrical steel must reduce losses at higher frequencies while maintaining strength. Permanent magnets must operate at higher temperatures while providing increased flux. The document argues that cooperation between motor and material suppliers will be important to develop new materials that allow improvements in motor design and help accelerate electric vehicle adoption.
Study on Bogie and Suspension System of an Electric Locomotive (Wap-4) IJMER
This document summarizes a study on the bogie and suspension system of the Indian Railways' WAP-4 electric locomotive. Some key points:
- The WAP-4 locomotive was introduced in 1994 to haul heavier passenger trains at higher speeds of up to 140 km/h. It has a more powerful electrical system compared to the earlier WAP-1.
- The bogie uses a conventional Flexicoil design with a cast steel frame and bolster. It has a two-stage suspension system using helical springs between the axle boxes and bogie frame, and between the bogie frame and bolster.
- The bogie supports the locomotive body through a center pivot
This document discusses vehicle aerodynamics and the various road loads that affect a vehicle's performance and fuel efficiency. It covers topics such as aerodynamic drag, lift forces, pressure distributions, rolling resistance, and how factors like air density, drag coefficients, tire design and crosswinds influence a vehicle's handling and energy usage. The goal of vehicle aerodynamics is to optimize these elements to reduce wind resistance, improve stability, and minimize fuel consumption during driving.
This presentation defines hybrid vehicles as those that use two distinct energy sources, such as gasoline and electricity, to power the vehicle. It describes the three main types of hybrids: parallel, series, and a combination of the two. Parallel hybrids have both an internal combustion engine and electric motor connected directly to the transmission, while series hybrids use only the electric motor to power the vehicle. Combination hybrids use both a mechanical and electrical connection between the engine and drive axle. The presentation outlines the advantages and disadvantages of each system and discusses degrees of hybridization from mild to plug-in hybrids.
“MATERIAL AND STRUCTURE OPTIMIZATION AND VALUE ENGINEERING APPLIED TO CAR DOO...Jayesh Sarode
In this project automobile window regulator is selected as a case study for the use of optimization technique in engineering design. This is a project of the work performed towards the stiffness optimization of an automobile window regulator.
The aim of the project is to analyze the car window regulator with presently used material steel and replacing with Plastic if Possible. Also we are going to reduce weight of the window by using Plastic materials replacing with steel. The aim is to achieve the essential function at the lowest overall cost while maintaining optimum value assurance. In this project, the Car window regulator modeled using software CATIA.
This project intends to explore the adoption of Value Engineering (VE) as a value creation tool. This project presents the basics of Value Engineering and its different phases that can be implemented to a window regulator for its optimization. Value Engineering can improve the product cost by reducing the unnecessary costs associated with the product.
My long term goal is to postulate and validate design metrics which effectively and efficiently measure the remanufacturability of given designs. As well as identifying existing re manufacturing guidelines, philosophies, and practices.
- A normal modes analysis was performed on a finite element model of a clamping set to determine its vibration mode shapes. The model was imported into HyperMesh and material properties and constraints were applied.
- An eigenvalue extraction was specified to calculate the first 6 modes. The results were viewed in HyperView and showed the component deforming in different patterns for each mode.
This document outlines the contents and concepts of a course on finite element analysis. It covers fundamental concepts like discretization, matrix algebra, and weighted residual methods. It also covers one-dimensional problems involving bars, beams, and trusses. Shape functions, stiffness matrices, and finite element equations are derived for one-dimensional elements. Two-dimensional problems involving plane stress, strain, and heat transfer are also introduced. Numerical integration techniques are discussed. A variety of finite element applications are listed including structural and non-structural problems.
This document provides an introduction to vehicle dynamics and its key concepts. It discusses topics such as ride and handling, suspension systems, forces acting on vehicles, vehicle motion including pitch, roll and yaw, and power characteristics. Vehicle dynamics is the study of how vehicles react to driver inputs based on mechanics. Key aspects covered include body flex, weight transfer during braking, types of steering like understeer and oversteer, suspension design impacts on ride quality, and engine power outputs. The document provides a high-level overview of fundamental vehicle dynamics principles.
07 a70102 finite element methods in civil engineeringimaduddin91
This document contains 8 questions related to the finite element method in civil engineering. The questions cover various topics including:
1) Deriving expressions for potential energy and determining displacements using Rayleigh Ritz method for a 1D rod subjected to loading.
2) Assembling stiffness and force matrices and determining displacements and stresses for a 1D rod under thermal loading using finite element discretization.
3) Evaluating shape functions and determining the Jacobian for an isoparametric triangular element.
The document provides figures and equations to accompany the questions. It examines a range of finite element techniques including shape function derivation, element formulation, structural and thermal analysis, and plate bending elements.
This presentation gives us clear idea on Electric vehicles. Need of EV in building a new methods in transportation world to reduce carbon emissions. Need of batteries into the cars.
Optimization for Frontal Impact under section FMVSS-208 and IIHS criteria in which analysis carried on Fixed barrier with 100%, 40% collision and small offset rigid barrier with 25% collision. Done simulation to see how well a passenger vehicle would protect its occupants in the event of a serious real-world frontal crash.
The document provides details about wheel slide protection (WSP) systems used on Indian Railways. It describes the working principle of WSP, which uses speed sensors and a microprocessor to monitor wheel speeds during braking and control dump valves to adjust brake cylinder pressure if wheels start sliding. The document focuses on the WSP systems supplied by Faiveley and Knorr Bremse, outlining their key components, testing procedures, and troubleshooting guidelines.
ME6603 - FINITE ELEMENT ANALYSIS UNIT - IV NOTES AND QUESTION BANKASHOK KUMAR RAJENDRAN
This document contains a collection of practice problems related to finite element analysis of two-dimensional vector variable problems, including axisymmetric problems. The problems cover derivation of element stiffness matrices and strain-displacement matrices for various element types under different conditions, calculation of element stresses and displacements, modeling of cylinders under pressure, and determination of global stiffness matrices for structures. The elements and conditions include constant strain triangles, linear strain triangles, axisymmetric triangles, plane stress, plane strain, and shells.
This document provides an overview of continuously variable transmissions (CVTs). It discusses the history and development of CVTs, the main types including pulley-based, cone, toroidal, and hydraulic CVTs. The advantages of CVTs are allowing the engine to run at an ideal RPM regardless of vehicle speed and fewer moving parts compared to automatic transmissions. Disadvantages include limited torque capacity and higher cost compared to manual transmissions. CVTs are commonly used in automobiles and are being developed for other applications like trucks, buses, and wind turbines.
Suspension Systems & Components design & AnalysisVinay Tiwari
The document discusses suspension systems and components. It outlines the objectives of suspension systems which include providing good ride and handling performance, ensuring steering control is maintained during maneuvering, and providing isolation from high frequency vibrations. It describes types of independent and dependent suspensions and components such as springs, dampers, wishbones. It covers analyses like mobility, kinematics and forces in suspension members for different load conditions. Different suspension configurations are discussed including MacPherson strut, double wishbone, solid axle leaf spring systems.
