BloodSim: Coupled Solid-Fluid Simulation of Cardiovascular Systems

Save this PDF as:
 WORD  PNG  TXT  JPG

Size: px
Start display at page:

Download "BloodSim: Coupled Solid-Fluid Simulation of Cardiovascular Systems"

Transcription

1 BloodSim: Coupled Solid-Fluid Simulation of Cardiovascular Systems D.R.Hose 1, P.V.Lawford, A.J.Narracott, J.M.T.Penrose 2, C.J.Staples, I.P.Jones 1 University of Sheffield, England, 2 AEA Technology, England Abstract P. Nuesser 3, L.Choub 3,D.Quinn 4 3 Berlin Heart AG, Germany, 4 AVE/Medtronic, Ireland Cardiovascular systems typically feature strong interaction between solid and fluid phases. Software has been developed to couple ANSYS to CFX, via an external interface, to produce the capacity for simulation of systems of this type. The interface software passes pressure data from the fluid phase to the solid phase, which returns boundary position and velocity information. This process iterates until consistent results are obtained across the wetted boundary. There is facility for relaxation of pressure, displacement or both to assist convergence of the process. Automatic remeshing of the fluid domain is performed when the distorting mesh violates quality constraints. This feature is necessary for systems like heart valves that feature severe topological distortion. Results are presented for a series of applications including comparison with Womersley's analytical solutions for pulse transmission in an elastic-walled artery, analysis of the fluid and structural characteristics of a stented artery and simulations of the operation of an extracorporeal heart assist device. Introduction There are several approaches to the solution of coupled solid-fluid systems. It is likely that the most stable approach is the development of a fully coupled solver, with degrees of freedom for both solid and fluid phases present in the same analysis system. The primary drawback of this approach in the context of the cardiovascular system is that it is unlikely to be the most versatile in terms of its functionality. The advanced features required to describe many of the phenomena associated with cardiovascular systems are unlikely to be resident within a single suite of programmes. On the structures side the tissues are primarily nonlinear and anisotropic, and appropriate functions for the representation of their stress/strain characteristics are featured only in advanced structural solvers. On the fluids side, the rheology of blood is complex: it is certainly non-newtonian at some shear rates, and indeed two-phase plasma/erythrocyte representations might be most appropriate. There is also the likelihood of turbulence in some cardiovascular systems, including distal to aortic heart valve prostheses and at some arterial stenoses. For real application to benefit our understanding of haemodynamic processes including haemostasis and thrombosis, multiple species and chemical reaction representation are important. In terms of postprocessing, transient particle tracking is an important feature for the assessment of haemolysis and its contribution to thrombotic processes. There have been a number of attempts to write a generic interface for the external coupling of structural and fluids solvers, including one that featured an analysis of a mechanical heart valve as a target application 1. Many investigators have coupled specific codes for a particular application, including for arterial segments 2 and bifurcations 3. In these analyses the procedure has been to couple the solid and fluid domains at a wetted boundary, typically passing surface components of a stress tensor from the fluid domain to the solid and displacement or velocity back from solid to fluid. This process is repeated until the pressure and displacements are converged. The most common approach to the solution is some variant of a Jacobi iteration scheme, and indeed this is the basis of the approach adopted in the current programme. It is often the case, particularly for incompressible fluids, that a relatively small movement of the solid wall causes a large change in the local pressure and so inevitably some form of relaxation is applied to stabilize the system to try to achieve convergence. It has been demonstrated 4 that the relative stability of a Newton scheme might be more appropriate for some problems.

2 The selection of codes for coupling is based on the requirements from the analysis. Clearly the solids code must include the appropriate tissue materials modeling, together with any necessary contact facilities. The fluids code must feature the facility for moving the mesh as the boundary deforms, and must handle the mesh deformation terms appropriately. The implementation of the mesh movement terms within CFX is based on the methodology described by Hawkins 5. In the study of systems such as heart valve prostheses it is likely that topological changes of the mesh will be required, and so a facility for automatic remeshing and appropriate results interpolation is required. It is unlikely that the most efficient mesh for the problem will be of similar density in the solid and fluid domains (almost always the fluid mesh will be denser) and so a surface load and displacement interpolation facility should be provided by the coupling software. ANSYS and CFX were chosen for the solids and fluids phases respectively. Significant developments were required in the CFX software to produce the required functionality. Procedure A standalone coupling program has been produced to provide a software interface between ANSYS to CFX to enable the passing of results across a common wetted boundary between solid and fluid domains. Details of the coupling strategy and of the interpolation routines are presented by Penrose and Staples 6. The fundamental procedure is to compute the components of the stress tensor at the wetted boundary in the fluid phase, and to pass these to the solid phase a surface loads. In the current implementation only the static pressure component of the surface load is passed. The motion of the solid phase under the imposed fluid pressures is computed, and the displacements of the wetted boundary passed back to the fluid phase. The fluid solve is performed with the consequent boundary motion to produce a new pressure distribution. This procedure is repeated until the process converges, measured by the convergence of a pressure norm, before progression to the next timestep. A displacement norm is also monitored. If the fluid is incompressible, as blood is, then a small change in the boundary motion can lead to a large change in pressure. The coupling program offers the facility to relax the values passed across the boundary towards those generated at the previous solution. It is our experience that quite high values of relaxation (of the order of 90% or more of the previous solution) are required to achieve convergence, and in extreme conditions convergence might not occur at all. In the course of the BloodSim project satisfactory solutions were obtained for eight out of nine test cases. A mesh of the solid domain is set up in ANSYS. Appropriate boundary conditions are prescribed and the nodes on the wetted boundary are assigned to a component. The fluids mesh is set up in CFX and again appropriate boundary conditions prescribed and the wetted boundary is identified. The CFX Build programme features the facility to read an ANSYS cdb file, and so it is possible to define both meshes within ANSYS if this is preferred. Analysis The program of work was undertaken by a European consortium of industrial and academic users. The technology providers were led by AEA Technology (the developers of CFX), supported by IDAC (a European ANSYS distributor), ASD (expert on blood damage and haemodynamic modeling) and PFD (for dissemination and exploitation in chemical plant simulation). The end users were led by Medical Physics at the University of Sheffield, with industrial support and input from the Berlin Heart Institute (Cardiac Assist Device), Angiomed and Medtronic AVE (stent manufacturers), and Autogenics (Tissue Heart Valve Prostheses). Sheffield had a dual role as technology provider and end user. At the start of the program a series of eight test and validation cases were prescribed. The first was a development vehicle, representing pulsatile flow in an elastic-walled vessel, for which linearised analytical solutions are available. Two were simplified representations of coupled systems for which experimental results were available. Four were direct simulations of devices of direct interest to the industrial partners. Simulations were also performed of an in vivo treatment procedure involving the stenting of a coronary arterty. In this paper we present a brief overview of results from the elastic-walled tube, for a tube containing a stent and for the Cardiac Assist Device.

