BloodSim: Coupled Solid-Fluid Simulation of Cardiovascular Systems

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

CPM Specifications Document Healthy Vertebral:

CPM Specifications Document Healthy Vertebral: CPM Specifications Document Healthy Vertebral: OSMSC 0078_0000, 0079_0000, 0166_000, 0167_0000 May 1, 2013 Version 1 Open Source Medical Software Corporation 2013 Open Source Medical Software Corporation.

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

Solved with COMSOL Multiphysics 4.2

Solved with COMSOL Multiphysics 4.2 Peristaltic Pump Solved with COMSOL Multiphysics 4.2 Introduction In a peristaltic pump, rotating rollers squeeze a flexible tube. As the pushed-down rollers move along the tube, fluids in the tube follow

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

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

Application of Finite Volume Method for Structural Analysis

Application of Finite Volume Method for Structural Analysis Application of Finite Volume Method for Structural Analysis Saeed-Reza Sabbagh-Yazdi and Milad Bayatlou Associate Professor, Civil Engineering Department of KNToosi University of Technology, PostGraduate

More information

Example 24 Spring-back

Example 24 Spring-back Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static

More information

Hydro-elastic analysis of a propeller using CFD and FEM co-simulation

Hydro-elastic analysis of a propeller using CFD and FEM co-simulation Fifth International Symposium on Marine Propulsors smp 17, Espoo, Finland, June 2017 Hydro-elastic analysis of a propeller using CFD and FEM co-simulation Vesa Nieminen 1 1 VTT Technical Research Centre

More information

LS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA.

LS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA. 12 th International LS-DYNA Users Conference FSI/ALE(1) LS-DYNA 980 : Recent Developments, Application Areas and Validation Process of the Incompressible fluid solver (ICFD) in LS-DYNA Part 1 Facundo Del

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

Demo problem: Steady finite-reynolds-number flow through an iliac bifurcation

Demo problem: Steady finite-reynolds-number flow through an iliac bifurcation Chapter 1 Demo problem: Steady finite-reynolds-number flow through an iliac bifurcation The purpose of this tutorial is to demonstrate the simulation of cardiovascular fluid mechanics problems with oomph-lib.

More information

Optimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells

Optimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells Excerpt from the Proceedings of the COMSOL Conference 2010 Boston Optimizing Bio-Inspired Flow Channel Design on Bipolar Plates of PEM Fuel Cells James A. Peitzmeier *1, Steven Kapturowski 2 and Xia Wang

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

Step Change in Design: Exploring Sixty Stent Design Variations Overnight

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

More information

CHAPTER 1. Introduction

CHAPTER 1. Introduction ME 475: Computer-Aided Design of Structures 1-1 CHAPTER 1 Introduction 1.1 Analysis versus Design 1.2 Basic Steps in Analysis 1.3 What is the Finite Element Method? 1.4 Geometrical Representation, Discretization

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

1.2 Numerical Solutions of Flow Problems

1.2 Numerical Solutions of Flow Problems 1.2 Numerical Solutions of Flow Problems DIFFERENTIAL EQUATIONS OF MOTION FOR A SIMPLIFIED FLOW PROBLEM Continuity equation for incompressible flow: 0 Momentum (Navier-Stokes) equations for a Newtonian

More information

Reduced Oder Modeling techniques to predict the risk of fatigue fracture of peripheral stents. Michel Rochette

Reduced Oder Modeling techniques to predict the risk of fatigue fracture of peripheral stents. Michel Rochette Reduced Oder Modeling techniques to predict the risk of fatigue fracture of peripheral stents Michel Rochette 1 RT3S: Real Time Simulation for Safer vascular Stenting 2 The vascular disease in peripheral