Vibration analysis of Drivelines using MBD and the ability of the solvers is showcased in this ppt.
Consideration of 1D, 2D and 3D MBD models for drivelines and performing order analysis for the same.
Result shows the MBD capability of driveline simulations.
A seminar report on hybrid electric vehicle007skpk
This document is a seminar report submitted by Sanjay Kumar Yadav to fulfill the requirements for a Bachelor of Technology degree in Electrical Engineering. The report discusses hybrid electric vehicles, including their technical workings, advantages, disadvantages, and policy considerations. It provides an overview of hybrid electric vehicle technology, comparisons to other vehicle technologies like compressed natural gas vehicles and clean diesel vehicles, and the role of fuel quality. The report aims to guide policymakers in developing and transitional countries on enabling greater vehicle efficiency.
This project report investigates the aerodynamic benefits of replacing traditional car side mirrors with rear-facing cameras through computational fluid dynamics (CFD) simulations. The report was authored by Agate Utane for their BEng in Automotive Engineering with Motorsport. It includes a literature review on CFD methods, fluid mechanics, aerodynamics, and the movement from side mirrors to cameras. The report details the CFD methodology used to simulate a Chevrolet Camaro model with no mirrors, traditional mirrors, and a rear camera design. Results found the rear camera configuration had the lowest drag coefficient, indicating potential fuel savings.
Design analysis of the roll cage for all terrain vehicleeSAT Journals
Abstract We have tried to design an all terrain vehicle that meets international standards and is also cost effective at the same time. We have focused on every point of roll cage to improve the performance of vehicle without failure of roll cage. We began the task of designing by conducting extensive research of ATV roll cage through finite element analysis. A roll cage is a skeleton of an ATV. The roll cage not only forms the structural base but also a 3-D shell surrounding the occupant which protects the occupant in case of impact and roll over incidents. The roll cage also adds to the aesthetics of a vehicle. The design and development comprises of material selection, chassis and frame design, cross section determination, determining strength requirements of roll cage, stress analysis and simulations to test the ATV against failure. Keywords: Roll cage, material, finite element analysis, strength
This document provides a question bank for the Finite Element Analysis course ME6603 taught at R.M.K College of Engineering and Technology. It contains 180 questions divided into two parts - Part A (short questions) and Part B (long questions). The questions cover the main topics of the course including the basic concepts and procedure of finite element analysis, discretization, element types, weighted residual methods, potential energy approach, and boundary conditions. Commercial FEA software packages and steps to use them are also discussed. The document aims to help students prepare for exams by providing a variety of questions related to the finite element method and its applications in engineering problems.
This document discusses mesh quality parameters and the penalty approach in finite element analysis. It defines key parameters that affect mesh quality such as skewness, aspect ratio, warp angle, and Jacobian. Values for tetrahedral meshing are also defined, including tetra collapse, volumetric skew, stretch, and distortion. The document explains that improving element quality manually or through automatic programs can enhance accuracy. It concludes with an overview of the penalty approach theory in finite element analysis.
The document discusses vehicle aerodynamics and the forces involved. It introduces concepts like drag, lift, and side forces caused by air flow over a moving vehicle. Drag opposes the vehicle's motion and is made up of skin friction, induced, and pressure drag. Lift and side forces can cause rolling, pitching, and yawing moments. The key aerodynamic forces of drag, lift, and side forces are defined using equations that relate them to air density, velocity, vehicle area, and coefficient values. Reducing aerodynamic drag improves fuel efficiency and vehicle design.
Resistances to vehicle motion include aerodynamic drag, gradient resistance from inclines, rolling resistance from flexing tires and road surfaces, and inertia forces during acceleration and braking. A gearbox is needed to reduce the high rotational speed of the engine to slower wheel speeds required for starting, stopping, and slower travel while increasing torque. Gears provide increased torque through speed reduction to help overcome resistances when starting from a stop, and shift to faster gears as speed increases to handle higher loads without overstressing components.
- A normal modes analysis was performed on a finite element model of a clamping set to determine its vibration mode shapes. The model was imported into HyperMesh and material properties and constraints were applied.
- An eigenvalue extraction was specified to calculate the first 6 modes. The results were viewed in HyperView and showed the component deforming in different patterns for each mode.
This document outlines the contents and concepts of a course on finite element analysis. It covers fundamental concepts like discretization, matrix algebra, and weighted residual methods. It also covers one-dimensional problems involving bars, beams, and trusses. Shape functions, stiffness matrices, and finite element equations are derived for one-dimensional elements. Two-dimensional problems involving plane stress, strain, and heat transfer are also introduced. Numerical integration techniques are discussed. A variety of finite element applications are listed including structural and non-structural problems.
This document provides an introduction to vehicle dynamics and its key concepts. It discusses topics such as ride and handling, suspension systems, forces acting on vehicles, vehicle motion including pitch, roll and yaw, and power characteristics. Vehicle dynamics is the study of how vehicles react to driver inputs based on mechanics. Key aspects covered include body flex, weight transfer during braking, types of steering like understeer and oversteer, suspension design impacts on ride quality, and engine power outputs. The document provides a high-level overview of fundamental vehicle dynamics principles.
07 a70102 finite element methods in civil engineeringimaduddin91
This document contains 8 questions related to the finite element method in civil engineering. The questions cover various topics including:
1) Deriving expressions for potential energy and determining displacements using Rayleigh Ritz method for a 1D rod subjected to loading.
2) Assembling stiffness and force matrices and determining displacements and stresses for a 1D rod under thermal loading using finite element discretization.
3) Evaluating shape functions and determining the Jacobian for an isoparametric triangular element.
The document provides figures and equations to accompany the questions. It examines a range of finite element techniques including shape function derivation, element formulation, structural and thermal analysis, and plate bending elements.
This presentation gives us clear idea on Electric vehicles. Need of EV in building a new methods in transportation world to reduce carbon emissions. Need of batteries into the cars.
Optimization for Frontal Impact under section FMVSS-208 and IIHS criteria in which analysis carried on Fixed barrier with 100%, 40% collision and small offset rigid barrier with 25% collision. Done simulation to see how well a passenger vehicle would protect its occupants in the event of a serious real-world frontal crash.
The document provides details about wheel slide protection (WSP) systems used on Indian Railways. It describes the working principle of WSP, which uses speed sensors and a microprocessor to monitor wheel speeds during braking and control dump valves to adjust brake cylinder pressure if wheels start sliding. The document focuses on the WSP systems supplied by Faiveley and Knorr Bremse, outlining their key components, testing procedures, and troubleshooting guidelines.