3 Analysis Results & Discussion A comprehensive description of the results of a series of eight validation tests and a case study is presented in the final technical report for the project 7. Elastic Tube The first test vehicle was the elastic tube. The Moens Korteweg solution for the speed of progression, c 0, of a wave in a fluid of density ρ in an elastic tube of Young's modulus E and wall thickness t is: Et c0 =. 2Rρ This equation is based on assumptions of an incompressible inviscid fluid and linear elastic displacement of the tube. A modification by Womersley 8 to introduce viscosity and longitudinal tethering results in a phase difference between pressure and flow waves. The modified wavespeed for a wave of frequency ω is: 1 F 3 / J ( ) c = c0, where 1 i α 1 [ ] υ 3 / ( 3 / = 1 F. i J i ) α α α is the dimensionless Womersley parameter, where α 2 =R 2 ωρ/µ (µ is the fluid viscosity), and J 0,J 1 are Bessel functions of order zero and one respectively. Analyses were performed for a vessel of dimensions similar to those of a small artery. One quarter of the vessel was modeled with appropriate symmetry conditions on the boundaries. A transient pressure in the form of a Fourier series was applied to the inlet, with zero pressure specified at the outlet. Results are illustrated in figure 1. The pressure and wall displacement wave travels along the vessel at a finite speed of magnitude consistent with that computed from the Womersley solution. There is significant axial dispersion of the wave as it travels along the vessel. Investigations continue to check the validity of this dispersion. The analytical solution does not recognize any radial variation of pressure (dp/dr =0), wheras in the computational solution there is significant radial variation, particularly close to the moving wall.

4 Figure 1 - Travelling wave in elastic walled tube: Pressure and radial displacement (Snapshot from Justin's latest avi) Earlier analyses had indicated that the computed wavespeed varied with the square root of Young's modulus over the range 0.5 to 8 MPa, typical of literature values for the tangent modulus of arterial wall at physiological strains. An analysis was also performed with a hyperelastic wall model more consistent with arterial material characteristics and, although no analytical solution was available for comparison, plausible results were obtained. The ready implementation of the wide range of material models available in ANSYS is one of the justifications for the multi-code approach to the solid-fluid coupling problem. Detailed analyses were performed of a segment of the tube with a prescribed sinusoidal pressure at inlet and outlet. The anticipated velocity solution, w, a complex function of radius and time, was computed from the Womersley solutions for the elastic tube. 3 / 2 ( α y i ) ( ) i e 3 / 2 0 α i A * J = 0 ω t ω 1 iωρ J The computed radial velocity profiles and temporal peak velocity profiles are compared with the analytical values in figure 2. There was good agreement during the positive pressure phase between the computed velocity profile at each instant in time and the analytical solution. It was interesting and encouraging to note that the tube buckled during the negative pressure phase, and that significant distortion of the mesh was possible before the solution process failed. This is illustrated in figure 3.

5 Figure 2 - Comparison between numerical and analytical results for elastic walled tube (Composite of Figures 1.29 through 1.32, Final Deliverable D4.1) Figure 3 - Buckled Tube during external pressure phase (Composite of figures 1.33 and 1.34 from final report)

6 Stented Artery Balloon angioplasty is a treatment for diseased arteries. An uninflated balloon on a catheter wire is guided along the artery to the site of a partial occlusion, or stenosis, that has been identified clinically as producing an excessive restriction to flow, or an excessive pressure drop. The balloon is inflated to break up the plaques in the wall of the vessel that form the stenosis. There is a significant failure rate in this operation, associated with the relatively short term re-occurrence of the stenosis. Stents are wire scaffold devices introduced into the diseased arteries to attempt to prevent restenosis. Two of the companies involved in the BloodSim program are stent manufacturers, and stenting is an important application of the analysis code. It was considered necessary that the analysis should explicitly model the wires of the stent, because the flow disturbance associated with their intrusion into the fluid domain might promote separation and other fluid dynamic processes associated with the short and long term patency of the device. The modeling of the deployment of a stent is a significant undertaking in its own right 9, and it was not within the remit of the BloodSim program to perform detail modeling of this process. To simplify the model construction process, a metal stent was expanded thermally to expand an artery locally. Contact was defined between stent and artery. The artery tends to 'quilt' through the gaps between the wires of the stent. An illustration of the quilting effect on an idealised stent geometry is presented in figure 4. Typical coupled analysis results are indicated in figure 5. The displacement results are shown relative to the initial state of the tubing after the deployment of the stent. This represents the displacements caused purely by the fluid loading conditions and not by the force of the stent on the tubing. The fluid results show the presence of a linear pressure gradient with undeveloped flow profiles at both inlet and outlet. The contact pressure of the stent wires on the wall of the artery holds the artery at a fixed radius at these locations, because the applied arterial fluid pressure is not sufficient to lift the vessel away from the stent. In between the stent wires the artery wall pulses in synchrony with the fluid pressure. This variation in fluid domain geometry has a significant effect on the local fluid dynamics at the wall of the vessel. Since local wall shear stress and 'fluid age', or residence time, have been implicated in thrombotic and neo-endothelialisation processes it is suggested that the detail assessment of these parameters might represent an important tool in the stent design process. At this point in time the primary value would be for device comparison and incremental evolution because, in common with many other physiological design processes, quantitative data relating absolute magnitudes of physical parameters to clinical consequence are unavailable. Figure 4 - Idealised stent deployed in elastic artery (Composite of figures 7.16 and 7.17

