Cardiovascular Engineering and Technology

, Volume 3, Issue 1, pp 88–100

Experimentally Validated Hemodynamics Simulations of Mechanical Heart Valves in Three Dimensions

Authors

    • Institute of High Performance Computing
  • Yee Han Kuan
    • Division of BioengineeringNational University of Singapore
  • Po-Yu Chen
    • Division of BioengineeringNational University of Singapore
  • Liang Ge
    • Division of Adult Cardiothoracic SurgeryUniversity of California
  • Fotis Sotiropoulos
    • Department of Civil EngineeringUniversity of Minnesota
  • Ajit P. Yoganathan
    • Walter H. Coulter School of Biomedical EngineeringGeorgia Institute of Technology
  • Hwa Liang Leo
    • Division of BioengineeringNational University of Singapore
Article

DOI: 10.1007/s13239-011-0077-z

Cite this article as:
Nguyen, V., Kuan, Y.H., Chen, P. et al. Cardiovasc Eng Tech (2012) 3: 88. doi:10.1007/s13239-011-0077-z

Abstract

Mechanical heart valves (MHV) have been widely deployed as a routine surgical treatment option for patients with heart valve diseases due to its durability and performance. Understanding hemodynamics of MHV plays a key role in performance assessment as well as design. In this work, we propose a numerical method for simulations of full three dimensional MHV with moving valve leaflets in a typical human cardiac cycle. A cell-centered finite volume method is employed to model incompressible flows in MHV. As the flow experiences from laminar to turbulence over every cardiac cycle, the unsteady Reynolds average Navier–Stokes (URANS) equations is solved with \(k{-}\epsilon\) and Spalart–Allmaras turbulence models to resolve large scaled turbulent eddies in high Reynolds number flow regimes. URANS approach chosen for the balance of turbulence resolution and computational cost shows good agreement with more detailed turbulence models as well as experimental data. For capturing the large amplitude movement of the valves, we develop an optimization-based moving mesh technique with objective functions operating on different mesh quality metrics. The method is capable of extensively providing an effective way to maintain and improve the mesh quality due to large movement of domain boundaries. The numerical results for laminar and turbulent flows are validated against experimental data using Particle Image Velocimetry technique. The simulation is able to capture essential features of flows in MHV. The triple jet structure is observed in the simulations together with a switching of central orifice jet flow from horizontal axis to vertical axis downstream of the leaflets and the results are well compared with the experimental data. The moving mesh technique has enabled us to simulate a whole cardiac cycle with pulsatile physiological conditions and prescribed motions of the leaflets. The simulations can essentially reproduce the varying pressure profiles at the left ventricle and aorta. The wall shear stress and vorticity can then be deduced from the simulation results to further access the valve performance. This study also constitutes an important step towards understanding hemodynamics in MHV and contributing to the advancement in study of improved MHV.

Keywords

Prosthetic valvesMechanical heart valvesHemodynamicsSimulationsNavier–Stokes equationsFinite volumePIV

Introduction

Heart valve diseases affect more than 100 million people worldwide19 and since the 1960s, replacement of defective heart valves with prosthetic valves has been a routine surgical treatment option for this condition. Over 300,000 heart valve replacements are performed worldwide yearly.9 Nearly 65% of these replacements opted for MHV (MHV) due to their superior durability and satisfactory bulk flow hemodynamics as opposed to non-mechanical options such as the bioprosthetic heart valves.27 Nevertheless, all MHV are prone to thromboembolic complications thus necessitating lifelong anti-coagulation therapy for improved prognosis.12,26

The most widely implanted mechanical heart valve is the bileaflet mechanical heart valve design. The essential design features of a bileaflet valve consists of two mobile leaflets that are shaped as approximately semicircular disks retained within the valve annular housing by four hinges. The leaflets open and close passively in response to the forces exerted by blood flow through the valve. At opened position, the leaflets will divide the flow orifice into the central and lateral regions, thus giving rise to a characteristics three forward jets flow profile; one central jet sandwiched by two lateral jets. The velocity gradient across these three forward jets have been a constant attention of heart valve engineers these past decades. This is because research has shown that the velocity gradient can lead to energy losses and high turbulent shear stresses downstream of the valve, and these hemodynamic parameters have been demonstrated to be good performance indicators for the success of a bileaflet mechanical heart valve (BMHV).

In recent years, Computational Fluid Dynamics (CFD) has emerged as a potentially promising alternative to investigate the hemodynamics within the heart valves. Since the pioneering work of two dimensional simulations by Peskin20,21 the CFD study of flows in BHMV has achieved a considerable progress towards understanding of hemodynamics and the associated issues. King et al.14 investigated the effect of opening angles on the time-dependent flow through a BMHV using a quarter valve symmetric model. The assumption of a symmetric flow showed that secondary flow features such as mixing on the edges of the jets and spiraling vortices shed shows differences between experimental and CFD simulations demonstrating that a full 3D model is required for a better accuracy. Another numerical study was performed by Ge et al.11 where full 3D flows over BMHV were investigated at different Reynolds numbers. The study simulates flows through aortic position at Re = 750 corresponding to the flow at unsteady laminar regime and Re = 6000 corresponding to the flow near peak-systole and fully turbulent. For turbulent flows, the unsteady Reynolds Averaged Navier–Stokes (URANS) and detached eddy simulation (DES) models were employed. However, pulsatile effects and leaflet motions were not considered.

