HiFi-TURB-DLR rounded step

Semi-confined flows

Underlying Flow Regime 3-36

Test Case Study

Brief Description of the Study Test Case

In the framework of the project, four different geometries with different separation behaviors were designed. Each configuration was computed with two different Reynolds numbers. The configuration described here presents an incipient separation test case where the flow is on the brink of separation but does not separate with Reynolds number ${Re_{H}=78,490}$ based on the step height ${H}$ .The geometry of this UFR alongside the mesh is shown in Fig. 1. The geometry comprises three main sections: Constant-Width Forebody section ${L_{F}}$ with the largest width ${Y_{F}}$ , Contoured Boat-tail section ${L_{B}}$ with the contoured width ${Y_{B}}$ and Constant-Width-Aftbody section ${L_{A}}$ with the smallest width ${Y_{A}}$ . The width of the last section is modified to generate the desired APG. This modification is achieved through the variation of ${\sigma }$ , which is the ratio of ${Y_{A}}$ to ${Y_{F}}$ . For incipient separation, $\sigma =0.62$ .

Figure 1: Flow Domain and grid of RANS simulations

The parametric geometry definition for the three relevant sections is given in [‌6] and is depicted in Fig. 1. The axial origin ${x=0}$ is set at the beginning of the Contoured Boat-tail section.

{\begin{aligned}y_{wall}&=y_{F}=H/(1-\sigma )\qquad \mathrm {for} \qquad -L_{F}<x/H\leq 0\\y_{wall}&=y_{B}=a_{1}+a_{2}x^{3}+a_{3}x^{4}+a_{4}x^{5}\qquad \mathrm {for} \qquad 0<x/H\leq L_{B}\qquad \qquad (1)\\y_{wall}&=Y_{A}=\sigma H/(1-\sigma )\qquad \mathrm {for} \qquad L_{B}<x/H\leq L_{B}+L_{A}\\\\\end{aligned}}

with ${a_{1}=H/(1-\sigma )}$ , ${a_{2}=-10H/L_{B}^{3}}$ , ${a_{3}=15H/L_{B}^{4}}$ and ${a_{4}=-6H/L_{B}^{5}}$ with ${\sigma =Y_{A}/Y_{F}=0.62}$ .

The different parameters with the corresponding values are listed in the table below:

Parameter	${L_{F}}$	${L_{B}}$	${L_{A}}$
Value	${11.8H}$	${5.5H}$	${14.5H}$

Table 1: Geometry parameters

CFD Methods

Reynolds-Averaged Navier-Stokes computations

SSG/LRR- $\omega$ model

For the entire computational domain, a structured 2D mesh was created using Pointwise V18.2. Sensitivity studies were carried out on various meshes and the final mesh used in this UFR contains a total of $266,112$ points. Along the body contour $448$ points are used in streamwise direction with a smaller spacing in the focus region. In the normal direction to the body wall $298$ points are used, $98$ of which are concentrated near the body wall region. The body wall-normal growth ratio is approximatively $1,077$ and the dimensionless distance from the wall is ${y^{+}<1}$ along the body wall for all meshes and simulation scenarios. For the inflow boundary situated at ${x=-11.8H}$ a reservoir-pressure inflow boundary condition is used. This boundary condition prescribes total pressure and total density. The inflow direction is by default perpendicular to the boundary face. For the outflow boundary at ${x=20H}$ an exit-pressure outflow boundary condition is used. The exit pressure is adapted during the simulation to match the reference pressure at the coordinate point ${Z_{ref}=(-5.18H,0,6.25H)}$ . The upper boundary is a far-field boundary condition situated ${179H}$ from the viscous body wall. Symmetry boundary condition is used on both side planes of the 2D domain. Reference parameters for ${Re_{H}=78,490}$ are presented in Table 2.

Parameter	${Ma}$	${P_{exit}}$	${P_{t,inflow}}$	${\rho _{t,inflow}}$	${T_{t,inflow}}$	${P_{s,ref}}$	${\rho _{s,ref}}$	${T_{s,ref}}$	${P_{(Z{ref})}}$
Value	${0.13455}$	${89769Pa}$	${93074Pa}$	${1.0943kg/m^{3}}$	${296.36K}$	${89593.581Pa}$	${1.065kg/m^{3}}$	${293.15K}$	${89300Pa}$

Table 2: Boundary conditions

with the Mach number $Ma$ , the exit pressure ${P_{exit}}$ , total inflow pressure ${P_{t,inflow}}$ , total inflow density ${\rho _{t,inflow}}$ , total inflow temperature ${T_{t,inflow}}$ , statistic pressure ${P_{s,ref}}$ at the reference position $Z_{ref}$ , statistic density ${\rho _{s,ref}}$ at the reference position $Z_{ref}$ , statistic temperature ${T_{s,ref}}$ at the reference position $Z_{ref}$ and the measured pressure ${P_{(Z{ref})}}$ at the reference position $Z_{ref}$ .