7 Figure 5 - Radial displacement and fluid pressure along a generator at an instant in time in coupled simulation of idealized stented artery (Composite of 7.20 and 7.21) A model of a real stent geometry was constructed. The applied boundary conditions were a downstream pressure and an upstream flow rate, both functions of time. Results at a snapshot in time are illustrated in figure 6. A test rig was constructed to measure the transient pressure drop across the stented vessel during the application of an appropriate flow waveform. Results for the measured pressure drop over time are compared with those from a coupled analysis of a real stent geometry in figure 7. Gross qualitative agreement was found, but the accurate measurement of transient pressure drop in the experimental system proved difficult. This is illustrated in figure 8, in which total system pressures and measurements of difference and differential pressures are presented. The pressure drop across the stented segment is only a small proportion of system pressure. Clearly it is important in the coupled simulation to apply the appropriate system pressure in order to expand and to stress the vessel in accordance with the cardiovascular pressure waveform, whilst at the same time achieving the right pressure drop to generate the right amount of flow. For an equivalent rigid walled analysis of flow of an incompressible fluid only the pressure differential need be specified. A consistent theme in the application of coupled analysis to real physiological problems is the great care required in the specification of appropriate boundary conditions. Integration with external system models, as described by Formaggia et al 2, is represents a productive area of research for coupled systems. The coupling software developed in the current program supports a simple Windkessel model at both inlet and outlet, so that boundary pressures can be adjusted as a function of flow and flow gradient. This feature has proved invaluable for the simulation of medical devices, including the Berlin Heart, discussed in the next section.

8 Figure 6 - Stented vessel and results at an instant in time (Composite of 7.27 and 7.29) Figure 7 - Test rig for stented vessel and comparison between measured and simulated pressure drops (Composite of 7.5, 7.28)

9 Figure 8 - System and differential pressure measurements in stented artery test rig (Composite of figure 7.10 and 7.11) Berlin Heart The elastic artery and the stented vessel feature relatively small displacements. Many medical devices, such as heart valve prostheses, undergo very large displacement in the normal course of operation. Indeed in these systems topological changes to the mesh are required during the course of the simulation. Automatic remeshing and results interpolation are required features for an analysis system. Berlin Heart AG, members of the BloodSim program, have produced an extracorporeal blood pump designed to assist the heart, sometimes as a bridge to transplant. This device features large displacements and coupling of solid and fluid phases. One of the Berlin designs features a blood chamber bounded by two opposed flexible roll membranes, with valves at inlet and outlet. The device fills from the left ventricle of the patient heart and expels the blood under pressure into the aorta. During the fill phase the membranes move apart under the pressure generated by the left ventricle, providing a relatively low resistance to flow and thus relatively low load on the ventricle. During the pump phase the membranes are driven by external pistons to pump blood into the aorta. The valves at inlet and outlet control the direction of flow. Coupled simulation of this device has been undertaken by Berlin Heart AG, supported by Sheffield University. The geometry for both the solid and the fluid mesh models was imported directly from generic CAD models (via the IGES format) into the respective Cfx and Ansys pre-processors. This ensures that consistent mesh models can be obtained directly from the Berlin Heart designers, and that the solid and fluid domains overlap correctly at the solid-fluid coupling interface. A time-dependent velocity function was prescribed at the inlet to simulate the flow from the ventricle, and a Windkessel opening was specified at the outlet. A simple resistance model was specified at the outlet, with pressure proportional to instantaneous flow. For the pump phase the resistance was assigned a value of 2x10 8 PaSecm -3, consistent with a pressure increase of about 120mmHg at the peak outflow rate. For the fill phase the value is essentially arbitrary: it must be large enough to prevent significant leakage at the outlet, but small enough not to cause coupling instability A value of 8.3 x10 7 PaSecm -3 was found to limit outflow during filling, whilst maintaining stability of the analysis. Once again this analysis highlighted the requirement for careful specification of bpundary conditions for the coupled analysis. The deformation of the membrane during the fill phase of the pump cycle is illustrated in figure 9, together with an indication of the massless particle pathlines. These show how the fluid enters the domain and fills the void vacated by the deforming membrane. The pressure in the domain is determined by the stiffness and displacement of the membrane, with a controlled leakage through the outlet. In;let and outlet flow rates during a simulation cycle are illustrated in figure 10.

10 Figure 9 - Simulation of the operation of a Berlin Heart - membrane displacement and particle paths (D4.1c, version3.1, figure 6.7) Figure 10 - Flowrate at inlet and outlet over one simulated pulse (D4.1c, version3.1, figure 6.8) Conclusion Coupling software has been developed to interface ANSYS to CFX, iterating across the wetted boundary until pressure and displacement are converged. The software has been applied to the simulation of several cardiovascular and biomedical systems with encouraging results. Although significant development tasks

11 remain, the software represents an important resource able to address leading edge design and research questions for the biomedical community. It is apparent that specification of appropriate boundary conditions for coupled analyses is an issue that requires careful consideration in the analysis planning phase, as well as appropriate functionality in the software. References 1. MpCCI - Mesh-based parallel Code Coupling Interface, 2. Formaggia L, Gerbau JF, Nobile F, Quarteroni A, On the Coupling of 3D and 1D Navier Stokes Equations for Flow Problems in Compliant Vessels, Zhao SZ, Xu XY, et al. The numerical analysis of fluid-solid interactions for blood flow in arterial structures - Part 2: development of coupled fluid-solid algorithms. Proceedings of the Institution of Mechanical Engineers Part H-Journal of Engineering in Medicine 212(H4): , Klein A, Gerlach G, Simulation of fluid-structure interaction in micropumps by coupling of two commercial finite-element programmes. 5. Hawkins I, Wilkes N. Moving Grids in Harwell-FLOW3D, AEA-InTech-0608, JMT Penrose, CJ Staples, Implicit Fluid Structure Coupling for Simulation of Cardiovascular Problems, Accepted for publication in the International Journal of Numerical Methods in Fluids, November Penrose JMT, Narracott A, Jones IP, Hose DR, Validation Report D4.1c, BloodSim Project EP28350, CEC IT Program, Framework 4, Womersley J, Oscillatory flow in arteries: the constrained elastic tube as a model of arterial flow and pulse transmission. Physics in Medicine and Biology 2: , Narracott AJ, Balloon Folding Influences Stent Deployment, PhD Thesis, University of Sheffield, 2001

Isogeometric Analysis of Fluid-Structure Interaction

Isogeometric Analysis of Fluid-Structure Interaction Isogeometric Analysis of Fluid-Structure Interaction Y. Bazilevs, V.M. Calo, T.J.R. Hughes Institute for Computational Engineering and Sciences, The University of Texas at Austin, USA e-mail: {bazily,victor,hughes}@ices.utexas.edu