There are several challenges in CFD simulations such the complex BMHV geometry, leaflet motion and flow unsteadiness. Studies have been done to investigate the wall shear stresses in the clearance region with the leaflets in closed position.16,22 Nevertheless, the effect of leaflet motion was neglected. Bluestein et al.2 did a simulation of the motion of leaflets for the last few degrees of motion during valve closure. There were more simulations conducted by coupling the fluid flow with the leaflet motion from fully open to closed position. Aluri and Chandran1 used a prescribed valve motion in a simplified flow domain. It was reported that the simulation with leaflet motion was simplified by restricting it to a 2D model. Lai et al.15 also used a 2D model with a prescribed motion of the leaflets obtained from experimental data.

In this study, we developed a computational method to incorporate the leaflet motion by simulating the flow dynamics in a full 3D model of a BMHV. The leaflet motion was prescribed from a fully open position to full closure position, corresponding to the velocity wave profile of a typical cardiac cycle. A validation study was conducted for a full 3D model with leaflets fixed at a fully open position in a laminar flow using our numerical model. As the current methodology is different from earlier work,11 there is a need to report the validation of our simulation and we used the laminar flow model. The turbulence modeling was also conducted to investigate the flow for fixed valve leaflets at fully open position. This current investigation forms part of a continuing study of heart valve engineering. The broader objective of this study is to provide an improved quantitative and qualitative understanding of the functionality and potential thrombogenicity of BMHVs beyond that available from previous studies. This forms part of the effort to develop a computational framework which can support decision-making for clinicians. The results of this work should also provide new insight into the roles the subtle design features have on the potential for blood damage.

The paper is organized as follows. First we outline the experimental procedures used to collect measurements for CFD validation. Next, we present the governing equations and describe the computational methods and modeling used in this study. Then we present and compare the results for laminar flow simulations and experiments. Next we focus on turbulence simulations using Spalart–Allmaras (SA) and \(k{-}\epsilon\) models, followed by a full cardiac cycle flow. Finally, we conclude our findings of this work and discuss future research directions.

Methodology

Experimental Setup

Flow experiments were conducted with setups and operating conditions similar to the simulation runs. The mechanical heart valve used for this study was the 29 mm ATS Medical Open Pivot Heart Valve. The valve was placed in a clear acrylic test section of length of at least 5D and 10D upstream and downstream respectively (D is the diameter of the pipe inlet), to facilitate visualization and measurement of the flow. The flow entering the test section had a fully developed profile matching that of the numerical simulations, by passing the flow through a straight circular pipe of length 1800 mm in the upstream of the valve as shown in Fig. 1.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig1_HTML.gif
Figure 1

Schematic diagram of steady flow loop setup

The fluid used in the experiment was composed of 59% saturated aqueous sodium iodide, 40% glycerin and 1% deionized water by volume, which was transparent to allow the measurement of flow velocities using Particle Image Velocimetry (PIV) technique. With such ratio, a kinematic viscosity of 3.81 cSt was achieved, which is similar to blood at high shear (3.5–4.0 cSt). We tried to match the refractive index of the fluid, 1.44, to the acrylic valve holder, 1.49, in order to reduce optical distortion. The kinematic viscosity could be adjusted by addition of glycerin for an increase or addition of deionized water for a decrease in viscosity. The refractive index on the other hand, could be increased with the addition of saturated aqueous sodium iodide.

The flow was seeded with 9−13 μm glass spheres and illuminated by Minilase-III PIV system (New Wave Research, USA). The system was a 15 Hz Q-switched, double cavity pulsed Nd:YAG laser. The images were recorded with a charge coupled device (CCD) camera (FlowSense, Dantec Dynamics, Denmark) and the velocity flow fields were averaged from 200 image pairs which were analyzed using the DynamicStudio software (Dantec Dynamics, Denmark). The investigation area was a 99 × 74 vector field and the velocity range observed in the experiment was 0–0.3 m/s. In order to reduce the near wall bias, the boundary of the interrogation areas were matched with that of our model. The mean flow velocity measurements were obtained under steady inflow conditions for flow rates with Reynolds numbers Re = 350, Re = 750 and Re = 1000.

Flow was measured using the PIV system at the upstream of the mechanical valve to find out the incoming flow profile. The experiment flow profiles were similar to the fully developed flow in the simulations for all the simulated Reynolds numbers in terms of the shape as well as the magnitude. An example of the resultant time-averaged flow profile obtained from the experiment can be seen in Fig. 2 for Reynolds number 350.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig2_HTML.gif
Figure 2

Fully developed flow profile for Re = 350 at the inlet

Finite Volume Method for Simulations of BMHV Hemodynamics

In the CFD simulations, we investigated flows over the BMHV at different Reynolds numbers ranging from 350 to 5000 corresponding to the parabolic laminar flow seen at late systole and during diastole as well as peak systolic velocity of the cardiac cycle. The flows were first studied at the maximum opening of the valves at 85o and comparisons with experimental data were made to validate the simulations. Experimental validations under steady conditions were conducted for Reynolds numbers ranging from 350 to 1000. Nevertheless, Dumont et al.7 found that the ATS valve opened to less than maximal opening angle. To understand flow regimes in a cardiac cycle, we also performed CFD simulations to investigate flows over BMHV at aortic area under the pulsatile conditions of velocity and pressure deduced from a typical human cardiac cycle.