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

Numerical Wave Tank Modeling of Hydrodynamics of Permeable Barriers

Numerical Wave Tank Modeling of Hydrodynamics of Permeable Barriers ICHE 2014, Hamburg - Lehfeldt & Kopmann (eds) - 2014 Bundesanstalt für Wasserbau ISBN 978-3-939230-32-8 Numerical Wave Tank Modeling of Hydrodynamics of Permeable Barriers K. Rajendra & R. Balaji Indian

More information

Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach

Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach Simulation of In-Cylinder Flow Phenomena with ANSYS Piston Grid An Improved Meshing and Simulation Approach Dipl.-Ing. (FH) Günther Lang, CFDnetwork Engineering Dipl.-Ing. Burkhard Lewerich, CFDnetwork

More information

Eulerian Techniques for Fluid-Structure Interactions - Part II: Applications

Eulerian Techniques for Fluid-Structure Interactions - Part II: Applications Published in Lecture Notes in Computational Science and Engineering Vol. 103, Proceedings of ENUMATH 2013, pp. 755-762, Springer, 2014 Eulerian Techniques for Fluid-Structure Interactions - Part II: Applications

More information

ENERGY-224 Reservoir Simulation Project Report. Ala Alzayer

ENERGY-224 Reservoir Simulation Project Report. Ala Alzayer ENERGY-224 Reservoir Simulation Project Report Ala Alzayer Autumn Quarter December 3, 2014 Contents 1 Objective 2 2 Governing Equations 2 3 Methodolgy 3 3.1 BlockMesh.........................................

More information

VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL

VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models

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

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić

Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions. Milovan Perić Coupling of STAR-CCM+ to Other Theoretical or Numerical Solutions Milovan Perić Contents The need to couple STAR-CCM+ with other theoretical or numerical solutions Coupling approaches: surface and volume

More information

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following:

This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Tutorial 22. Modeling Solidification Introduction This tutorial illustrates how to set up and solve a problem involving solidification. This tutorial will demonstrate how to do the following: Define a

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

2.7 Cloth Animation. Jacobs University Visualization and Computer Graphics Lab : Advanced Graphics - Chapter 2 123

2.7 Cloth Animation. Jacobs University Visualization and Computer Graphics Lab : Advanced Graphics - Chapter 2 123 2.7 Cloth Animation 320491: Advanced Graphics - Chapter 2 123 Example: Cloth draping Image Michael Kass 320491: Advanced Graphics - Chapter 2 124 Cloth using mass-spring model Network of masses and springs

More information

Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)

Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini

More information

INVESTIGATION OF HYDRAULIC PERFORMANCE OF A FLAP TYPE CHECK VALVE USING CFD AND EXPERIMENTAL TECHNIQUE

INVESTIGATION OF HYDRAULIC PERFORMANCE OF A FLAP TYPE CHECK VALVE USING CFD AND EXPERIMENTAL TECHNIQUE International Journal of Mechanical Engineering and Technology (IJMET) Volume 10, Issue 1, January 2019, pp. 409 413, Article ID: IJMET_10_01_042 Available online at http://www.ia aeme.com/ijmet/issues.asp?jtype=ijmet&vtype=

More information

Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine

Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Co-Simulation von Flownex und ANSYS CFX am Beispiel einer Verdrängermaschine Benoit Bosc-Bierne, Dr. Andreas Spille-Kohoff, Farai Hetze CFX Berlin Software GmbH, Berlin Contents Positive displacement compressors

More information

CFD Simulation of Cavitation in an Internal Gear Pump

CFD Simulation of Cavitation in an Internal Gear Pump CFD Simulation of Cavitation in an Internal Gear Pump Dr. Andreas Spille-Kohoff Jan Hesse CFX Berlin Software GmbH Berlin andreas.spille@cfx-berlin.de Contents Introduction Geometry and mesh Simulation

More information

Effect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection

Effect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection Effect of initial turbulence intensity and velocity profile on liquid jets for IFE beamline protection A. Konkachbaev, N.B. Morley and M. A. Abdou Mechanical and Aerospace Engineering Department, UCLA