ME6603 - FINITE ELEMENT ANALYSIS UNIT - IV NOTES AND QUESTION BANKASHOK KUMAR RAJENDRAN
This document contains a collection of practice problems related to finite element analysis of two-dimensional vector variable problems, including axisymmetric problems. The problems cover derivation of element stiffness matrices and strain-displacement matrices for various element types under different conditions, calculation of element stresses and displacements, modeling of cylinders under pressure, and determination of global stiffness matrices for structures. The elements and conditions include constant strain triangles, linear strain triangles, axisymmetric triangles, plane stress, plane strain, and shells.
This document provides an overview of continuously variable transmissions (CVTs). It discusses the history and development of CVTs, the main types including pulley-based, cone, toroidal, and hydraulic CVTs. The advantages of CVTs are allowing the engine to run at an ideal RPM regardless of vehicle speed and fewer moving parts compared to automatic transmissions. Disadvantages include limited torque capacity and higher cost compared to manual transmissions. CVTs are commonly used in automobiles and are being developed for other applications like trucks, buses, and wind turbines.
Suspension Systems & Components design & AnalysisVinay Tiwari
The document discusses suspension systems and components. It outlines the objectives of suspension systems which include providing good ride and handling performance, ensuring steering control is maintained during maneuvering, and providing isolation from high frequency vibrations. It describes types of independent and dependent suspensions and components such as springs, dampers, wishbones. It covers analyses like mobility, kinematics and forces in suspension members for different load conditions. Different suspension configurations are discussed including MacPherson strut, double wishbone, solid axle leaf spring systems.
Vibration analysis of Drivelines using MBD and the ability of the solvers is showcased in this ppt.
Consideration of 1D, 2D and 3D MBD models for drivelines and performing order analysis for the same.
Result shows the MBD capability of driveline simulations.
A seminar report on hybrid electric vehicle007skpk
This document is a seminar report submitted by Sanjay Kumar Yadav to fulfill the requirements for a Bachelor of Technology degree in Electrical Engineering. The report discusses hybrid electric vehicles, including their technical workings, advantages, disadvantages, and policy considerations. It provides an overview of hybrid electric vehicle technology, comparisons to other vehicle technologies like compressed natural gas vehicles and clean diesel vehicles, and the role of fuel quality. The report aims to guide policymakers in developing and transitional countries on enabling greater vehicle efficiency.
This project report investigates the aerodynamic benefits of replacing traditional car side mirrors with rear-facing cameras through computational fluid dynamics (CFD) simulations. The report was authored by Agate Utane for their BEng in Automotive Engineering with Motorsport. It includes a literature review on CFD methods, fluid mechanics, aerodynamics, and the movement from side mirrors to cameras. The report details the CFD methodology used to simulate a Chevrolet Camaro model with no mirrors, traditional mirrors, and a rear camera design. Results found the rear camera configuration had the lowest drag coefficient, indicating potential fuel savings.
Design analysis of the roll cage for all terrain vehicleeSAT Journals
Abstract We have tried to design an all terrain vehicle that meets international standards and is also cost effective at the same time. We have focused on every point of roll cage to improve the performance of vehicle without failure of roll cage. We began the task of designing by conducting extensive research of ATV roll cage through finite element analysis. A roll cage is a skeleton of an ATV. The roll cage not only forms the structural base but also a 3-D shell surrounding the occupant which protects the occupant in case of impact and roll over incidents. The roll cage also adds to the aesthetics of a vehicle. The design and development comprises of material selection, chassis and frame design, cross section determination, determining strength requirements of roll cage, stress analysis and simulations to test the ATV against failure. Keywords: Roll cage, material, finite element analysis, strength
This document provides a question bank for the Finite Element Analysis course ME6603 taught at R.M.K College of Engineering and Technology. It contains 180 questions divided into two parts - Part A (short questions) and Part B (long questions). The questions cover the main topics of the course including the basic concepts and procedure of finite element analysis, discretization, element types, weighted residual methods, potential energy approach, and boundary conditions. Commercial FEA software packages and steps to use them are also discussed. The document aims to help students prepare for exams by providing a variety of questions related to the finite element method and its applications in engineering problems.
This document discusses mesh quality parameters and the penalty approach in finite element analysis. It defines key parameters that affect mesh quality such as skewness, aspect ratio, warp angle, and Jacobian. Values for tetrahedral meshing are also defined, including tetra collapse, volumetric skew, stretch, and distortion. The document explains that improving element quality manually or through automatic programs can enhance accuracy. It concludes with an overview of the penalty approach theory in finite element analysis.
The document discusses vehicle aerodynamics and the forces involved. It introduces concepts like drag, lift, and side forces caused by air flow over a moving vehicle. Drag opposes the vehicle's motion and is made up of skin friction, induced, and pressure drag. Lift and side forces can cause rolling, pitching, and yawing moments. The key aerodynamic forces of drag, lift, and side forces are defined using equations that relate them to air density, velocity, vehicle area, and coefficient values. Reducing aerodynamic drag improves fuel efficiency and vehicle design.
Resistances to vehicle motion include aerodynamic drag, gradient resistance from inclines, rolling resistance from flexing tires and road surfaces, and inertia forces during acceleration and braking. A gearbox is needed to reduce the high rotational speed of the engine to slower wheel speeds required for starting, stopping, and slower travel while increasing torque. Gears provide increased torque through speed reduction to help overcome resistances when starting from a stop, and shift to faster gears as speed increases to handle higher loads without overstressing components.
Seaworld celebrates 50 years in 2014 and offers a variety of attractions that allow guests to observe and interact with marine animals. Attractions include Antarctica: Empire of the Penguins where guests can see penguins up close, Wild Arctic to view beluga whales, walruses and polar bears, and Dolphin Nursery to watch dolphin calves with their mothers. Other attractions let guests hand feed sea lions and seals, ride rollercoasters near manta rays, and learn about SeaWorld's legacy of rescuing over 22,000 animals over 40 years.
This document is a certificate of participation certifying that Om Prakash Dave participated in a workshop on Database Management Systems conducted by IIT Bombay from June 13-15, 2012. The certificate includes the name and signature of the professor in charge of the workshop.
This document provides a link to the website www.thesalesexpertusa.com and suggests visiting the site for more information. However, the document itself does not contain any other context or details to effectively summarize in 3 sentences or less.
Candi Borobudur memiliki arsitektur unik dengan bentuk piramida sepuluh tingkat yang melambangkan raja-raja Wangsa Sailendra dan ajaran agama Buddha. Bangunan ini terletak di dataran tinggi buatan dan dibedakan atas dasar, badan, dan bagian atasnya.
The Hussaini Association has found a new 31-acre property located near Circle Drive and Valley Road that could serve as a permanent place for their mosque, community center, and Imambargah. The land includes an existing 1000 square foot building and has electricity, gas, and heating already in place. It is a 10 minute drive from the city and surrounded by acreage houses and farmland. The association has raised $295,000 in donations and mortgage funds so far for the $463,500 property, with $121,000 as a down payment and $147,500 remaining on the mortgage. They will be holding a Q&A session to discuss the new property and management plans.
