Revision as of 11:11, 4 October 2019

Aerosol deposition in the human upper airways

Application Challenge AC7-01 © copyright ERCOFTAC 2019

CFD Simulations

Overview of CFD Simulations

LES and RANS simulations were carried out in the benchmark geometry. The details of these numerical tests and their predicted deposition are given in the following paragraphs. In summary, the main differences in LES and RANS simulations are:

Computational meshes
Turbulence modeling
Different outlet boundary conditions
In RANS simulations a turbulent dispersion model was used to account for the effect of turbulence on particle transport.

Large Eddy Simulations

Computational domain and meshes

The geometry used in the calculations is the same as the one used in the experiments developed by the group in Brno University of Technology (BUT). The computational domain, shown in Figure 10, has one inlet and ten different outlets, for which appropriate boundary conditions must be speciﬁed in the simulations.

Figure 10: Computational domain viewed from different angles.

The digital model of the physical geometry was used to generate a proper computational mesh in order to perform the simulations. For the LES simulations, three meshes were generated to allow us to examine the sensitivity of the results on the mesh resolution. The coarser mesh includes 10 million computational cells, the intermediate one 30 million cells and the ﬁner approximately 50 million cells. In these meshes, the near-wall region was resolved with prismatic elements, while the core of the domain was meshed with tetrahedral elements. Cross-sectional Views of these meshes at seven stations are shown in ﬁgure 11. A grid convergence analysis was carried out in order to determine the appropriate resolution for the LES simulations. This analysis is presented in section 3.2.4.

Table 5 reports grid characteristics, such as the height of the wall-adjacent cells ${\Delta r_{min}}$ , the number of prism layers near the walls, the average expansion ratio of the prism layers ( ${\lambda }$ ), the total number of computational cells, the average cell volume ( ${V}$ ) and the average and maximum ${y+}$ values. The higher ${y+}$ values (above 1) are found near the glottis constriction and the bifurcation carinas, which are characterised by high wall shear stresses.

Solution strategy and boundary conditions – Airﬂow

Large Eddy Simulations (LES) are performed using the dynamic version of the Smagorinsky-Lilly subgrid scale model (Lilly, 1992) in order to examine the unsteady ﬂow in the realistic airway geometries. Previous studies have shown that this model performs well in transitional ﬂows in the human airways (Radhakrishnan & Kassinos, 2009; Koullapis et al., 2016). The airﬂow is described by the ﬁltered set of incompressible Navier-Stokes equations,

${{\frac {\partial {\bar {u}}_{j}}{\partial x_{j}}}=0}$	${(10)}$
${{\frac {\partial {\bar {u}}_{i}}{\partial t}}+{\bar {u}}_{j}{\frac {\partial {\bar {u}}_{i}}{\partial x_{j}}}=-{\frac {1}{\rho }}{\frac {\partial {\bar {p}}}{\partial x_{i}}}+{\frac {\partial }{\partial x_{j}}}\left[(\nu +\nu _{sgs}){\frac {\partial {\bar {u}}_{i}}{\partial x_{j}}}\right],}$	${(11)}$

where ${{\bar {u}}_{i},{\bar {p}},\rho =1.2kg/m^{3},\nu =1.7\times 10^{-5}m^{2}/s}$ and ${\nu _{sgs}}$ are the velocity component in the i-direction, the pressure, the density and kinematic viscosity of air, and the subgrid-scale (SGS) turbulent eddy viscosity, respectively. The overbar denotes resolved quantities.

The governing equations are discretized using a ﬁnite volume method and solved using OpenFOAM, an open-source CFD code. In this framework, unstructured boundary ﬁtted meshes are used with a collocated cell-centred variable arrangement. The ﬁnite volume method in OpenFOAM is in general 2nd-order accurate in space, depending on the convection differencing scheme (CDS) used. Whenever possible (usually in the cases with lower Reynolds numbers), the 2nd-order linear CDS is used.

Contributed by: *** — ***