CFD Simulations AC7-02

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

Airflow in the human upper airways

Application Challenge AC7-02   © copyright ERCOFTAC 2020

Overview of CFD Simulations

Three LES (LES1-3) and one RANS simulation were carried out in the benchmark geometry at an air flowrate of 60 L/min. This flowrate results in a Reynolds number of 4921 in the model’s trachea. This is slightly higher than the Reynolds number in the experiments, due to the reasons discussed in section 2.4. The details of the numerical tests are given in the following paragraphs. In summary, the main differences between the simulations are:
1. Computational meshes: LES1&2 employ the same comp. meshes, whereas LES3 and RANS use different meshes.
2. Turbulence modeling: LES1 uses the dynamic version of the Smagorinsky-Lilly subgrid scale model, whereas LES2&3 employ the Wall-adapting eddy viscosity (WALE) SGS model. In RANS simulations, the k-ω SST, standard k-ε and RNG k-ε turbulence model have been tested.
3. Discretisation method: LES1&2 and RANS use the Finite Volume approach whereas LES3 employs the Finite Element Method.

Large Eddy Simulations — Case LES1

Computational domain and meshes

The geometry used in the calculations is the same as the one used in the experiments developed by the group at Brno University of Technology (BUT). The computational domain, shown in Fig. 8, has one inlet and ten different outlets, for which appropriate boundary conditions must be specified in the simulations.

Figure 8: 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 LES1, two meshes were generated to allow us to examine the sensitivity of the results to the mesh resolution. The coarser mesh includes 10 million computational 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 Fig. 9. A grid convergence analysis was carried out in order to determine the appropriate resolution for the simulations. This analysis is presented in section 3.2.3. Table 3 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.

Figure 9: Cross-sectional views of the three generated meshes employed in LES1&2 at seven stations (A-G).

Table 3: Characteristics of Meshes 1-3. $\Delta r_{min}$ is the height of the wall-adjacent cells, $\lambda$ the average expansion ratio of the prism layers and $V_{cell,avg}.$ the average cell volume in the domain.

Solution strategy and boundary conditions — Airflow

LES were performed using the dynamic version of the Smagorinsky-Lilly subgrid scale model with localized filtering (Lilly, 1992; Zang et al., 1993) 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,

where ${\overline {u}}_{i}$, p, $\rho =1.2kg/m^{3}$, $\nu =1.59\times 10^{-5}m^{2}/s$ and $\nu _{sgs}$ are the filtered velocity component in the i-direction, the filtered 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 (OpenFOAM Foundation, 2013b,a). 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. The order of accuracy had to be decreased in some cases in order to stabilize the simulation. In these cases, the clippedLinear scheme was used, which provides a good compromise between the accuracy of the (2nd order) linear scheme and the stability of the (1st order) mid-point scheme (OpenFOAM Foundation, 2013b). The temporal derivative is discretized using backward differencing, which is is also second order accurate in time and implicit. To ensure numerical stability the time step used is $2.5\times 10^{-6}s$ at inhalation flowrate of 60 L/min. The non-linearity in the momentum equation is lagged in OpenFOAM (linearization of equation before discretisation). The system of partial differential equations is treated in a segregated way, with each equation being solved separately with explicit coupling between the results. In turbulent flow applications, where the time step is kept small enough to capture the smaller turbulent time scales, the pressure-implicit split-operator algorithm, or PISO-algorithm, is used.

At the inhalation flowrate of 60 L/min, the Reynolds number at the inlet, based on the inflow bulk velocity and inlet tube diameter, is $Re_{in}={\frac {u_{in}D_{in}}{\nu }}=3745$, which lies in the turbulent regime. In order to generate turbulent inflow conditions, a mapped inlet, or recycling, boundary condition was used (Tabor et al., 2004). To apply this boundary condition, the pipe at the inlet was extended by a length equal to ten times its diameter, as shown in fig. 9. The pipe section was initially fed with an instantaneous turbulent velocity field generated in a precursor pipe flow LES. During the simulation of the airway geometry, the velocity field from the mid-plane of the pipe domain was mapped to the extended pipe’s inlet boundary (fig. 9). Scaling of the velocities was applied to enforce the specified bulk flow rate. In this manner, turbulent flow is sustained in the extended pipe section, and a turbulent velocity profile enters the mouth inlet. To match the experimental conditions, uniform pressure is prescribed in the simulations at the 10 terminal outlets. A no-slip velocity condition is imposed on the airway walls.

RANS Simulations

Numerical accuracy

---

Contributed by: P. Koullapis^a, J. Muela^b, O. Lehmkuhl^c, F. Lizal^d, J. Jedelsky^d, M. Jicha^d, T. Janke^e, K. Bauer^e, M. Sommerfeld^f, S. C. Kassinos^a — 
^aDepartment of Mechanical and Manufacturing Engineering, University of Cyprus, Nicosia, Cyprus
^bHeat and Mass Transfer Technological Centre, Universitat Politècnica de Catalunya, Terrassa, Spain
^cBarcelona Supercomputing center, Barcelona, Spain
^dFaculty of Mechanical Engineering, Brno University of Technology, Brno, Czech Republic
^eInstitute of Mechanics and Fluid Dynamics, TU Bergakademie Freiberg, Freiberg, Germany
^fInstitute Process Engineering, Otto von Guericke University, Halle (Saale), Germany

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

© copyright ERCOFTAC 2020