More information

Life Sciences Applications: Modeling and Simulation for Biomedical Device Design SGC 2013

Life Sciences Applications: Modeling and Simulation for Biomedical Device Design SGC 2013 Life Sciences Applications: Modeling and Simulation for Biomedical Device Design Kristian.Debus@cd-adapco.com SGC 2013 Modeling and Simulation for Biomedical Device Design Biomedical device design and

More information

NUMERICAL STUDY OF BLOOD FLOW IN A VESSEL WITH INCREASING DEGREE OF STENOSIS USING DYNAMIC MESHES

NUMERICAL STUDY OF BLOOD FLOW IN A VESSEL WITH INCREASING DEGREE OF STENOSIS USING DYNAMIC MESHES XIII CONGRESO INTERNACIONAL DE INGENIERÍA DE PROYECTOS Badajoz, 8-10 de julio de 2009 NUMERICAL STUDY OF BLOOD FLOW IN A VESSEL WITH INCREASING DEGREE OF STENOSIS USING DYNAMIC MESHES Ana Cristina Ferreira,

More information

CFD Simulation of a dry Scroll Vacuum Pump including Leakage Flows

CFD Simulation of a dry Scroll Vacuum Pump including Leakage Flows CFD Simulation of a dry Scroll Vacuum Pump including Leakage Flows Jan Hesse, Rainer Andres CFX Berlin Software GmbH, Berlin, Germany 1 Introduction Numerical simulation results of a dry scroll vacuum

More information

Webinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines

Webinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines Webinar: TwinMesh for Reliable CFD Analysis of Rotating Positive Displacement Machines 14.07.2015 Dipl.-Ing. Jan Hesse Jan.hesse@cfx-berlin.de CFX Berlin Software GmbH Karl-Marx-Allee 90 A 10243 Berlin

More information

CFD simulations of blood flow through abdominal part of aorta

CFD simulations of blood flow through abdominal part of aorta CFD simulations of blood flow through abdominal part of aorta Andrzej Polanczyk, Aleksandra Piechota Faculty of Process and Enviromental Engineering, Technical University of Lodz, Wolczanska 13 90-94 Lodz,

More information

Three Dimensional Numerical Simulation of Turbulent Flow Over Spillways

Three Dimensional Numerical Simulation of Turbulent Flow Over Spillways Three Dimensional Numerical Simulation of Turbulent Flow Over Spillways Latif Bouhadji ASL-AQFlow Inc., Sidney, British Columbia, Canada Email: lbouhadji@aslenv.com ABSTRACT Turbulent flows over a spillway

More information

Fluid-Structure Interaction Model of Active Eustachian Tube Function in Healthy Adult Patients

Fluid-Structure Interaction Model of Active Eustachian Tube Function in Healthy Adult Patients Excerpt from the Proceedings of the COMSOL Conference 2008 Boston Fluid-Structure Interaction Model of Active Eustachian Tube Function in Healthy Adult Patients Sheer, F.J. 1, Ghadiali, S.N. 1,2 1 Mechanical

More information

The viscous forces on the cylinder are proportional to the gradient of the velocity field at the

The viscous forces on the cylinder are proportional to the gradient of the velocity field at the Fluid Dynamics Models : Flow Past a Cylinder Flow Past a Cylinder Introduction The flow of fluid behind a blunt body such as an automobile is difficult to compute due to the unsteady flows. The wake behind

More information

Introduction to C omputational F luid Dynamics. D. Murrin

Introduction to C omputational F luid Dynamics. D. Murrin Introduction to C omputational F luid Dynamics D. Murrin Computational fluid dynamics (CFD) is the science of predicting fluid flow, heat transfer, mass transfer, chemical reactions, and related phenomena

More information

Using a Single Rotating Reference Frame

Using a Single Rotating Reference Frame Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is

More information

CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence

CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence CFD Analysis of 2-D Unsteady Flow Past a Square Cylinder at an Angle of Incidence Kavya H.P, Banjara Kotresha 2, Kishan Naik 3 Dept. of Studies in Mechanical Engineering, University BDT College of Engineering,

More information

Mesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley

Mesh Morphing and the Adjoint Solver in ANSYS R14.0. Simon Pereira Laz Foley Mesh Morphing and the Adjoint Solver in ANSYS R14.0 Simon Pereira Laz Foley 1 Agenda Fluent Morphing-Optimization Feature RBF Morph with ANSYS DesignXplorer Adjoint Solver What does an adjoint solver do,

More information

CFD MODELING FOR PNEUMATIC CONVEYING

CFD MODELING FOR PNEUMATIC CONVEYING CFD MODELING FOR PNEUMATIC CONVEYING Arvind Kumar 1, D.R. Kaushal 2, Navneet Kumar 3 1 Associate Professor YMCAUST, Faridabad 2 Associate Professor, IIT, Delhi 3 Research Scholar IIT, Delhi e-mail: arvindeem@yahoo.co.in

More information

Case Study- Importing As-Molded Plastic Part Conditions into CAE tools

Case Study- Importing As-Molded Plastic Part Conditions into CAE tools 1 IEI Innova Engineering 1 Park Plaza Suite 980 Irvine, California 92614 Case Study- Importing As-Molded Plastic Part Conditions into CAE tools 2 CONTENTS CONTENTS... 2 EXECUTIVE SUMMARY... 3 APPROACH...

More information

Mutltiphysics for Ironcad Demonstration Models (Rev. 1.1)

Mutltiphysics for Ironcad Demonstration Models (Rev. 1.1) Centrifuge Model The centrifuge model demonstrates how to perform a rotational spinning centrifugal load analysis. It also demonstrates how to group different parts with/without the intended initial bonding

More information

Tutorial School on Fluid Dynamics: Topics in Turbulence May 24-28, 2010

Tutorial School on Fluid Dynamics: Topics in Turbulence May 24-28, 2010 Applications of Large-eddy Simulation to Biological Flows Tutorial School on Fluid Dynamics: Topics in Turbulence May 24-28, 2010 Methodologies & Applications Elias Balaras Fischell Department of Bioengineering

More information

Comparison of Classic and Finned Piston Reciprocating Linear Air Compressor Using COMSOL Multiphysics