In this study flows were modeled as the incompressible viscous fluid and governed by incompressible Navier–Stokes equations. The computational domain was subdivided into an unstructured tetrahedral mesh of approximately one million elements. The governing equations were then discretized in space using the finite volume method where a finite set of discrete equations were constructed on unstructured hybrid grids to approximate the NS equations. The construction was performed by a cell-centered FV approach where the FV discretization was based on the integral form of the governing equation over a polyhedral control volume. To handle movement of heart valves, the arbitrary Lagrangian Eulerian (ALE) formulation was used to discretize the system. We used second order Crank-Nicholson implicit time discretization with adjustable time step dependent on the Courant–Friedrichs–Lewy (CFL) number. A dynamic moving mesh approach was adopted to deform and regenerate the mesh following moving boundaries. The resulting numerical scheme was able to solve for flows over moving heart valves.

Governing Equations

Considering incompressible viscous flows over a domain \(\Upomega, \) the governing incompressible Navier–Stokes equations that express the conservation of mass and momentum are written as follows
$$ \nabla \cdot {\user2{u}}=0 \quad \hbox{in} \,\, \Upomega, $$
(1)
$$ \frac{\partial \rho {\user2{u}}}{\partial t} + {\user2{u}} \cdot \nabla \rho {\user2{u}} = -\nabla p + \nabla \cdot (\mu \nabla {\user2{u}}) +{\user2{f}} \quad \hbox{in} \,\, \Upomega, $$
(2)
$$ {\user2{u}}(t=0)={\user2{u}}_0 \quad \hbox{in} \,\, \Upomega. $$
(3)
In these equations, velocity vector is denoted by \({\user2{u}}, \rho\) is the density, p is the pressure and μ is the dynamic viscosity of the fluid. The blood is considered as Newtonian fluid of density ρ = 1025 kgm−3 and kinematic viscosity of \(\nu=3.81 \times 10^{-5} \hbox{m}^2\hbox{s}^{-1}.\,\, {\user2{f}}\) is the body force and the total fluid stress tensor including pressure and viscous force can be expressed as
$$ \sigma = {\user2{\tau}}-p{\user2{I}}, \quad {\user2{\tau}} = \mu(\nabla {\user2{u}} + \nabla {\user2{u}}^T), $$
(4)
where τ is the viscous stress. The flow is characterized by Reynolds number, \({\text{Re}} = \frac{U_{\text{ref}} L_{\text{ref}}}{\nu}\) where Uref and Lref are the reference velocity and length scale. The equations are closed with boundary conditions imposed on the boundary of the domain \(\Upgamma = \delta \Upomega\) as
$$ {\user2{u}} = \bar{{\user2{u}}} \quad \hbox{in } \Upgamma_{\text{D}}, $$
(5)
$$ {\user2{\sigma}}\cdot {\user2{n}} = \bar{{\user2{t}}} \quad \hbox{in } \Upgamma_{\text{N}}, $$
(6)
where \(\Upgamma=\Upgamma_{\text{N}} \cup \Upgamma_{\text{D}}. \, \Upgamma_N\) denotes a boundary where Neumann conditions are applied in the form of prescribed tractions (\(\bar{{\user2{t}}}\)) and \(\Upgamma_{\text{D}}\) corresponds to a Dirichlet boundary on which the velocity is imposed.

Finite Volume Discretization

Finite volume method is based on the integral form of the governing equations over the arbitrary moving domain \(\Upomega\) bounded by closed surface \(\Upgamma\) as follows
$$ \oint\limits_{\Upgamma}{{\user2{n}}\cdot{\user2{u}}} {\text{d}}S=0 $$
(7)
$$ \frac{\partial}{\partial t} \int\limits_{\Upomega}{\rho {\user2{u}}{\text{d}}V}+ \oint\limits_{\Upgamma}{{\user2{n}}\cdot \rho ({\user2{u}}-{\user2{u}}_S){\user2{u}}{\text{d}}S} =\oint\limits_{\Upgamma}{{\user2{n}}\cdot(\mu \nabla{\user2{u}}) {\text{d}}S}- \int\limits_{\Upomega}{\nabla p {\text{d}}V} + \int\limits_{\Upomega}{{\user2{f}} {\text{d}}V}. $$
(8)
In the above expression, \({\user2{n}}\) is the outward normal vector to the bounding surface \(\Upgamma\) and \({\user2{u}}_S\) is the the moving velocity of the surface. As the boundary moves, the geometric conservation law (GCL)8 defines the conservation of space with respect to the change in volume and boundary velocity
$$ \frac{\partial}{\partial t} \int\limits_{\Upomega}{{\text{d}}V} - \oint\limits_{\Upgamma}{{\user2{n}}\cdot{\user2{u}}_{S} {\text{d}}S} = 0. $$
(9)
The computational domain is then subdivided into a set of non-overlapping polyhedral elements or control volumes. Figure 3 shows a sample control volume at point P and its notations of faces and neighbouring cells. The FV discretization transforms surface and volume integrals into a sum of face and control volume integrals and approximates them to second order accuracy. The FV discretization of momentum Eq. (8) for every moving control volume VP is written as
$$ \frac{\partial}{\partial t} {\rho {\user2{u}}_{P} V_{P}} + \sum_{f}{(F-{F}_{S}) {\user2{u}}_{f}} = \sum_{f}{\mu_f{\user2{n}}_{f} \cdot (\nabla {\user2{u}})_{f} S_{f}} + (\nabla p)_{P} V_{P} $$
(10)
where the subscript P denotes volume values, f represents face values, VP is the cell volume and Sf is the face area. In this expression F is the face fluid flux \(F=\rho_f({\user2{n}}_f \cdot {\user2{u}}_f) S_f\) and FS is the face moving volume flux satisfied the GCL condition (9). In the discrete form, Eq. (9) is expressed as
$$ \frac{V_{P}^{(t+\Updelta t)}-V_{P}^{t}}{\Updelta t}-\sum_{f}{F_{S}}=0. $$
(11)
Thus the moving volume flux FS is consistently computed as the volume swept by the face f in motion during the current time step rather than from the mesh velocity \({\user2{u}}_S. \) The spatial and temporal discretizations are implemented and well tested in the open source package OpenFOAM.28
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig3_HTML.gif
Figure 3