For the most comfortable Tolo accommodation, go through our rated hotels in Tolo. We offer complete information on each listing to make your booking easier.
- The workshop simulates quasi-static rolling of a thick plate using ABAQUS/Explicit and ABAQUS/Standard. A half-symmetry plane strain model of a plate and roller is used.
- In ABAQUS/Explicit, mass scaling is used to speed up the single-pass simulation. Adaptive meshing maintains mesh quality during the large deformations. Surface contact is defined between the plate and roller.
- In ABAQUS/Standard, a two-step static analysis is used: contact is first established, then the roller draws the plate in the roll pass. Solution controls account for the discontinuous contact/friction behavior.
This document provides instructions for simulating a pipe-on-pipe impact using ABAQUS/Explicit. It describes modeling two steel pipes, applying initial conditions to one pipe to simulate impact, defining contact and constraints between the pipes, meshing the model, submitting the job for analysis, and visualizing the results. The simulation determines stress and deformation in the pipes from the impact event over a time period of 0.015 seconds using an explicit dynamics step with output of fields, histories, and contour plots.
1. Two analysis steps were defined: a static step to apply internal pressure, and a transient step to analyze creep over 50 years.
2. Output requests were specified to write displacements, stresses, and creep strains to the output database every 2 increments, as well as displacements at a point.
3. Boundary conditions of symmetry and a displacement constraint were applied, and internal pressure and end cap pressure loads were prescribed. An initial temperature of 540°C was also specified.
This document describes the steps to create a geometry model of an intersecting pipe and pressure vessel system in ABAQUS. The model represents the system operating at elevated temperature carrying internal pressure. The geometry creation involves:
1. Sketching concentric circles to define the vessel shape and dimensioning them.
2. Creating a datum plane offset from the vessel to sketch the intersecting pipe profile.
3. Extruding the pipe profile through the vessel and cutting out the intersection.
4. Filletting the intersection edge and quartering the model to reduce complexity for future analysis.
When complete, the model will be used in subsequent workshops to build the full analysis model and perform the creep
The document describes defining material and section properties for a pipe creep model in ABAQUS. It includes:
1) Defining a single material with temperature-dependent linear elastic and power-law creep properties based on data in three tables for properties like Young's modulus and creep coefficients.
2) Creating a solid homogeneous section assigning the material and thickness, then assigning the section to the entire part.
3) Instancing the part in the assembly to include it in the model.
1) The document describes creating a linear static analysis model of a cantilever beam in ABAQUS. Key steps include creating the part, material, section, assembly, applying boundary conditions and a pressure load, meshing, creating an analysis job, and viewing the stress contour results.
2) A cantilever beam part is created by sketching a rectangle and extruding it. A linear elastic material, homogeneous solid section, and assembly are defined. Fixed boundary conditions are applied to one end and a pressure load to the top face.
3) The model is meshed with C3D8I elements and a static analysis job is created and submitted. Von Mises stress contours are viewed, showing
This document provides instructions for performing both linear and nonlinear static and dynamic analyses of a skewed plate model in ABAQUS. It describes defining the plate geometry, material properties, and mesh for a linear elastic analysis. It then provides steps for assigning boundary conditions and loads before submitting the linear analysis job. Finally, it gives directions for modifying the model to include geometric nonlinearity and redefining the output requests for the nonlinear analysis.
The document provides instructions for modeling a pump assembly in ABAQUS. Key steps include:
1. Importing the mesh of a pump housing as an orphan mesh and modifying nodal coordinates to change the inner diameter of a hole.
2. Deleting elements to remove ribs from the pump housing and halving the part using element deletion.
3. Importing CAD geometry for other components (cover, gasket, bolts) and halving the imported parts using extruded cuts.
4. Creating the full assembly model by combining the modified pump housing mesh with the halved CAD components. Instructions are provided to ensure the model is set up correctly for subsequent analysis workshops.
The document provides instructions for using the CFD software PHOENICS (v 3.5) to simulate indoor and outdoor airflows. It describes:
1) How to set up an outdoor airflow simulation case to model wind flowing around a rectangular building within a defined domain. This includes setting boundary conditions and object properties.
2) How to run the simulation in PHOENICS and view the velocity profile results.
3) How to set up an indoor airflow simulation case without heat transfer to model air movement inside a room, including defining the geometry and boundary conditions.
The document provides step-by-step guidance for completing these example cases in PHOENICS to demonstrate its capabilities for architectural
Last Rev. August 2014 Calibration and Temperature Measurement.docxsmile790243
This document provides instructions for an experiment to determine the time constants and calibrate three temperature sensors: a thermometer, thermocouple, and thermistor. Students will create a calibration curve by measuring the sensors in ice water and boiling water. They will then determine the time constants of each sensor when exposed to step changes in temperature from ambient air to ice water and hot air to ambient air. Finally, students will analyze the frequency response of each sensor and compare their capabilities to respond to changing temperature inputs.
This document provides instructions for completing a nonlinear static analysis of a pump assembly model using ABAQUS. It describes defining analysis steps, contact interactions between components, applying bolt preloads and pressure loads, and evaluating results. Key steps include:
1) Creating two analysis steps - one for bolt pretensioning and one for pressurization.
2) Defining surfaces on components and specifying contact interactions between surfaces using a friction coefficient.
3) Applying bolt preloads of 500 lbs by defining pretension sections and fixing bolt lengths after pretensioning.
4) Applying 1000 psi pressure loads to pump and cover surfaces.
5) Evaluating results such as gasket sealing pressure, bolt forces,
This document discusses structured meshing of a pipe creep model in ABAQUS. It describes partitioning the model into regions that can be meshed using structured techniques. This includes partitioning the pressure vessel, pipe faces on symmetry planes, and the inner vessel surface. The pipe is then partitioned using 4-sided patches. Once partitioned, a global seed is assigned and 20-node hexahedral elements with reduced integration are used to generate a structured mesh of the entire model.
1. The document describes steps to create agro-climatic zones of Tanzania using GIS by analyzing temperature, rainfall, and evapotranspiration data.
2. Key steps include converting vector data to raster, calculating moisture availability, classifying temperature and moisture zones, and combining the zones to produce the final agro-climatic map.
3. Models are created in GIS software to automate the process and allow easy reproduction of the analysis.
The document is an instructor's guide for Pro/ENGINEER Wildfire for Designers. It contains 16 chapters that provide instruction on various aspects of using Pro/ENGINEER. Each chapter includes review questions, exercise instructions, and solutions to the exercises. The guide is intended to help teach students how to use Pro/ENGINEER for mechanical design tasks.