Comparison of Classic and Finned Piston Reciprocating Linear Air Compressor Using COMSOL Multiphysics Comparison of Classic and Finned Piston Reciprocating Linear Air Compressor Using COMSOL Multiphysics M. Heidari*, P. Barrade, and A. Rufer LEI, École Polytechnique Fédérale de Lausanne, Lausanne, Switzerland

More information

A Workflow for Computational Fluid Dynamics Simulations using Patient-Specific Aortic Models

A Workflow for Computational Fluid Dynamics Simulations using Patient-Specific Aortic Models 2.8.8 A Workflow for Computational Fluid Dynamics Simulations using Patient-Specific Aortic Models D. Hazer 1,2, R. Unterhinninghofen 2, M. Kostrzewa 1, H.U. Kauczor 3, R. Dillmann 2, G.M. Richter 1 1)

More information

CFD design tool for industrial applications

CFD design tool for industrial applications Sixth LACCEI International Latin American and Caribbean Conference for Engineering and Technology (LACCEI 2008) Partnering to Success: Engineering, Education, Research and Development June 4 June 6 2008,

More information

Introduction to ANSYS CFX

Introduction to ANSYS CFX Workshop 03 Fluid flow around the NACA0012 Airfoil 16.0 Release Introduction to ANSYS CFX 2015 ANSYS, Inc. March 13, 2015 1 Release 16.0 Workshop Description: The flow simulated is an external aerodynamics

More information

Marine Hydrodynamics Solver in OpenFOAM

Marine Hydrodynamics Solver in OpenFOAM Marine Hydrodynamics Solver in OpenFOAM p. 1/14 Marine Hydrodynamics Solver in OpenFOAM Hrvoje Jasak and Henrik Rusche h.jasak@wikki.co.uk, h.rusche@wikki.co.uk Wikki, United Kingdom and Germany 4 December

More information

FLUID MECHANICS TESTS

FLUID MECHANICS TESTS FLUID MECHANICS TESTS Attention: there might be more correct answers to the questions. Chapter 1: Kinematics and the continuity equation T.2.1.1A flow is steady if a, the velocity direction of a fluid

More information

CFD Simulation of a Dry Scroll Vacuum Pump Including Leakage Flows

CFD Simulation of a Dry Scroll Vacuum Pump Including Leakage Flows Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2016 CFD Simulation of a Dry Scroll Vacuum Pump Including Leakage Flows Jan Hesse CFX Berlin

More information

Using MSC.Nastran for Explicit FEM Simulations

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

More information

Guidelines for proper use of Plate elements

Guidelines for proper use of Plate elements Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known

More information

Acknowledgements. Prof. Dan Negrut Prof. Darryl Thelen Prof. Michael Zinn. SBEL Colleagues: Hammad Mazar, Toby Heyn, Manoj Kumar

Acknowledgements. Prof. Dan Negrut Prof. Darryl Thelen Prof. Michael Zinn. SBEL Colleagues: Hammad Mazar, Toby Heyn, Manoj Kumar Philipp Hahn Acknowledgements Prof. Dan Negrut Prof. Darryl Thelen Prof. Michael Zinn SBEL Colleagues: Hammad Mazar, Toby Heyn, Manoj Kumar 2 Outline Motivation Lumped Mass Model Model properties Simulation

More information

NUMERICAL SIMULATION OF SHALLOW WATERS EFFECTS ON SAILING SHIP "MIRCEA" HULL

NUMERICAL SIMULATION OF SHALLOW WATERS EFFECTS ON SAILING SHIP MIRCEA HULL NUMERICAL SIMULATION OF SHALLOW WATERS EFFECTS ON SAILING SHIP "MIRCEA" HULL Petru Sergiu ȘERBAN 1 1 PhD Student, Department of Navigation and Naval Transport, Mircea cel Batran Naval Academy, Constanța,

More information

Wall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3,

Wall thickness= Inlet: Prescribed mass flux. All lengths in meters kg/m, E Pa, 0.3, Problem description Problem 30: Analysis of fluid-structure interaction within a pipe constriction It is desired to analyze the flow and structural response within the following pipe constriction: 1 1

More information

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

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

More information

Rotating Moving Boundary Analysis Using ANSYS 5.7

Rotating Moving Boundary Analysis Using ANSYS 5.7 Abstract Rotating Moving Boundary Analysis Using ANSYS 5.7 Qin Yin Fan CYBERNET SYSTEMS CO., LTD. Rich Lange ANSYS Inc. As subroutines in commercial software, APDL (ANSYS Parametric Design Language) provides

More information

Advanced ANSYS FLUENT Acoustics

Advanced ANSYS FLUENT Acoustics Workshop Modeling Flow-Induced (Aeroacoustic) Noise 14.5 Release Advanced ANSYS FLUENT Acoustics 2011 ANSYS, Inc. November 7, 2012 1 Introduction This tutorial demonstrates how to model 2D turbulent flow

More information

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

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

More information

CFD Topology Optimization of Automotive Components

CFD Topology Optimization of Automotive Components CFD Topology Optimization of Automotive Components Dr.-Ing. Markus Stephan, Dr.-Ing. Dipl.-Phys. Pascal Häußler, Dipl.-Math. Michael Böhm FE-DESIGN GmbH, Karlsruhe, Germany Synopsis Automatic CFD optimization

More information

Realtime Water Simulation on GPU. Nuttapong Chentanez NVIDIA Research

Realtime Water Simulation on GPU. Nuttapong Chentanez NVIDIA Research 1 Realtime Water Simulation on GPU Nuttapong Chentanez NVIDIA Research 2 3 Overview Approaches to realtime water simulation Hybrid shallow water solver + particles Hybrid 3D tall cell water solver + particles

More information

Behaviour of cold bent glass plates during the shaping process

Behaviour of cold bent glass plates during the shaping process Behaviour of cold bent glass plates during the shaping process Kyriaki G. DATSIOU *, Mauro OVEREND a * Department of Engineering, University of Cambridge Trumpington Street, Cambridge, CB2 1PZ, UK kd365@cam.ac.uk

More information

Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts

Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Fabio Kasper Comparison Between Numerical & PIV Experimental Results for Gas-Solid Flow in Ducts Rodrigo Decker, Oscar Sgrott Jr., Henry F. Meier Waldir Martignoni Agenda Introduction The Test Bench Case

More information

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution.