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

Analysis Comparison between CFD and FEA of an Idealized Concept V- Hull Floor Configuration in Two Dimensions

Analysis Comparison between CFD and FEA of an Idealized Concept V- Hull Floor Configuration in Two Dimensions 2010 NDIA GROUND VEHICLE SYSTEMS ENGINEERING AND TECHNOLOGY SYMPOSIUM MODELING & SIMULATION, TESTING AND VALIDATION (MSTV) MINI-SYMPOSIUM AUGUST 17-19 DEARBORN, MICHIGAN Analysis Comparison between CFD

More information

Good Practice in CFD. A rough guide.

Good Practice in CFD. A rough guide. Good Practice in CFD. A rough guide. Prof. Neil W. Bressloff March 2018 Material covered Introduction External and internal flow The CFD process Geometry, meshing, simulation, post-processing The issues

More information

Facundo DEL PIN / Iñaki ÇALDICHOURY / Rodrigo PAZ / / Livermore Software Technology Corporation

Facundo DEL PIN / Iñaki ÇALDICHOURY / Rodrigo PAZ / / Livermore Software Technology Corporation LS-DYNA R R7 : Strong Fluid Structure Interaction (FSI) capabilities and associated meshing tools for the incompressible CFD solver (ICFD), applications and examples Facundo DEL PIN / Iñaki ÇALDICHOURY

More information

Fluid Structure Modelling of Blood Flow in Vessels

Fluid Structure Modelling of Blood Flow in Vessels Copyright 2014 Tech Science Press MCB, vol.11, no.4, pp.221-234, 2014 Fluid Structure Modelling of Blood Flow in Vessels M. Moatamedi, M. Souli and E. Al-Bahkali Abstract: This paper describes the capabilities

More information

Shape optimisation using breakthrough technologies

Shape optimisation using breakthrough technologies Shape optimisation using breakthrough technologies Compiled by Mike Slack Ansys Technical Services 2010 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary Introduction Shape optimisation technologies

More information

Solving Partial Differential Equations on Overlapping Grids

Solving Partial Differential Equations on Overlapping Grids **FULL TITLE** ASP Conference Series, Vol. **VOLUME**, **YEAR OF PUBLICATION** **NAMES OF EDITORS** Solving Partial Differential Equations on Overlapping Grids William D. Henshaw Centre for Applied Scientific

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

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

Problem description. The FCBI-C element is used in the fluid part of the model.

Problem description. The FCBI-C element is used in the fluid part of the model. Problem description This tutorial illustrates the use of ADINA for analyzing the fluid-structure interaction (FSI) behavior of a flexible splitter behind a 2D cylinder and the surrounding fluid in a channel.

More information

Meta-model based optimization of spot-welded crash box using differential evolution algorithm

Meta-model based optimization of spot-welded crash box using differential evolution algorithm Meta-model based optimization of spot-welded crash box using differential evolution algorithm Abstract Ahmet Serdar Önal 1, Necmettin Kaya 2 1 Beyçelik Gestamp Kalip ve Oto Yan San. Paz. ve Tic. A.Ş, Bursa,

More information

Offshore Platform Fluid Structure Interaction (FSI) Simulation

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

More information

A NURBS-BASED APPROACH FOR SHAPE AND TOPOLOGY OPTIMIZATION OF FLOW DOMAINS

A NURBS-BASED APPROACH FOR SHAPE AND TOPOLOGY OPTIMIZATION OF FLOW DOMAINS 6th European Conference on Computational Mechanics (ECCM 6) 7th European Conference on Computational Fluid Dynamics (ECFD 7) 11 15 June 2018, Glasgow, UK A NURBS-BASED APPROACH FOR SHAPE AND TOPOLOGY OPTIMIZATION

More information

Chapter 5 Modeling and Simulation of Mechanism

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

More information

Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube

Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube Multiphase flow metrology in oil and gas production: Case study of multiphase flow in horizontal tube Deliverable 5.1.2 of Work Package WP5 (Creating Impact) Authors: Stanislav Knotek Czech Metrology Institute