Illustration of polyhedral control volume VP around point P located at the centroid of the cell. The control volume is bounded by convex polygons or faces Si with the face unit normal vector \({\user2{n}}_i. \) Each face Si is only shared between two adjacent cells P and Q

Boundary Conditions

Generally the Dirichlet and Neumann boundary conditions can be effectively implemented in the context of the current finite volume discretization. For a Dirichlet type of boundary condition where a fixed value of dependent variables ϕb is prescribed at the boundary, the value of the variable can be directly set as the boundary value ϕf = ϕb while the gradient of the variable can be reconstructed as
$$ {\user2{S}}_f \cdot (\nabla \phi)_f = |S_f|\frac{\phi_b - \phi_P}{|d|}. $$
(12)
In this expression, \({\user2{d}}\) is the distance vector from a point on the surface to the control point P. As for Neumann type of boundary conditions, gradient of dependent variables in normal direction to the boundaries are specified
$$ g_b = \left(\frac{{\user2{S}}}{|{\user2{S}}|} \cdot \phi \right)_{f}. $$
(13)
Thus the gradient of the variables at the face can be recovered directly as \({\user2{S}}_f \cdot (\nabla \phi)_f = |S|_f g_b, \) while the value of variable can be interpolated as
$$ \phi_f = \phi_P + |{\user2{d}}|g_b. $$
(14)
In the current work, flows over the MHV were initialized with free stream initial conditions where velocity and pressure were given. At the inlet and outlet, velocity and pressure were prescribed while no slip boundary condition was imposed at the channel walls as well as at the valves wall. In particular, velocity is specified at the inlet with either a parabolic profile for laminar flows or a velocity wave form in pulsatile flows. For consistency, the boundary condition for pressure was zero gradient. The pressure field at the outlet was given and a zero gradient boundary condition on velocity was specified. As for walls, the velocity of the fluid was set equal to that of the wall itself, i.e. a fixed value condition can be specified. The pressure was specified zero gradient to ensure zero flux through the walls.

Full Cardiac Cycle Modeling

As one of the main objectives in this current study, a full 3D flow was simulated over a typical human cardiac cycle in which the ATS valve placed at the aortic position was operated under a prescribed motion as well as given inlet and outlet wave forms. Typically, a cardiac cycle was divided into a systolic and diastolic time interval10 where the heart’s atria and ventricles were working synchronously to pump the blood through the circulatory system. The prescribed periodic condition started at fully open position of the valve where ejecting velocity kept increasing from zero to a peak value of 1.35 m/s. The duration of systolic was 300 ms. During this period, aortic pressure also increased. The valve then moved from open to closed position in about 40 ms while velocity dramatically dropped to zero until full closure of the valve leaflets. The valve remained at fully closed during diastolic for about 480 ms. Backflow occurred at the inlet when it opened again for about 40 ms due to a further decrease in aortic pressure. Figure 4 shows the prescribed velocity and pressure for a full cardiac cycle. The whole cycle of about 860 ms was derived from a heart beat condition of a healthy person, which corresponds to about 70 bpm. The simulation was driven by the inlet velocity boundary condition at the ventricle while aortic pressure was maintained at the outlet. The leaflets motion was set at a constant angular velocity corresponding to the valve moving from fully open to closed position and vice versa.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig4_HTML.gif
Figure 4

Prescribed inlet velocity and outlet pressure for a sample cardiac cycle in the current study

Turbulence Modeling

When the flow reaches a certain Reynolds number the flow goes from being laminar to turbulent. Turbulence is a three dimensional and highly transient continuum phenomenon where the fluid’s irregular motions are described in a continuously wide range of scale, from the smallest turbulence eddies (or eddies of turbulence) defined by Kolmogorov scales to the largest eddies characterized by the particular flow and these eddies carry most of the turbulent kinetic energy. The Reynolds number for most of pulsatile cardiovascular flows ranges from 0 to around 104 based on vessels geometric configuration. For MHV, as the velocity is pulsatile, the flows experience from laminar to turbulent regime over every cardiac cycle.

Depending on the level of resolution of turbulence scales, various methodologies for modeling turbulence can be employed. Among those, large eddy simulations (LES) and Reynolds averaged Navier–Stokes (RANS) approaches have gained much attention and exploration over the last few decades. In the LES approach, large scales are resolved on a given computational mesh using the same spatial discretization method for flow variables while the small scales are modeled. The LES approach is able to provide a more detailed description of turbulent flows. However, the requirements on mesh resolution and time step size put very high demands on the computer resources; thus rendered as a more computational intensive method.