Use 6DOF solver to calculate motion of the moving body. Create TIFF files for graphic visualization of the solution. Introduction The purpose of this tutorial is to provide guidelines and recommendations for setting up and solving a moving deforming mesh (MDM) case along with the six degree of freedom (6DOF) solver and

More information

Use of numerical flow simulations (CFD) for optimising heat exchangers

Use of numerical flow simulations (CFD) for optimising heat exchangers www.guentner.eu Technical article from 03.04.2017 Author Dr. Andreas Zürner Research Güntner GmbH & Co. KG Use of numerical flow simulations (CFD) for optimising heat exchangers Numerical flow simulations

More information

Fluent User Services Center

Fluent User Services Center Solver Settings 5-1 Using the Solver Setting Solver Parameters Convergence Definition Monitoring Stability Accelerating Convergence Accuracy Grid Independence Adaption Appendix: Background Finite Volume

More information

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil

Verification and Validation of Turbulent Flow around a Clark-Y Airfoil Verification and Validation of Turbulent Flow around a Clark-Y Airfoil 1. Purpose 58:160 Intermediate Mechanics of Fluids CFD LAB 2 By Tao Xing and Fred Stern IIHR-Hydroscience & Engineering The University

More information

Use of CFD in Design and Development of R404A Reciprocating Compressor

Use of CFD in Design and Development of R404A Reciprocating Compressor Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2006 Use of CFD in Design and Development of R404A Reciprocating Compressor Yogesh V. Birari

More information

SIMULATION OF A DETONATION CHAMBER TEST CASE

SIMULATION OF A DETONATION CHAMBER TEST CASE SIMULATION OF A DETONATION CHAMBER TEST CASE Daniel Hilding Engineering Research Nordic AB Garnisonen I4, Byggnad 5 SE-582 10 Linköping www.erab.se daniel.hilding@erab.se Abstract The purpose of a detonation

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 16. Modeling Evaporating Liquid Spray Introduction In this tutorial, FLUENT s air-blast atomizer model is used to predict the behavior of an evaporating methanol spray. Initially, the air flow

More information

ANSYS Workbench Guide

ANSYS Workbench Guide ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through

More information

SPH: Towards the simulation of wave-body interactions in extreme seas

SPH: Towards the simulation of wave-body interactions in extreme seas SPH: Towards the simulation of wave-body interactions in extreme seas Guillaume Oger, Mathieu Doring, Bertrand Alessandrini, and Pierre Ferrant Fluid Mechanics Laboratory (CNRS UMR6598) Ecole Centrale

More information

Backward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn

Backward facing step Homework. Department of Fluid Mechanics. For Personal Use. Budapest University of Technology and Economics. Budapest, 2010 autumn Backward facing step Homework Department of Fluid Mechanics Budapest University of Technology and Economics Budapest, 2010 autumn Updated: October 26, 2010 CONTENTS i Contents 1 Introduction 1 2 The problem

More information

2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube

2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube 2008 International ANSYS Conference Strongly Coupled FSI Simulation Moving Compressible Pressure Pulse through a Tube Daniel L. Cler, US Army RDECOM/ ARDEC/ WSEC/ Benet Labs 1 Overview Background Problem

More information

Support for Multi physics in Chrono

Support for Multi physics in Chrono Support for Multi physics in Chrono The Story Ahead Overview of multi physics strategy in Chrono Summary of handling rigid/flexible body dynamics using Lagrangian approach Summary of handling fluid, and

More information

Summary of the main PROBAND project results

Summary of the main PROBAND project results Summary of the main PROBAND project results WP2: WP2 was dedicated to the development and validation broadband noise prediction methods. Once validated on non rotating airfoils in WP2, these methods were

More information

Grid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam)

Grid. Apr 09, 1998 FLUENT 5.0 (2d, segregated, lam) Grid. Jul 31, 1998 FLUENT 5.0 (2d, segregated, lam) Tutorial 2. Around an Airfoil Transonic Turbulent Flow Introduction: The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a non-zero angle of attack. You will use the

More information

FOUR WHAT S NEW IN THIS VERSION? 4.1 FLOW-3D Usability CHAPTER

FOUR WHAT S NEW IN THIS VERSION? 4.1 FLOW-3D Usability CHAPTER CHAPTER FOUR WHAT S NEW IN THIS VERSION? FLOW-3D v11.2.0 continues to streamline engineers simulation workflows by enabling them to more quickly set up simulations, avoid common errors, identify and enter

More information

Continuum-Microscopic Models

Continuum-Microscopic Models Scientific Computing and Numerical Analysis Seminar October 1, 2010 Outline Heterogeneous Multiscale Method Adaptive Mesh ad Algorithm Refinement Equation-Free Method Incorporates two scales (length, time

More information

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent

Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent MEGR 7090-003, Computational Fluid Dynamics :1 7 Spring 2015 Computational Study of Laminar Flowfield around a Square Cylinder using Ansys Fluent Rahul R Upadhyay Master of Science, Dept of Mechanical

More information

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil

Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Express Introductory Training in ANSYS Fluent Workshop 04 Fluid Flow Around the NACA0012 Airfoil Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School 2013 -

More information

RSNA 2016 Introduction to Computational Fluid Dynamics from Medical Images: A Step-by-Step Demonstration (Hands-on) Training Guide

RSNA 2016 Introduction to Computational Fluid Dynamics from Medical Images: A Step-by-Step Demonstration (Hands-on) Training Guide RSNA 2016 Introduction to Computational Fluid Dynamics from Medical Images: A Step-by-Step Demonstration (Hands-on) Training Guide Dimitris Mitsouras Course Director Applied Imaging Science Lab Boston,

More information

Recent Approaches of CAD / CAE Product Development. Tools, Innovations, Collaborative Engineering.