More information

Computer Life (CPL) ISSN: Fluid-structure Coupling Simulation Analysis of Wavy Lip Seals

Computer Life (CPL) ISSN: Fluid-structure Coupling Simulation Analysis of Wavy Lip Seals Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Fluid-structure Coupling Simulation Analysis of Wavy Lip Seals Linghao Song a, Renpu Deng b and Chaonan Huang c College of Mechanical

More information

CFD-1. Introduction: What is CFD? T. J. Craft. Msc CFD-1. CFD: Computational Fluid Dynamics

CFD-1. Introduction: What is CFD? T. J. Craft. Msc CFD-1. CFD: Computational Fluid Dynamics School of Mechanical Aerospace and Civil Engineering CFD-1 T. J. Craft George Begg Building, C41 Msc CFD-1 Reading: J. Ferziger, M. Peric, Computational Methods for Fluid Dynamics H.K. Versteeg, W. Malalasekara,

More information

Modeling External Compressible Flow

Modeling External Compressible Flow Tutorial 3. Modeling External Compressible Flow Introduction The purpose of this tutorial is to compute the turbulent flow past a transonic airfoil at a nonzero angle of attack. You will use the Spalart-Allmaras

More information

Microwell Mixing with Surface Tension

Microwell Mixing with Surface Tension Microwell Mixing with Surface Tension Nick Cox Supervised by Professor Bruce Finlayson University of Washington Department of Chemical Engineering June 6, 2007 Abstract For many applications in the pharmaceutical

More information

Using ANSYS and CFX to Model Aluminum Reduction Cell since1984 and Beyond. Dr. Marc Dupuis

Using ANSYS and CFX to Model Aluminum Reduction Cell since1984 and Beyond. Dr. Marc Dupuis Using ANSYS and CFX to Model Aluminum Reduction Cell since1984 and Beyond Dr. Marc Dupuis 1980-84, 2D potroom ventilation model Physical model 1980-84, 2D potroom ventilation model Experimental results

More information

Characteristic Aspects of SPH Solutions

Characteristic Aspects of SPH Solutions Characteristic Aspects of SPH Solutions for Free Surface Problems: Source and Possible Treatment of High Frequency Numerical Oscillations of Local Loads. A. Colagrossi*, D. Le Touzé & G.Colicchio* *INSEAN

More information

Compressible Flow in a Nozzle

Compressible Flow in a Nozzle SPC 407 Supersonic & Hypersonic Fluid Dynamics Ansys Fluent Tutorial 1 Compressible Flow in a Nozzle Ahmed M Nagib Elmekawy, PhD, P.E. Problem Specification Consider air flowing at high-speed through a

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

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

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

More information

Medical device design using Computational Fluid Dynamics (CFD)

Medical device design using Computational Fluid Dynamics (CFD) Medical device design using Computational Fluid Dynamics (CFD) Session: Summer 2016 IMPORTANT NOTE: This project has 8 deliverables, for each one timely work is expected. 1. General Design Specifications

More information

Finite Volume Methodology for Contact Problems of Linear Elastic Solids

Finite Volume Methodology for Contact Problems of Linear Elastic Solids Finite Volume Methodology for Contact Problems of Linear Elastic Solids H. Jasak Computational Dynamics Ltd. Hythe House 200 Shepherds Bush Road London W6 7NY, England E-mail: h.jasak@cd.co.uk H.G. Weller

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

NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV)

NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) University of West Bohemia» Department of Power System Engineering NUMERICAL INVESTIGATION OF THE FLOW BEHAVIOR INTO THE INLET GUIDE VANE SYSTEM (IGV) Publication was supported by project: Budování excelentního