This document is an instructor's guide for Pro/ENGINEER Wildfire for Designers. It contains chapters that provide instruction on various aspects of using Pro/ENGINEER for design. The table of contents lists 16 chapters, each covering a different topic. Examples and exercises are provided at the end of chapters 2-4 to help students practice and reinforce the concepts covered.
The document provides a cooling load calculation report for a warehouse building with two floors. It includes input data on the building specifications, outdoor and indoor design conditions, external and internal loads, and ventilation requirements. Calculations were performed using HAP software to determine the cooling loads on a space-by-space and system-by-system basis. The report summarizes the input data, output cooling loads, and compares the results to design values.
This document provides step-by-step instructions for creating a beam model in AxisVM to analyze two reinforced concrete beams. It describes how to:
1. Create the geometry of two beams - one 12m long and one 10m long.
2. Define the material, cross section, supports, and degrees of freedom.
3. Apply self-weight and variable linear loads to the beams in different load cases.
4. Provide details on modeling options like perspectives, labels, and load combinations.
This document provides step-by-step instructions for modeling methane combustion using ANSYS CFX. It begins by importing a mesh file and defining boundary conditions including inlet velocities and species concentrations. Reaction kinetics are then specified by defining the combustion reaction and associated rate parameters. Finally, a high temperature boundary condition is applied to the mesh surface to ignite the combustion process. The tutorial aims to provide guidelines for initial combustion simulations while noting that input values may need refinement for accuracy.
This document describes how to create, run, and monitor a creep analysis job in ABAQUS to model the creep of a pipe intersection over 50 years. It discusses defining and submitting the job, visualizing and plotting the deformed shape and results, including displacement and stress/strain histories at the intersection point over time.
Transient thermal analysis of a clutch plate in AnsysRahul Shedage
This document describes how to perform a transient thermal analysis of a clutch plate using finite element analysis software. The analysis involves:
1) Setting up the project, defining engineering data like thermal conductivity, and importing the clutch plate geometry file.
2) Generating a mesh on the clutch plate model.
3) Applying loads like convection and a temperature profile on surfaces, and boundary conditions.
4) Solving the model to determine the temperature distribution and total heat flux over time.
5) Viewing the results of the transient thermal analysis like temperature, total heat flux.
HCL Notes and Domino License Cost Reduction in the World of DLAUpanagenda
Webinar Recording: https://www.panagenda.com/webinars/hcl-notes-and-domino-license-cost-reduction-in-the-world-of-dlau/
The introduction of DLAU and the CCB & CCX licensing model caused quite a stir in the HCL community. As a Notes and Domino customer, you may have faced challenges with unexpected user counts and license costs. You probably have questions on how this new licensing approach works and how to benefit from it. Most importantly, you likely have budget constraints and want to save money where possible. Don’t worry, we can help with all of this!
We’ll show you how to fix common misconfigurations that cause higher-than-expected user counts, and how to identify accounts which you can deactivate to save money. There are also frequent patterns that can cause unnecessary cost, like using a person document instead of a mail-in for shared mailboxes. We’ll provide examples and solutions for those as well. And naturally we’ll explain the new licensing model.
Join HCL Ambassador Marc Thomas in this webinar with a special guest appearance from Franz Walder. It will give you the tools and know-how to stay on top of what is going on with Domino licensing. You will be able lower your cost through an optimized configuration and keep it low going forward.
These topics will be covered
- Reducing license cost by finding and fixing misconfigurations and superfluous accounts
- How do CCB and CCX licenses really work?
- Understanding the DLAU tool and how to best utilize it
- Tips for common problem areas, like team mailboxes, functional/test users, etc
- Practical examples and best practices to implement right away
Taking AI to the Next Level in Manufacturing.pdfssuserfac0301
Read Taking AI to the Next Level in Manufacturing to gain insights on AI adoption in the manufacturing industry, such as:
1. How quickly AI is being implemented in manufacturing.
2. Which barriers stand in the way of AI adoption.
3. How data quality and governance form the backbone of AI.
4. Organizational processes and structures that may inhibit effective AI adoption.
6. Ideas and approaches to help build your organization's AI strategy.
Fueling AI with Great Data with Airbyte WebinarZilliz
This talk will focus on how to collect data from a variety of sources, leveraging this data for RAG and other GenAI use cases, and finally charting your course to productionalization.
Building Production Ready Search Pipelines with Spark and MilvusZilliz
Spark is the widely used ETL tool for processing, indexing and ingesting data to serving stack for search. Milvus is the production-ready open-source vector database. In this talk we will show how to use Spark to process unstructured data to extract vector representations, and push the vectors to Milvus vector database for search serving.
zkStudyClub - LatticeFold: A Lattice-based Folding Scheme and its Application...Alex Pruden
Folding is a recent technique for building efficient recursive SNARKs. Several elegant folding protocols have been proposed, such as Nova, Supernova, Hypernova, Protostar, and others. However, all of them rely on an additively homomorphic commitment scheme based on discrete log, and are therefore not post-quantum secure. In this work we present LatticeFold, the first lattice-based folding protocol based on the Module SIS problem. This folding protocol naturally leads to an efficient recursive lattice-based SNARK and an efficient PCD scheme. LatticeFold supports folding low-degree relations, such as R1CS, as well as high-degree relations, such as CCS. The key challenge is to construct a secure folding protocol that works with the Ajtai commitment scheme. The difficulty, is ensuring that extracted witnesses are low norm through many rounds of folding. We present a novel technique using the sumcheck protocol to ensure that extracted witnesses are always low norm no matter how many rounds of folding are used. Our evaluation of the final proof system suggests that it is as performant as Hypernova, while providing post-quantum security.
Paper Link: https://eprint.iacr.org/2024/257
Digital Banking in the Cloud: How Citizens Bank Unlocked Their MainframePrecisely
Inconsistent user experience and siloed data, high costs, and changing customer expectations – Citizens Bank was experiencing these challenges while it was attempting to deliver a superior digital banking experience for its clients. Its core banking applications run on the mainframe and Citizens was using legacy utilities to get the critical mainframe data to feed customer-facing channels, like call centers, web, and mobile. Ultimately, this led to higher operating costs (MIPS), delayed response times, and longer time to market.
Ever-changing customer expectations demand more modern digital experiences, and the bank needed to find a solution that could provide real-time data to its customer channels with low latency and operating costs. Join this session to learn how Citizens is leveraging Precisely to replicate mainframe data to its customer channels and deliver on their “modern digital bank” experiences.
Skybuffer SAM4U tool for SAP license adoptionTatiana Kojar
Manage and optimize your license adoption and consumption with SAM4U, an SAP free customer software asset management tool.