An alternative to overcome this problem is to solve the RANS appended with a turbulence model. In RANS turbulence modeling, all of the unsteadiness in the flow is averaged out and regarded as part of the turbulence. The instantaneous flow field is divided into a time-averaged part and a fluctuating part expressed in terms of mean quantities. Although known as a less detailed turbulence simulation method, RANS solutions show reasonable resolutions to turbulence flows, especially for relatively large Reynolds number. In addition, the method is the least expensive of all the turbulence modeling methods where the total arithmetic is independent of Reynolds number while it is in the order of Re2 and Re3 for LES and direct numerical simulations, respectively.

Since we are mainly interested in the large-scale features of the flow dynamics in this study, RANS provide a good balance between the results and the computational cost. In RANS turbulence modeling, all of the unsteadiness in the flow is averaged out and regarded as part of the turbulence. The instantaneous flow field is divided into a time-averaged part and a fluctuating part expressed in terms of mean quantities. Although known as a less detailed turbulence simulation method, RANS solutions show reasonable resolutions to turbulence flows, especially for relatively large Reynolds number. In addition, the method is the least expensive of all the turbulence modeling methods where the total arithmetic is independent of Reynolds number while it is in the order of Re2 and Re3 for LES and direct numerical simulations, respectively. We are interested in developing a code which can help the decision-making process for clinicians in the most effective way so we decided to employ the RANS approach appended with a turbulence model.

In this work, we solve RANS equations with two most popular turbulence models, namely SA and \(k{-}\epsilon. \) In both models, the transport equation for turbulence kinetic energy is written as
$$ \frac{\partial k}{\partial t} + \overline{u}_j \frac{\partial k}{\partial x_j} = \tau_{ij}\frac{\partial \overline{u}_i}{\partial x_j} - \epsilon + \frac{\partial}{\partial x_j} \left[ (\nu + \nu_t/\sigma_k) \frac{\partial k}{\partial x_j}\right]. $$
(15)
The Reynolds Averaged for velocity can be written as
$$ {\user2{u}}({\user2{x}},t) = \overline{{\user2{u}}}({\user2{x}},t) + {\user2{u}}'({\user2{x}},t). $$
(16)
where \({\user2{u}}'({\user2{x}},t)\) is the fluctuation about the average value \(\overline{{\user2{u}}}({\user2{x}},t). \) In these expressions, \(\epsilon=\nu \overline{{\user2{u}}'{\user2{u}}' : \nabla {\user2{u}}'}\) is the dissipation of the kinetic energy, σk is the closure coefficient and νt is the turbulent or eddy viscosity which is determined by the appended turbulence model.
Spalart-Allmaras (SA) Model
In the SA model,23 kinematic eddy viscosity is modeled as
$$ \nu_t = \tilde{\nu} f_{v1}, \quad f_{v1}=\frac{\chi^3}{\chi^3+c^3_{v1}}, \quad \chi = \frac{\tilde{\nu}}{\nu}, $$
(17)
where \(\tilde{\nu}\) is the modified kinematic viscosity. The transport equation for eddy viscosity is deduced from (15) as
$$ \frac{\partial \tilde{\nu}}{\partial t} + \overline{u}_j \frac{\partial \tilde{\nu}}{\partial x_j} = c_{b1}\tilde{S}\tilde{\nu} -c_{w1} f_{w} \left(\frac{\tilde{\nu}}{d}\right)^2 + \frac{1}{\sigma_k} \frac{\partial}{\partial x_j} \left[ (\nu + \tilde{\nu})\frac{\partial \tilde{\nu}}{\partial x_j}\right] + \frac{c_{b2}}{\sigma_k} \frac{\partial \tilde{\nu}}{\partial x_j} \frac{\partial \tilde{\nu}}{\partial x_j}, $$
(18)
where d is the distance from the closest surface. The standard SA model includes eight closure coefficients
$$ c_{b1} = 0.1335,\quad c_{b2}=0.622,\quad c_{v1}=7.1,\quad \sigma_k = \frac{2}{3} $$
(19)
$$ c_{w1}=\frac{c_{b1}}{\kappa^2}+\frac{(1+c_{b2})}{\sigma_k},\quad c_{w2}=0.3,\quad c_{w3}=2,\quad \kappa = 0.41 $$
(20)
There are many different forms of SA models and their details can be found in Spalart23
k–ε Model
In the \(k{-}\epsilon\) model, the kinematic eddy viscosity is expressed as a function of the turbulent kinetic energy k and its dissipation rate \(\epsilon\) as
$$ \nu_t = C_{\mu}\frac{k^2}{\epsilon}. $$
(21)
The transport equation for the dissipation rate is written as follows
$$ \frac{\partial \epsilon}{\partial t} + \overline{u}_j\frac{\partial \epsilon}{\partial x_j} = C_{\epsilon 1}\frac{\epsilon}{k}\tau_{ij}\frac{\partial \overline{u}_i}{\partial x_j} - C_{\epsilon 2}\frac{\epsilon^2}{k} + \frac{\partial}{\partial x_j} \left[(\nu + \nu_t / \sigma_{\epsilon}) \frac{\partial \epsilon}{\partial x_j}\right]. $$
(22)
The closure coefficients are:
$$ c_{\epsilon 1} =1.44,\quad C_{\epsilon 2} =1.92,\quad C_{\mu} =0.09, \quad \sigma_k =1.0,\quad \sigma_{\epsilon} =1.3 $$
(23)
There are several other two-equation models that try to describe the turbulence including the RNG \(k{-}\epsilon\) model29 and the nonlinear \(k{-}\epsilon\) Shih model.24 Many of them are based on the \(k{-}\epsilon\) model described above; however, they are more complicated and contain more parameters than the standard \(k{-}\epsilon\) model. All of these models including the above one equation Spalart Allmaras models are implemented in the OpenFOAM package.