More information

Using the Eulerian Multiphase Model for Granular Flow

Using the Eulerian Multiphase Model for Granular Flow Tutorial 21. Using the Eulerian Multiphase Model for Granular Flow Introduction Mixing tanks are used to maintain solid particles or droplets of heavy fluids in suspension. Mixing may be required to enhance

More information

Advances in FSI using body-fitted unstructured grids

Advances in FSI using body-fitted unstructured grids Fluid Structure Interaction and Moving Boundary Problems 25 Advances in FSI using body-fitted unstructured grids R. Löhner, B. Hübner & J. R. Cebral School of Computational Sciences, George Mason University,

More information

Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics

Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics Development of an Integrated Computational Simulation Method for Fluid Driven Structure Movement and Acoustics I. Pantle Fachgebiet Strömungsmaschinen Karlsruher Institut für Technologie KIT Motivation

More information

Ryian Hunter MAE 598

Ryian Hunter MAE 598 Setup: The initial geometry was produced using the engineering schematics provided in the project assignment document using the ANSYS DesignModeler application taking advantage of system symmetry. Fig.

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

Experimental and Numerical Analysis of Near Wall Flow at the Intake Valve and its Influence on Large-Scale Fluctuations

Experimental and Numerical Analysis of Near Wall Flow at the Intake Valve and its Influence on Large-Scale Fluctuations Experimental and Numerical Analysis of Near Wall Flow at the Intake Valve and its Influence on Large-Scale Fluctuations Frank Hartmann, Stefan Buhl, Florian Gleiß, Christian Hasse Philipp Barth, Martin

More information

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc.

Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications. Laz Foley, ANSYS Inc. Automotive Fluid-Structure Interaction (FSI) Concepts, Solutions and Applications Laz Foley, ANSYS Inc. Outline FSI Classifications FSI Solutions FSI Modeling Approaches ANSYS Workbench for FSI System

More information

Outline for the New ASME Standard for the Verification and Validation of Computational Fluid Dynamics (CFD) Simulation in Medical Devices

Outline for the New ASME Standard for the Verification and Validation of Computational Fluid Dynamics (CFD) Simulation in Medical Devices Outline for the New ASME Standard for the Verification and Validation of Computational Fluid Dynamics (CFD) Simulation in Medical Devices Marc Horner, Ph.D. ANSYS, Inc. 1 CFD Sub-group Members Marc Horner,

More information

A Comparative CFD Analysis of a Journal Bearing with a Microgroove on the Shaft & Journal

A Comparative CFD Analysis of a Journal Bearing with a Microgroove on the Shaft & Journal Proceedings of International Conference on Innovation & Research in Technology for Sustainable Development (ICIRT 2012), 01-03 November 2012 182 A Comparative CFD Analysis of a Journal Bearing with a Microgroove

More information

A Finite Element Analysis Workflow in Biomechanics. Define the problem and identify FEA as the favorable modeling & simulation strategy

A Finite Element Analysis Workflow in Biomechanics. Define the problem and identify FEA as the favorable modeling & simulation strategy Before you start Understand the Premise of FEA Finite element analysis is a computational modeling & simulation strategy; specifically, a numerical procedure for solving field problems, e.g., stress, by

More information

Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure

Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure In the final year of his engineering degree course a student was introduced to finite element analysis and conducted an assessment

More information

Viscoelastic Registration of Medical Images

Viscoelastic Registration of Medical Images Viscoelastic Registration of Medical Images Zhao Yi Justin Wan Abstract Since the physical behavior of many tissues is shown to be viscoelastic, we propose a novel registration technique for medical images

More information

CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING

CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it

More information

Coupled Analysis of FSI

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

More information

FIDAP Fidap 8.5 Page 1 of 6

FIDAP Fidap 8.5 Page 1 of 6 FIDAP 8.5 Page 1 of 6 FIDAP 8.5 is the CFD solver of choice for a wide variety of laminar and turbulent flows that arise in the polymer processing, thin film coating, biomedical, semiconductor crystal