SAM4U, an SAP complimentary software asset management tool for customers, delivers a detailed and well-structured overview of license inventory and usage with a user-friendly interface. We offer a hosted, cost-effective, and performance-optimized SAM4U setup in the Skybuffer Cloud environment. You retain ownership of the system and data, while we manage the ABAP 7.58 infrastructure, ensuring fixed Total Cost of Ownership (TCO) and exceptional services through the SAP Fiori interface.
Freshworks Rethinks NoSQL for Rapid Scaling & Cost-EfficiencyScyllaDB
Freshworks creates AI-boosted business software that helps employees work more efficiently and effectively. Managing data across multiple RDBMS and NoSQL databases was already a challenge at their current scale. To prepare for 10X growth, they knew it was time to rethink their database strategy. Learn how they architected a solution that would simplify scaling while keeping costs under control.
5th LF Energy Power Grid Model Meet-up SlidesDanBrown980551
5th Power Grid Model Meet-up
It is with great pleasure that we extend to you an invitation to the 5th Power Grid Model Meet-up, scheduled for 6th June 2024. This event will adopt a hybrid format, allowing participants to join us either through an online Mircosoft Teams session or in person at TU/e located at Den Dolech 2, Eindhoven, Netherlands. The meet-up will be hosted by Eindhoven University of Technology (TU/e), a research university specializing in engineering science & technology.
Power Grid Model
The global energy transition is placing new and unprecedented demands on Distribution System Operators (DSOs). Alongside upgrades to grid capacity, processes such as digitization, capacity optimization, and congestion management are becoming vital for delivering reliable services.
Power Grid Model is an open source project from Linux Foundation Energy and provides a calculation engine that is increasingly essential for DSOs. It offers a standards-based foundation enabling real-time power systems analysis, simulations of electrical power grids, and sophisticated what-if analysis. In addition, it enables in-depth studies and analysis of the electrical power grid’s behavior and performance. This comprehensive model incorporates essential factors such as power generation capacity, electrical losses, voltage levels, power flows, and system stability.
Power Grid Model is currently being applied in a wide variety of use cases, including grid planning, expansion, reliability, and congestion studies. It can also help in analyzing the impact of renewable energy integration, assessing the effects of disturbances or faults, and developing strategies for grid control and optimization.
What to expect
For the upcoming meetup we are organizing, we have an exciting lineup of activities planned:
-Insightful presentations covering two practical applications of the Power Grid Model.
-An update on the latest advancements in Power Grid -Model technology during the first and second quarters of 2024.
-An interactive brainstorming session to discuss and propose new feature requests.
-An opportunity to connect with fellow Power Grid Model enthusiasts and users.
Programming Foundation Models with DSPy - Meetup SlidesZilliz
Prompting language models is hard, while programming language models is easy. In this talk, I will discuss the state-of-the-art framework DSPy for programming foundation models with its powerful optimizers and runtime constraint system.
A Comprehensive Guide to DeFi Development Services in 2024Intelisync
DeFi represents a paradigm shift in the financial industry. Instead of relying on traditional, centralized institutions like banks, DeFi leverages blockchain technology to create a decentralized network of financial services. This means that financial transactions can occur directly between parties, without intermediaries, using smart contracts on platforms like Ethereum.
In 2024, we are witnessing an explosion of new DeFi projects and protocols, each pushing the boundaries of what’s possible in finance.
In summary, DeFi in 2024 is not just a trend; it’s a revolution that democratizes finance, enhances security and transparency, and fosters continuous innovation. As we proceed through this presentation, we'll explore the various components and services of DeFi in detail, shedding light on how they are transforming the financial landscape.
At Intelisync, we specialize in providing comprehensive DeFi development services tailored to meet the unique needs of our clients. From smart contract development to dApp creation and security audits, we ensure that your DeFi project is built with innovation, security, and scalability in mind. Trust Intelisync to guide you through the intricate landscape of decentralized finance and unlock the full potential of blockchain technology.
Ready to take your DeFi project to the next level? Partner with Intelisync for expert DeFi development services today!
leewayhertz.com-AI in predictive maintenance Use cases technologies benefits ...alexjohnson7307
Predictive maintenance is a proactive approach that anticipates equipment failures before they happen. At the forefront of this innovative strategy is Artificial Intelligence (AI), which brings unprecedented precision and efficiency. AI in predictive maintenance is transforming industries by reducing downtime, minimizing costs, and enhancing productivity.
Overcoming the PLG Trap: Lessons from Canva's Head of Sales & Head of EMEA Da...
Workshop16 heat-pipejoint
1. Workshop 16
Thermal-Stress Analysis of Intersecting Pipes
Introduction
This workshop involves the thermal-stress analysis of a cylindrical pipe intersection. The
pipes are surrounded by a fluid and are filled with another fluid. The interaction between
the pipes and the surrounding fluids are modeled using surface convection. The internal
pressure due to the inner fluid is modeled with a pressure load. Both the thermal and
mechanical responses are sought. The mechanical behavior of the part is expected to
influence the thermal response weakly. Thus a sequential thermal stress analysis is
performed. The thermal analysis model will be developed first and will form the basis of
the structural analysis model. The structural analysis consists of two steps and will
illustrate the use of the restart capability in ABAQUS. The thermal-stress analysis will
also be performed with ABAQUS/Explicit. Only a quarter of the intersection will be
modeled because of symmetry.
Importing and defeaturing the part
1. Start a new session of ABAQUS/CAE from the workshops/heatTransfer
directory.
2. From the main menu bar, select FileImportPart.
3. In the Import Part dialog box, select the file named pipe_int.sat and click
Continue.
4. In the Create Part from ACIS File dialog box, review the basic information
about the geometry and click OK to proceed.
5. The geometry of the model is shown in Figure W16–1.
Figure W16–1. Initial part geometry
2. 6. A quarter-symmetry model will be used in the analysis. From the main menu bar,
select ShapeCut Extrude to create two extruded cuts. For the first cut,
select the face highlighted in Figure W16–2 as the plane for the extruded cut.
Select the vertical edge highlighted in the figure as the edge that will appear
vertical and to the right of the sketch.
Figure W16–2. First extruded cut
7. Sketch the section for the extruded cut as shown in Figure W16–3. In the
viewport, click mouse button 2 to complete the operation and in the prompt area
click Done to proceed. (Mouse button 2 is the middle mouse button on a 3-button
mouse; on a 2-button mouse, press both mouse buttons simultaneously.) In the
Edit Cut Extrusion dialog box, select the direction of cut as shown in Figure
W16–2 and select the end condition Through All.
W16.2
Select this
face
Direction of cut
Edge that will appear vertical
and to the right of the sketch
3. Figure W16–3. Shape of the first cut
8. Repeat steps 6 and 7 for the second cut, as shown in Figures W16–4 and W16–5.
Figure W16–4. Second extruded cut
W16.3
Select this
face
Direction of cut
Edge that will appear vertical
and to the right of the sketch
4. Figure W16–5. Shape of the second extruded cut
9. From the main menu bar, select ToolsRepair. In the Geometry Repair
Tools dialog box, select the Remove faces tool to remove the fillets shown in
Figure W16–6 (you may use the selection filters to facilitate the face selection).