Moving Mesh Technique

In the ALE formulation, the moving mesh velocity \({\user2{u}}_S\) can be arbitrarily found such that the moving velocity at the interface must be equal to the boundary velocity \({\user2{u}}_{\Upgamma}, \) either prescribed for fixed boundaries or obtained from the structure response in applications of fluid-structure interaction. Due to the movement of the boundaries, the computational mesh is deformed and possibly fails to preserve its quality. A moving mesh solver is necessary to deform the mesh and move the internal points in order to maintain the quality of the mesh and avoid solution degeneration due to mesh validity. In the context of ALE framework, one has to either regularize the grid moving velocity or decide to do the remeshing after certain steps, which often leads to an increased in computational cost and loss of accuracy and conservation. Deriving a robust and efficient scheme of constructing mesh velocity could help in reducing the effort of remeshing. This has motivated many different approaches for computing the grid velocity, including the velocity smoothing technique in which the mesh velocity is directly computed from the velocity of the moving boundaries in order to minimize the grid distortion, such as Laplacian smoothing with variable diffusivity approaches.17,18 The Laplacian smoothing is able to distribute nodes according to a certain distribution function. However, it is not directly related to a measure of element quality and may cause badly-shaped elements during the process, especially for 3D unstructured grids. In parallel development, a mesh optimization-based smoothing approach,3 adopted in the work, is more attractive in maintaining the quality of the mesh for moving boundary problems. Casting the mesh smoothing as an optimization problem, the method optimizes the mesh quality based on a particular quality metric and optimization criteria to ensure the quality of mesh. Given a distorted mesh \(\mathcal{M}(v_i,e_j)\) of n vertices and k elements, the objective of the method is to distribute the mesh points such that the quality of the mesh is maximized. Mathematically, the mesh optimization problem can be formulated as follows
$$ {\user2{x}} = \arg \max {\mathcal{F}} = f(q_i({\user2{x}})), \quad \forall {\user2{x}},i \in {\mathcal{M}}, $$
(24)
where \(q_i({\user2{x}})\) is the element or vertex based quality metric of mesh entities and \(f(q_i({\user2{x}}))\) is the objective function. There are several objective functions used in Brewer et al.3 including the standard \(\mathcal{l}_P\) (where P is a positive integer) and the \(\mathcal{l}_{\infty}\) function. The objective functions operating on different quality metrics can be combined together to provide maximum flexibility in controlling the mesh quality. When the mesh has been modified, conjugate gradient or feasible Newton optimization algorithms can be used to look for optimal positions. The method is proven to be capable of extensively providing an effective way to maintain and improve the mesh quality due to the movement of domain boundaries. In situations of large deformations, vertices may be undesirably be too much deformed; and upon exceeding the smoothing capability, mesh topology needs to be modified. In order to maintain the mesh quality, topology modification operations including edge swapping, bisection and collapse as shown in Dai and Schmidt5 can be employed. Figure 5 shows application of the approach for a simple problem of two cubes rotating with prescribed velocities.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig5_HTML.gif
Figure 5

Moving mesh solver for motion of 2 cubes in a channel. (a) Initial mesh and (b) the deformed mesh conforming to the motion of the cubes

Results and Discussion

We first validated the proposed numerical scheme against experiment for flows over a fixed valve opening angle at different flow velocities. Numerical simulations for flows at Reynolds numbers in the laminar regimes were carried out for Re = 350, Re = 750 and Re = 1000. In all three cases, we used direct numerical simulation with similar valve and sinus geometries as those in the experiment setup of an ATS valve. The valve was assumed to be fully opened at the angle of 85° between the leaflet and the XY plane. Figure 6 shows the Cartesian coordinate system used which is defined as follows: The X-axis is perpendicular to the leaflets when the valve is fully opened, the Y-axis is parallel to the long axis of the leaflets and the Z-axis is along the flow streamwise direction.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig6_HTML.gif
Figure 6

Plan view of streamwise velocity contours (Re  =  1000) at 3 cross sectional planes, Z = 1D, 2D and 4D

Steady Flows over BMHV

3D Laminar Flows over BMHV

The origin of X and Y axes is at the center of the flow channel with the Z = 0 plane located at the trailing edge of the leaflets with the corresponding velocity components u, v & w respectively. Comparisons for the streamwise velocity profiles (physical velocity) were made at three different locations as follow: Z = 1D, 2D and 4D, as shown in Fig. 6.