More information

2008 International ANSYS Conference

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

More information

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

Simulation of Fuel Sloshing Comparative Study

Simulation of Fuel Sloshing Comparative Study 3. LS-DYNA Anwenderforum, Bamberg 2004 Netfreie Verfahren Simulation of Fuel Sloshing Comparative Study Matej Vesenjak 1, Heiner Müllerschön 2, Alexander Hummel 3, Zoran Ren 1 1 University of Maribor,

More information

FEMLAB Exercise 1 for ChE366

FEMLAB Exercise 1 for ChE366 FEMLAB Exercise 1 for ChE366 Problem statement Consider a spherical particle of radius r s moving with constant velocity U in an infinitely long cylinder of radius R that contains a Newtonian fluid. Let

More information

An added mass partitioned algorithm for rigid bodies and incompressible flows

An added mass partitioned algorithm for rigid bodies and incompressible flows An added mass partitioned algorithm for rigid bodies and incompressible flows Jeff Banks Rensselaer Polytechnic Institute Overset Grid Symposium Mukilteo, WA October 19, 216 Collaborators Bill Henshaw,

More information

ANALYSIS OF PIEZOELECTRIC MICRO PUMP

ANALYSIS OF PIEZOELECTRIC MICRO PUMP Int. J. Mech. Eng. & Rob. Res. 2013 S Nagakalyan and B Raghu Kumar, 2013 Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 2, No. 3, July 2013 2013 IJMERR. All Rights Reserved ANALYSIS OF PIEZOELECTRIC

More information

FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS

FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS Proceedings of ICAD26 FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS ICAD-26-43 Enrico Armentani enrico.armentani@unina.it University of Naples P.le V. Tecchio, 8 8125 Naples Italy Francesco

More information

1. Carlos A. Felippa, Introduction to Finite Element Methods,

1. Carlos A. Felippa, Introduction to Finite Element Methods, Chapter Finite Element Methods In this chapter we will consider how one can model the deformation of solid objects under the influence of external (and possibly internal) forces. As we shall see, the coupled

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

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

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

More information

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

Development of Hybrid Fluid Jet / Float Polishing Process

Development of Hybrid Fluid Jet / Float Polishing Process COMSOL Conference - Tokyo 2013 Development of Hybrid Fluid Jet / Float Polishing Process A. Beaucamp, Y. Namba Dept. of Mechanical Engineering, Chubu University, Japan Zeeko LTD, United Kingdom Research

More information

Unstructured Mesh Generation for Implicit Moving Geometries and Level Set Applications

Unstructured Mesh Generation for Implicit Moving Geometries and Level Set Applications Unstructured Mesh Generation for Implicit Moving Geometries and Level Set Applications Per-Olof Persson (persson@mit.edu) Department of Mathematics Massachusetts Institute of Technology http://www.mit.edu/

More information

Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it.

Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it. Thank you! Thank you for downloading one of our ANSYS whitepapers we hope you enjoy it. Have questions? Need more information? Please don t hesitate to contact us! We have plenty more where this came from.

More information

FLOWVISION CFD FREQUENTLY ASKED QUESTIONS

FLOWVISION CFD FREQUENTLY ASKED QUESTIONS FLOWVISION CFD FREQUENTLY ASKED QUESTIONS 1. Installation and Licensing 1.1. Does FlowVision have floating licenses? 1.1.1. Actually all FlowVision licenses have floating capability and no extra fees are

More information

Strömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4

Strömningslära Fluid Dynamics. Computer laboratories using COMSOL v4.4 UMEÅ UNIVERSITY Department of Physics Claude Dion Olexii Iukhymenko May 15, 2015 Strömningslära Fluid Dynamics (5FY144) Computer laboratories using COMSOL v4.4!! Report requirements Computer labs must

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

Non-Newtonian Transitional Flow in an Eccentric Annulus

Non-Newtonian Transitional Flow in an Eccentric Annulus Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent

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

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

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