Select the faces highlighted in the figure. Remember to toggle on Local stitch in
the prompt area before completing the operation.
Figure W16–6. Fillets to be removed
10. The fillets will be removed and the adjacent faces are automatically extended by
ABAQUS/CAE to fill the gaps as shown in Figure W16–7. Rename the model
thermal, and save the ABAQUS/CAE model database as pipe-intersection.
W16.4
Remove these faces
5. Figure W16–7. Final part geometry
Properties and model assembly
The units used in this model are SI (kg, m, s, N, °C). The pipes are made of a typical
commercial purity aluminum alloy. The material is assumed to harden isotropically. The
dependence of the flow stress on the temperature is included.
1. Switch to the Property module.
11. From the main menu bar, select MaterialCreate. Name the material
aluminum, and specify the following thermal properties:
· Temperature dependent conductivity:
204 W/m°C at 0°C
225 W/m°C at 300°C
· Specific heat = 880 J/kg°C
· Inelastic heat fraction = 0.0 (for the ABAQUS/Explicit analysis)
· Density = 2700 kg/m3
12. Add the following mechanical properties. (These properties will be used in the
subsequent stress analysis.)
· Modulus of elasticity = 6.9E10 Pa
· Poisson's ratio = 0.33
· Coefficient of thermal expansion = 8.42E-5
· Temperature-dependent plasticity:
Read the data from an ASCII text file. Toggle on Use temperature-
dependent data, as shown in Figure W16–8, and right-click in the data field
indicated in the figure. From the list of available options, select Read from
File. Read the data from the file plasticProps.inp
W16.5
6. Figure W16–8. Reading plastic material properties from a file
13. Create a homogeneous solid section named aluminumSection, and assign it
to the part.
14. Switch to the Assembly module, and create an instance of the part pipe-int.
Analysis procedure and output
To simulate the thermal response of the part, a single heat transfer step will be used.
1. Switch to the Step module.
15. From the main menu bar, select StepCreate. In the Create Step dialog box,
select Heat transfer as the general procedure type and create a transient heat
transfer analysis step using the following parameters:
· Description: Thermal analysis
· Total time period = 200
· Maximum number of increments allowed = 100
· Initial increment size = 1
· End the step when the temperature change rate is less than 0.5
· Maximum allowable temperature change per increment = 10
16. Accept all default ODB output requests. Specify a restart frequency of 5.
Surface film condition
The conditions to model the surface convection will now be applied.
1. Switch to the Interaction module.
17. From the main menu bar, select InteractionCreate. In the Create
Interaction dialog box, select Film condition as the interaction type and click
Continue. Specify a film condition for the outer surface of the pipe shown in
Figure W16–10. Use a film coefficient of 50 W/m2
·s°C and sink temperature of
20°C.
W16.6
Toggle this on
Right click
here
7. Figure W16–10. Surface for outer film condition
18. The fluid temperature on the inner surface is time-dependent. Thus, an amplitude
curve is required to prescribe the temperature history. From the main menu bar,
select ToolsAmplitudeCreate. Accept the default Tabular type, and click
Continue. Enter the film sink temperature amplitude data points (0, 20),
(10, 400), and (200, 400) in the table. Click OK.
19. Create a film condition for the interior surface of the pipe shown in
Figure W16–11. Specify a film coefficient of 1200 W/m2
·s·°C. Enter a value of
1°C for the sink temperature, and use amplitude curve Amp-1 created earlier for
the sink amplitude. The magnitude of the sink temperature will be the product of
the specified value and the amplitude.
W16.7
8. Figure W16–11. Surface for inner film condition
Initial conditions
The pipe is initially at room temperature (20°C).
1. Switch to the Load module.
20. The pipes are initially at a temperature of 20°C. From the main menu bar, select
FieldCreate.
21. In the Create Field dialog box, set the step to Initial, the category to Other, the
type to Temperature, and click Continue.
22. Select the complete model by dragging the mouse across the viewport with the left
mouse button held down. Click Done.
23. In the Edit Field dialog box, enter a value of 20°C for the initial temperature
Magnitude.
Partitioning and meshing the part
You will now generate the finite element mesh. Rather than creating more complicated
partitions for the sake of generating an all-hex mesh, create a series of simple partitions to
subdivide the part instance into hex- and tet-meshable regions. ABAQUS/CAE will
automatically impose the necessary tie constraints between regions of the mesh that are
incompatible.
1. Switch to the Mesh module.
24. From the main menu bar, select ToolsPartition. In the Create Partition
dialog box, select Cell as the partition type and Extend face as the method.
Partition the end region shown in Figure W16–12. Use the face highlighted in the
figure as the face to be extended.
W16.8
9. Figure W16–12. First partition
25. Similarly create a partition for the other end, as shown in Figure W16–13.
Figure W16–13. Second partition
26. Create another partition near the pipe junction using the Define Cutting plane
technique and the Point & Normal method for specifying the partitioning plane.
Select the point highlighted in Figure W16–14 as the point through which the
plane will pass and the highlighted edge as the normal direction.
Extend this face
Extend this face
W16.9
10. Figure W16–14. Third partition
27. Similarly create another partition using the same technique as shown in
Figure W16–15.
Figure W16–15. Fourth (and final) partition
28. From the main menu bar, select MeshControls and assign the Tet element
shape to the region highlighted in Figure W16–16.
Define cutting
plane through
this point
Edge normal to the
cutting plane
Define cutting plane
through this point
Edge normal to the
cutting plane
W16.10
11. Figure W16–16. Region assigned tet elements
29. From the main menu bar, select MeshElement Type and then select the
whole model as the region to be assigned an element type. In the Element Type
dialog box, choose Standard as the element library and Heat Transfer as the
element family. Accept the default element type (DC3D8 elements for hex-
meshable regions and DC3D4 for tet-meshable regions).
30. From the main menu bar, select SeedInstance and assign a global seed size
of 0.05 to the part instance.
31. From the main menu bar, select MeshInstance to generate the part instance
mesh. The message shown in Figure W16–17 appears to indicate that tie
constraints will be automatically generated at the interface between the tet and hex
element regions. Click Continue.
Figure W16–17. Warning message regarding tie constraints
W16.11
12. The meshed part is shown in Figure W16–18.
Figure W16–18. Finite element mesh
Thermal analysis
1. Switch to the Job module.
32. From the main menu bar, select JobCreate, create a job named pipe-
thermal, and click Continue. Accept the default job parameters, and click OK.