Recent Approaches of CAD / CAE Product Development. Tools, Innovations, Collaborative Engineering. Recent Approaches of CAD / CAE Product Development. Tools, Innovations, Collaborative Engineering. Author: Dr.-Ing. Peter Binde Abstract: In this paper, the latest approaches in the field of CAD-CAE product

More information

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

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

More information

ixcube 4-10 Brief introduction for membrane and cable systems.

ixcube 4-10 Brief introduction for membrane and cable systems. ixcube 4-10 Brief introduction for membrane and cable systems. ixcube is the evolution of 20 years of R&D in the field of membrane structures so it takes a while to understand the basic features. You must

More information

Keywords Fluid dynamics, turbulence, computational fluid dynamics, CFD, fluidized bed, computing

Keywords Fluid dynamics, turbulence, computational fluid dynamics, CFD, fluidized bed, computing Bakker A., Marshall E.M. (2004) Computational Fluid Dynamics. Encyclopedia of Chemical Processing. Editor Prof. Sunggyu Lee. Marcel Dekker Inc. New York. Computational Fluid Dynamics André Bakker and Elizabeth

More information

Modeling Evaporating Liquid Spray

Modeling Evaporating Liquid Spray Tutorial 17. Modeling Evaporating Liquid Spray Introduction In this tutorial, the air-blast atomizer model in ANSYS FLUENT is used to predict the behavior of an evaporating methanol spray. Initially, the

More information

Steady Flow: Lid-Driven Cavity Flow

Steady Flow: Lid-Driven Cavity Flow STAR-CCM+ User Guide Steady Flow: Lid-Driven Cavity Flow 2 Steady Flow: Lid-Driven Cavity Flow This tutorial demonstrates the performance of STAR-CCM+ in solving a traditional square lid-driven cavity

More information

APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3

APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 APPLIED COMPUTATIONAL FLUID DYNAMICS-PROJECT-3 BY SAI CHAITANYA MANGAVELLI Common Setup Data: 1) Mesh Proximity and Curvature with Refinement of 2. 2) Double Precision and second order for methods in Solver.

More information

Simulation of Laminar Pipe Flows

Simulation 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 information

Module 1 Lecture Notes 2. Optimization Problem and Model Formulation

Module 1 Lecture Notes 2. Optimization Problem and Model Formulation Optimization Methods: Introduction and Basic concepts 1 Module 1 Lecture Notes 2 Optimization Problem and Model Formulation Introduction In the previous lecture we studied the evolution of optimization

More information

Die Wear Profile Investigation in Hot Forging

Die Wear Profile Investigation in Hot Forging Die Wear Profile Investigation in Hot Forging F. R. Biglari, M Zamani Abstract In this study, the wear profile on the die surface during the hot forging operation for an axisymmetric cross-section is examined.

More information

Fluid-Structure Interaction Modeling of High-Aspect Ratio Nuclear Fuel Plates using COMSOL

Fluid-Structure Interaction Modeling of High-Aspect Ratio Nuclear Fuel Plates using COMSOL Fluid-Structure Interaction Modeling of High-Aspect Ratio Nuclear Fuel Plates using COMSOL Franklin Curtis 1 Kivanc Ekici 1 James Freels 2 1 University of Tennessee, Knoxville, TN 2 Oak Ridge National

More information

Numerical Methods for (Time-Dependent) HJ PDEs

Numerical Methods for (Time-Dependent) HJ PDEs Numerical Methods for (Time-Dependent) HJ PDEs Ian Mitchell Department of Computer Science The University of British Columbia research supported by National Science and Engineering Research Council of

More information

Analysis of a curvature corrected turbulence model using a 90 degree curved geometry modelled after a centrifugal compressor impeller

Analysis of a curvature corrected turbulence model using a 90 degree curved geometry modelled after a centrifugal compressor impeller Analysis of a curvature corrected turbulence model using a 90 degree curved geometry modelled after a centrifugal compressor impeller K. J. Elliott 1, E. Savory 1, C. Zhang 1, R. J. Martinuzzi 2 and W.

More information

CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force

CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the

More information

Adjoint Solver Workshop

Adjoint Solver Workshop Adjoint Solver Workshop Why is an Adjoint Solver useful? Design and manufacture for better performance: e.g. airfoil, combustor, rotor blade, ducts, body shape, etc. by optimising a certain characteristic

More information

Interaction of Fluid Simulation Based on PhysX Physics Engine. Huibai Wang, Jianfei Wan, Fengquan Zhang

Interaction of Fluid Simulation Based on PhysX Physics Engine. Huibai Wang, Jianfei Wan, Fengquan Zhang 4th International Conference on Sensors, Measurement and Intelligent Materials (ICSMIM 2015) Interaction of Fluid Simulation Based on PhysX Physics Engine Huibai Wang, Jianfei Wan, Fengquan Zhang College

More information

Tutorial. BOSfluids. Water hammer (part 3) Dynamic Analysis using Caesar II

Tutorial. BOSfluids. Water hammer (part 3) Dynamic Analysis using Caesar II BOSfluids Tutorial Water hammer (part 3) Dynamic Analysis using Caesar II The Water hammer tutorial is a 3 part tutorial describing the phenomena of water hammer in a piping system and how BOSfluids can

More information

Simulating the Suspension Response of a High Performance Sports Car

Simulating the Suspension Response of a High Performance Sports Car Simulating the Suspension Response of a High Performance Sports Car Paul Burnham McLaren Automotive McLaren Technology Centre, Chertsey Road, Woking, Surrey, GU21 4YH paul.burnham@mclaren.com Abstract

More information

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes

Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Express Introductory Training in ANSYS Fluent Workshop 06 Using Moving Reference Frames and Sliding Meshes Dimitrios Sofialidis Technical Manager, SimTec Ltd. Mechanical Engineer, PhD PRACE Autumn School

More information

LS-Dyna CAE A ssociates Associates

LS-Dyna CAE A ssociates Associates LS-Dyna at CAE Associates Overview Experience with LS-Dyna for Dynamics Modeling CAE Associates engineers have nearly 30 years of experience using explicit dynamics finite element codes for complex design

More information

Benchmark of Topology Optimization Methods for Crashworthiness Design

Benchmark of Topology Optimization Methods for Crashworthiness Design 12 th International LS-DYNA Users Conference Optimization(2) Benchmark of Topology Optimization Methods for Crashworthiness Design C. H. Chuang and R. J. Yang Ford Motor Company Abstract Linear structural

More information

TryItNow! Step by Step Walkthrough: Spoiler Support

TryItNow! Step by Step Walkthrough: Spoiler Support TryItNow! Step by Step Walkthrough: Spoiler Support 1 2015 ANSYS, Inc. March 28, 2016 TryItNow! Step by Step Walkthrough: Spoiler Support ANSYS designed this TryItNow! experience to give you quick access

More information

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

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

More information

A kinematically coupled time-splitting scheme for fluid-structure interaction in blood flow

A kinematically coupled time-splitting scheme for fluid-structure interaction in blood flow A kinematically coupled time-splitting scheme for fluid-structure interaction in blood flow Giovanna Guidoboni a Roland Glowinski a,b Nicola Cavallini a,d Suncica Canic a Serguei Lapin c a Department of