In Fig. 7, the predictive capabilities of our numerical model were demonstrated by comparing the time-averaged, streamwise velocity profiles for laminar flow at Re = 350 at the three locations downstream of flow. At position 1D, the triple jet structure of the flow can be seen clearly, just as predicted by the simulation. However, the center jet measured in the experimental result showed lower values of velocity at 0.0855 m/s compared to 0.0893 m/s obtained from the simulation. On the other hand, two lateral jet profiles were evidently shown and accurately predicted from both numerical simulation and experiment.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig7_HTML.gif
Figure 7

Velocity profile comparisons between experimental (o) and numerical simulation (–) for Re = 350 at position z = 1D, 2D and 4D

At position 2D, the velocity profile was near the transition phase from a triple jet structure merging into two lateral jets downstream, as can be seen with a flatter center jet velocity profile. The simulation was able to provide an accurate prediction as compared to the experimental results in terms of magnitude and velocity profile. Further downstream at position 4D, two flatter lateral jets were visibly taking shape. At this location, the simulation results at the center profile had a nearly identical velocity magnitude to the experimental results. The two side profiles in the experiment were within 10% of the simulation results. We have shown that the numerical simulations are able to capture essential features as observed in the experiments with good accuracy in terms of the magnitude and general velocity profile. Some of the features that can be seen were the complex transverse velocity distribution across the Y-axis and the fluid velocity of the flow profiles. The well-known triple jet structure of the flow in the wake of the leaflets can be seen clearly at position 1D before it merged into two lateral jets further downstream at position 4D.

In Fig. 8, similar comparison can be seen for Re = 750 and Re = 1000 at position 1D. The flow profile and velocity magnitude obtained in the simulation showed good agreement with the experimental results. A significant feature captured by the simulation which was also verified experimentally was the formation of vortices near the edge of the wall, as shown in Fig. 8. The magnitude of the vortices obtained from the simulation was almost identical to the experimental results. The triple jet structure was also visible at position 1D for Re = 750 and Re = 1000. However, there were asymmetries in the experiment results obtained where the velocity profile was slightly shifted to the right-hand side (higher X values). The likely reason is due to the breakdown of the steady flow assumptions in the flow domain. It could also be due the valve not being at fully open position at the time of experiment. The experiments and the simulations in terms of the velocity profiles and velocity magnitudes were quite instructive. The simulations were able to capture the essential features of the mean flow in the experiment, notably the vortices near the walls of the sinus chamber.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig8_HTML.gif
Figure 8

Velocity profile comparisons between experimental (o) and numerical simulation (–) for Re  =  750 and Re = 1000 at position z = 1D

As mentioned earlier, the triple jet structure which resulted from the blockage of the flow by the two valve leaflets and the vortex formation can be observed in the simulations at both Reynolds numbers, which was also reported by Ge et al.11

3D Turbulent Flows

We considered a CFD simulation of flow at near peak systolic condition in this study. As the flow approaching this condition, Reynolds number was estimated at about Re = 5000–6000 in which full turbulent regimes were expected to be observed in the flows. In the current study, the URANS approach was employed with \(k{-}\epsilon\) and SA models to simulate turbulent flows. Figure 9 shows time-averaged velocity contour of flow at Reynolds number Re = 5000 using SA turbulence model. The current model was able to capture flow features at high Reynolds number in which the three jet structure is present and the rotation of flow axis at downstream is observed through velocity vector profile at 4 xy planes at z = 0D, 1D, 2D and 4D downstream.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig9_HTML.gif
Figure 9

Flow at Re = 5000 using Spalart–Allmaras turbulence model plan view and 4 cut-planes of Z = 0D, 1D, 2D and 4D

The flow solutions of SA turbulence model were then compared with \(k{-}\epsilon\) model as depicted in Figs. 10 and 11. In Fig. 10 comparing velocity profiles at different cut-planes, it can be seen that the time-averaged velocity was slightly different between the two models as the \(k{-}\epsilon\) results show more symmetric profiles although the difference in velocity magnitude between the two turbulence models was minimal. This can be observed more clearly in Fig. 11 where the two turbulence models showed similar vorticity contours. As these models can only predict the time-averaged quantities, it required more detailed turbulence models such as LES or DES to be able to probe more turbulence statistics. In particular for flows over hinge areas, URANS approach will not surface to capture small scale turbulent eddies as shown in Ge et al.11
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig10_HTML.gif
Figure 10

Comparison of velocity profiles at Re = 5000 using different Reynolds Averaged turbulence models

https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig11_HTML.gif
Figure 11

Comparison of vorticity profiles at Re = 5000 using different Reynolds Averaged turbulence models (a) Spalart–Allmaras & (b) \(k{-}\epsilon\)

Pulsatile Flows over BMHV

Next the proposed method was applied for simulations of pulsatile flows over BMHV with prescribed motions in a typical human cardiac cycle. The motion of the leaflets as well as boundary conditions is described in the earlier section “Full Cardiac Cycle Modeling”. In order to investigate the errors of the initial configuration over multiple cardiac cycles, we simulated the BMHV over two cardiac cycles. The results from first and second cycle were compared and there were no significant differences. As such, results presented for the second cycle single cardiac cycle simulation is sufficient to represent the dynamic operation of BMHV.

Figure 12 shows the variation of pressure and velocity at the inlet and outlet during a complete cardiac cycle. It is noted that the inlet pressure curve showed some variation from the anatomical ventricle pressure curve. One of the possible reasons for such observation was the initial position of the valve leaflets at fully open position. As such, it is physically impossible for the left ventricle pressure to be below the aortic valve at the beginning of the systole.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig12_HTML.gif
Figure 12

(a) Pressure variation with time at inlet and outlet. (b) Velocity variation with time at inlet and outlet

During diastole phase, typical pressure waveform would have ventricular pressure approached close to zero and increased slowly due to mitral filling. Since atrium was not involved in this study, a steady pressure close to zero was expected. During diastole, there was no flow from left ventricle to aorta while the aortic valve was fully closed. However in our study, the BMHV was not fully closed, with a small gap which was necessary for the simulation to converge.