33. The nodal temperatures must be written to the results file for them to be read by
the subsequent stress analysis. Currently there is no direct way of requesting this
output using the ABAQUS/CAE menus. The output must be requested using the
Keywords Editor. From the main menu bar, select ModelEdit
Keywordsthermal to open the Keywords Editor. Select the last text block
available (before the *End step option), and click Add After. Enter the
following two lines in the new text block:
*node file
nt,
34. Click OK to close the Keywords Editor.
35. Save the model database.
W16.12
13. 36. Open the Job Manager, and submit the job for analysis.
Postprocessing
1. Once the analysis completes, click Results in the Job Manager.
37. Plot the contours of nodal temperature by selecting the variable NT11 from the
Field Output dialog box. The contour plot is shown in Figure W16–19.
Figure W16–19. Temperature distribution in the pipes
Stress analysis
The stress analysis consists of two steps. In the first step, a pressure load is applied. In the
second step, the thermal load is applied. The complete structural analysis will be
performed using two jobs to illustrate the use of the restart analysis capability.
The thermal analysis model and properties will form the basis of the stress analysis
model. From the main menu bar, select ModelCopy Model and copy the model
named thermal to a new model named stress. From the Model pull down list,
select stress. Make the following changes to this model.
1. Enter the Step module. Delete the Heat Transfer step, and create a Static,
General step with a time period of 10 and an initial time increment size of 1.
38. Create a set named n-hist consisting of the two vertices on the outer and inner
surface of the pipe as shown in Figure W16–20. Request displacement history
output for this set.
W16.13
14. Figure W16–20. Vertices belonging to set n-hist
39. Enter the Load module. Apply a pressure with magnitude 3.50E6 Pa to the
internal surfaces of the pipe.
40. In the Initial step, define symmetry boundary conditions to each symmetry plane
and a pinned condition to the top face as shown in Figure W16–21,
Figure W16–22, and Figure W16–23.
Tip: Set the selection filter type to Face to facilitate the selections.
Figure W16–21. XSYMM faces
Select these two
vertices
W16.14
Select these
faces
15. Figure W16–22. ZSYMM faces
W16.15
Select
these
faces
Boundary condition on this face
represents attachment to a larger
structure.
16. Figure W16–23. PINNED face
41. Enter the Mesh module. Change the element type assigned to the part instance
regions to C3D4 and C3D8I by choosing the 3D Stress element family.
42. From the main menu bar, select ModelEdit Keywordsstress and click
Discard All Edits to delete the two keyword lines added for the temperature file
output in the thermal analysis.
43. Enter the Job module. Create a job named pipe-stress, and run the analysis job.
44. Save the model database.
45. Once the job completes, enter the Visualization module and plot the contours of
stress and displacement. The displacement magnitude contour plot is shown in
Figure W16–24. In this figure the displacement magnification has been set to
1.0.
W16.16
Select this
face
17. Figure W16–24. Contour of displacement magnitude
Restart analysis
The remainder of the stress analysis will now be performed using the restart analysis
capability. Copy the model stress to stress-restart. For the stress-restart, do the
following:
1. Enter the Step module. Create an additional static step for the restart analysis. Set
the step time period to 200 and the initial time increment to 0.2.
46. Modify the history output request for the node set n-hist. In the second analysis
step, add an output request for nodal temperatures.
47. Enter the Load module. Open the Field Manager. For the second analysis step,
edit Field-1 (the initial temperature) so that its status is set to Reset to initial.
This effectively deactivates the field in this step.
48. Create a new field to apply the temperatures obtained in the thermal analysis. In
the Edit Field dialog box, specify the values shown in Figure W16–25.
W16.17
18. Figure W16–25. Reading temperatures from the .fil file
49. From the main menu bar, select ModelEdit Attributesstress-restart to
edit the model attributes for the restart analysis model. Use the parameters shown
in Figure W16–26. Please note that text input to ABAQUS/CAE is case sensitive.
Figure W16–26. Restart analysis model attributes
50. Enter the Job module. Create a job named pipe-stress-restart. Set the
job type to Restart in the Edit Job dialog box.
51. Save the model database, and submit the analysis job.
W16.18
19. 52. When the job completes, plot the Mises stress contours. The plot is shown in
Figure W16–27.
Figure W16–27. Mises stress distribution at the end of the analysis
Coupled thermal-stress analysis with ABAQUS/Explicit
You will now perform the full thermal stress analysis using the explicit dynamics solver.
Even though a fully coupled procedure is used, the thermal response has been uncoupled
from the mechanical response since the inelastic heat fraction has been set to zero. Thus,
in effect a sequential analysis is performed. The steps required to complete this analysis
are described next.
1. Copy the model named stress to a new model named stress-explicit.
53. Enter the Step module. Delete the Static, General step, and create two
Dynamic, Temp-disp, Explicit steps. For the first step use a time period of
10 seconds, while for the second step use a time period of 200 seconds.
54. For each step, apply Semi-automatic mass scaling using a scale factor of
1.0e8.
55. Enter the Interaction module. Create the following surface film conditions in
Step-2:
· For the outer surfaces of the pipes, use a film coefficient of
50 W/m2
·s°C and sink temperature of 20°C.
· For the inner surfaces of the pipes, use a film coefficient of 1200
W/m2
·s·°C. Enter a value of 1 °C for the sink temperature and use
amplitude curve Amp-1 for the sink amplitude.
56. Enter the Load module. Recall that in dynamic analysis procedures, loads are
applied instantaneously. However, in this problem, a quasi-static response is
W16.19
20. sought. In order to promote a quasi-static response, loads must be applied
gradually. For this purpose create a smooth-step amplitude curve. Name the curve
Amp-2; use the points (0,0), (10,1) to define the curve.
57. Apply a pressure load of 3.50E6 Pa in Step-1.Use the amplitude Amp-2 for
the load application.
58. Enter the Mesh module. Change the element library to Explicit, the element
family to Thermally Coupled, and the element type to C3D8RT and C3D4T.
59. Enter the Job module. Create a job named pipe-stress-explicit and submit it
for analysis.
Postprocessing (continued)
1. Plot the contours for Mises stress and PEEQ on the deformed shape for both the
implicit and explicit analyses. The PEEQ contours for both analyses are shown in
Figure W16–28. The results predicted by ABAQUS/Standard and
ABAQUS/Explicit are nearly identical.
Figure W16–28. PEEQ contours at the end of the analysis
(explicit, left; implicit, right)
60. From the main menu bar, select ToolsPathCreate. Choose the Node list
type, and Continue. Click Select, and select the nodes along the edge shown in
Figure W16–29.
W16.20
21. Figure W16–29. Node path
61. From the main menu bar, select ToolXY DataCreate. Select Path from the
Create XY Data dialog box, and click Continue. Examine the various options
in the XY Data from Path dialog box. Click Plot to display the variation of
PEEQ along the path as shown in Figure W16–30.
Figure W16–30. Path plot of PEEQ (explicit analysis)
W16.21
The path starts
here
Select the nodes
on this edge to
define the path