More information

Verification and Validation in CFD and Heat Transfer: ANSYS Practice and the New ASME Standard

Verification and Validation in CFD and Heat Transfer: ANSYS Practice and the New ASME Standard Verification and Validation in CFD and Heat Transfer: ANSYS Practice and the New ASME Standard Dimitri P. Tselepidakis & Lewis Collins ASME 2012 Verification and Validation Symposium May 3 rd, 2012 1 Outline

More information

Introduction to the Finite Element Method (3)

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

More information

Application 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 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 information

2D numerical simulation of ocean waves

2D numerical simulation of ocean waves 2D numerical simulation of ocean waves Qingjie. Du,*, Y.C. Dennis. Leung Department of Mechanical Engineering, The University of Hong Kong, Hong Kong, China * Corresponding author. Tel: +852 51743593,

More information

ANSYS AIM 16.0 Overview. AIM Program Management

ANSYS AIM 16.0 Overview. AIM Program Management 1 2015 ANSYS, Inc. September 27, 2015 ANSYS AIM 16.0 Overview AIM Program Management 2 2015 ANSYS, Inc. September 27, 2015 Today s Simulation Challenges Leveraging simulation across engineering organizations

More information

A Graphical User Interface for Simulating Resin-Transfer-Molding Combining LS-DYNA and OpenFOAM

A Graphical User Interface for Simulating Resin-Transfer-Molding Combining LS-DYNA and OpenFOAM A Graphical User Interface for Simulating Resin-Transfer-Molding Combining LS-DYNA and OpenFOAM M. Martins-Wagner 1, M. Wagner 1, A, Haufe 2, C. Liebold 2 1 Ostbayerische Technische Hochschule Regensburg

More information

Numerical Analysis of Shock Tube Problem by using TVD and ACM Schemes

Numerical Analysis of Shock Tube Problem by using TVD and ACM Schemes Numerical Analysis of Shock Tube Problem by using TVD and Schemes Dr. Mukkarum Husain, Dr. M. Nauman Qureshi, Syed Zaid Hasany IST Karachi, Email: mrmukkarum@yahoo.com Abstract Computational Fluid Dynamics

More information

Towards a Fluid Solid Interaction Model of a Dynamic Lung

Towards a Fluid Solid Interaction Model of a Dynamic Lung University of Denver Digital Commons @ DU Electronic Theses and Dissertations Graduate Studies 1-1-2012 Towards a Fluid Solid Interaction Model of a Dynamic Lung Justin Jacobs University of Denver Follow

More information

Pressure Drop Evaluation in a Pilot Plant Hydrocyclone

Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Pressure Drop Evaluation in a Pilot Plant Hydrocyclone Fabio Kasper, M.Sc. Emilio Paladino, D.Sc. Marcus Reis, M.Sc. ESSS Carlos A. Capela Moraes, D.Sc. Dárley C. Melo, M.Sc. Petrobras Research Center

More information

3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation

3D 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 information

Metafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction

Metafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction ALE simulations ua sus using Metafor eao 1. Introduction 2. Operator split 3. Convection schemes 4. Rezoning methods 5. Contact with friction 1 Introduction EULERIAN FORMALISM Undistorted mesh Ideal for

More information

Fluid Motion Between Rotating Concentric Cylinders Using COMSOL Multiphysics

Fluid Motion Between Rotating Concentric Cylinders Using COMSOL Multiphysics Fluid Motion Between Rotating Concentric Cylinders Using COMSOL Multiphysics Kabita Barman 1, Sravanthi Mothupally 1, Archana Sonejee 1, and Patrick L. Mills *1 1 Department of Chemical and Natural Gas

More information

ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity

ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity ANSYS Fluid Structure Interaction for Thermal Management and Aeroelasticity Phil Stopford Duxford Air Museum 11th May 2011 2011 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Fluid Structure

More information

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016

FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 FLUENT Secondary flow in a teacup Author: John M. Cimbala, Penn State University Latest revision: 26 January 2016 Note: These instructions are based on an older version of FLUENT, and some of the instructions

More information

Computational Fluid Dynamics (CFD) for Built Environment

Computational Fluid Dynamics (CFD) for Built Environment Computational Fluid Dynamics (CFD) for Built Environment Seminar 4 (For ASHRAE Members) Date: Sunday 20th March 2016 Time: 18:30-21:00 Venue: Millennium Hotel Sponsored by: ASHRAE Oryx Chapter Dr. Ahmad

More information

Chapter 1 - Basic Equations

Chapter 1 - Basic Equations 2.20 Marine Hydrodynamics, Fall 2017 Lecture 2 Copyright c 2017 MIT - Department of Mechanical Engineering, All rights reserved. 2.20 Marine Hydrodynamics Lecture 2 Chapter 1 - Basic Equations 1.1 Description

More information

Modeling Strategies for Dynamic Finite Element Cask Analyses

Modeling Strategies for Dynamic Finite Element Cask Analyses Session A Package Analysis: Structural Analysis - Modeling Modeling Strategies for Dynamic Finite Element Cask Analyses Uwe Zencker, Günter Wieser, Linan Qiao, Christian Protz BAM Federal Institute for

More information

Flow and Heat Transfer in a Mixing Elbow

Flow and Heat Transfer in a Mixing Elbow Flow and Heat Transfer in a Mixing Elbow Objectives The main objectives of the project are to learn (i) how to set up and perform flow simulations with heat transfer and mixing, (ii) post-processing and

More information

Medical Image Segmentation using Level Sets

Medical Image Segmentation using Level Sets Medical Image Segmentation using Level Sets Technical Report #CS-8-1 Tenn Francis Chen Abstract Segmentation is a vital aspect of medical imaging. It aids in the visualization of medical data and diagnostics

More information

30 th Anniversary Event. New features in Opera By Nigel Atkinson, PhD. OPTIMIZER Automatically selects and manages multiple goalseeking

30 th Anniversary Event. New features in Opera By Nigel Atkinson, PhD. OPTIMIZER Automatically selects and manages multiple goalseeking FEA ANALYSIS General-purpose multiphysics design and analysis software for a wide range of applications OPTIMIZER Automatically selects and manages multiple goalseeking algorithms INTEROPERABILITY Built-in

More information