In our study, using the prescribed inlet velocity boundary condition, the peak systole was set at time 115 ms at the second cycle with a maximum inlet velocity magnitude of 1.35 m/s. Figure 13 shows the velocity variation along the radial distance at 7 mm downstream of the valve ring. The graphs showed reasonable agreement with simulation results investigated earlier using FIDAP.13 The study showed that the central jet was slightly higher than the lateral jet with the rest of features matched. However, the achieved velocity distribution along X-axis in our study had a triple jet structure with central jet having roughly equal magnitude with the lateral jet. The lateral jets were not as sharp as the central jet but comparatively flattened, and negative velocity was seen near left and right boundaries which arises from recirculation in the aortic sinus. The difference could be due to symmetric model used, where only a quarter of the BHMV was simulated in King et al.’s model.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig13_HTML.gif
Figure 13

Graph of velocity at peak systole against radial distance 7 mm downstream of the valve ring (a) velocity variation along X-axis (b) velocity variation along Y-axis

Our simplified model of aortic chamber consisted of a single axis-symmetric sinus instead of the anatomical three aortic sinuses. In our results, there is a laminar flow profile in the sinus region of the acceleration phase. Small vortex formation began in the aortic sinus near the leaflet ended at roughly a quarter through acceleration phase. The magnitude of vortex continued to increase in the sinus region and peaked at the start of the decelerating phase. Despite the decrease in the magnitude of vorticity, the size of the vortex continued to increase until the end of the deceleration phase, when the flow eventually broke into numerous small vortices. Such vortex formation pattern agreed with the numerical simulation and experiment performed by Dasi et al.6

Wall shear stress is another important phenomenon in BMHV simulations. Research has shown the association of wall shear stress with platelet activation, hemolysis and thrombus initiation on top of material properties and contact activation.4,13 As the valve leaflets open, the blood is being forced through the valve leaflets, resulting in high velocity jets. These velocity jets will in turn cause high velocity gradients and induce high shear stress. The shear stress may then cause hemolysis or platelet activation. Figure 14 show wall shear stress distribution on the valve leaflet during peak systole. It was seen from the contour plot that the shear stress was highest at valve leaflet edge especially at the edge close to the inlet. This agreed with CFD simulation by Dumont.7 It was also observed that the wall shear stress was higher on the side of the lateral orifice than the central orifice, which could be due to the tilting direction of the valve leaflet when the valve was fully opened. When it was fully opened, the leaflet surface at the lateral side would be exposed more to the fluid flow which caused elevated wall shear stress at the lateral surface.
https://static-content.springer.com/image/art%3A10.1007%2Fs13239-011-0077-z/MediaObjects/13239_2011_77_Fig14_HTML.gif
Figure 14

Wall shear stress distributions on valve leaflet at peak systole

Limitations

We simplified the BMHV model used in the simulation by neglecting the hinge mechanism of the valve leaflets. The lack of hinges may play a role in the upstream region during regurgitation. In reality, the hinge may vary from one side to another due to manufacturing tolerances. As shown by Simon et al.,25 the design of the hinge might play a role in the thromboembolic complications of the valve due to the unsteadiness of the hinge flow fields. The presence of hinge geometry should be accessed for a more accurate simulation. In such case, a more detailed turbulence model, for examples DES, LES as suggested in Ge et al.11 will be necessary to capture small scaled features of the flows.

For pulsatile flows, the simulation was started with the leaflets in the fully open position even though in reality, the valve moves from the closed position to the fully open position during diastole as the ventricular chamber is filled. We decided to simulate in such a way because of the problem faced in mesh regeneration at the start of the simulation if the valve moves from the closed to fully open position. A very high velocity jet is observed in the small clearance region between the leaflets. We did not encounter such problem when the valve moves from fully open to closed position. However, such problems were avoided when we simulated from fully open to closed position. Nevertheless, it is important to study the solver to include the motion of the leaflet according to the actual cardiac cycle for a more realistic simulation.

Conclusion

The simulations for both Re = 350, Re = 750 and Re = 1000 were validated through comparisons with experimental data. In both simulations, we were able to capture most experimental trends and magnitude with reasonable accuracy. An important feature that was clearly visible and was also reported in Ge et al.11 was the apparent switching of the axes of the main orifice jet downstream of the leaflets. The jet in between the two leaflets evolved under the action of the two vortex pairs on each side of the sinus chamber. The center jet in the experiments was similar to that of the simulations results obtained at Re = 350, Re = 750 and Re = 1000. Next, the SA turbulence model used in our simulation was compared to the \(k{-}\epsilon\) model and similar vorticity contours were found. At high Reynolds number, the SA model was able to show the basic flow features. Nevertheless, further work is required to validate the simulation results.

Our work constitutes an important step towards developing a more accurate numerical simulation for BMHV flows. The simulations used are able to provide a reasonably accurate and reliable solver. Further CFD work can be done to address the increase in complexity of the simulations using fluid structure interactions.

Acknowledgments

The authors are grateful to Professor Yeo Joon Hock of the School of Mechanical & Aerospace Engineering at Nanyang Technology University, Singapore, for arranging access to his Particle Imaging Velocimetry equipment. This work was supported primarily by a research grant from the Ministry of Education, Singapore (MOE) AcRF Tier 1 (R-397-000-085-133).

Copyright information

© Biomedical Engineering Society 2011