Simulations were performed using the DLR in-house software TAU [‌8] where the SSG/LRR- $\omega$ model is already implemented along with the length-scale correction. TAU is a Finite-Volume-based unstructured cell-centered on dual-grids code of second-order accuracy. For the computations performed here, the mean-flow and turbulence convective terms are discretized using second-order central schemes together with Matrix Dissipation. Low-Mach number preconditioning was applied and steady computations using a LU-SGS scheme were performed. All results presented in this report are based on fully converged simulations.

K- $\omega$ model

DNS Computations

The test case is designed as a numerical experiment with the aim of comparing RANS results to DNS data. For the set-up of the DNS, the inflow boundary conditions are different, e.g. a recycling method can be used to generate the turbulent input or synthetic turbulence can be injected. It is also possible to numerically trip the boundary layer from laminar to turbulent to generate the desired turbulent boundary layer. Hence, to ensure a comparison to the results achieved with RANS turbulence models, a reference position upstream of the APG-area is defined where boundary layer properties need to match between RANS and DNS computations to permit the comparison downstream in the region of interest. The reference position is located at ${x/H=-3.51}$ . Depending on the generation of turbulence at the inlet, the computational domain needs to be adapted to ensure the correct boundary layer properties at the reference position. If numerical tripping is performed, the laminar and turbulent distances need to be determined upstream of the reference position by precursor simulation as displayed in Fig. 2.

Figure 2: Set-up for DNS Simulation

At the reference position ${x_{ref}}$ , the properties of the turbulent boundary layer are determined by the Reynolds number based on the momentum thickness ${Re_{\theta }=1496}$ and the Reynolds number based on the friction velocity ${Re_{\tau }=609}$ computed with SA-neg-RC-QCR-LRe model. To estimate the computational effort for DNS, the largest values of ${Re_{\theta }}$ and ${Re_{\tau }}$ are also given at the position ${x/H=10.5}$ by $4,624$ and $1,399$ respectively.

Amongst the different flow condition proposed, UNIBG focused the effort on the incipient separation configuration case with ${Re_{H}=78,490}$ . A precursory computational campaign for the turbulent flow over a flat plate has been performed with the purpose of (i) assessing the effectiveness of the Synthetic Inlet Turbulence (SIT) injection strategy inspired by the work of Housseini et al. [‌18] and Schlatter and Örlü [‌19]; (ii) investigating the influence of the mesh density on the solution; (iii) defining the inlet boundary position and flow condition that ensure the target boundary layer integral parameters at the reference location ${x_{ref}}$ (see Fig. 3). According to the outcomes of this campaign, the inlet boundary is set at ${x/H=-12.71}$ , where the Blasius laminar velocity profile computed at ${Re_{x}=650,000}$ , the uniform static pressure and the uniform total temperature (see Table 2) are imposed. At location ${x/H=-12.1}$ , within the laminar boundary layer region, the tripping source term is activated to promote the transition to turbulence [‌18][‌19]. The outlet boundary is positioned at ${x/H=23.95}$ , with a pressure outflow condition having the same value of the inlet static pressure and at the end of a streamwise coarsened mesh region starting at ${x/H=13.82}$ . Following the setup of the RANS computations, the no-slip adiabatic boundary condition is set while at the upper boundary, situated at ${179H}$ from the wall upstream the smooth bump, the far-field boundary condition is imposed. Side planes, instead, are considered as periodic with a distance from each other of ${\Delta z=3H}$ .

The DNS have been performed by using the UNIBG in-house software MIGALE [‌20]. MIGALE is an implicit high-order discontinuous Galerkin solver for the compressible and incompressible Navier-Stokes equations. Godunov fluxes are treated with the exact solution of the local Riemann problems while viscous fluxes are handled by means of the BR2 scheme [‌21]. The time integration is performed with linearly implicit Rosenbrock type Runge-Kutta schemes with optimal stability properties up to order five. The computational mesh is made of $15,016,384$ hexahedral elements with quadratic edges concentrated near the wall region. The wall-normal growth ratio is approximatively $1.2$ with a first cell height of ${y^{+}\approx 1}$ . Time integration is performed with the fifth order – eight stages Rosenbrock scheme ROD5_1 [‌22] using a global time step adaptation strategy [‌23]. The corresponding average step size is ${\Delta t=19/14000}$ CTU, where the convective time unit (CTU) is defined as the ratio between ${H}$ and the freestream velocity ${U_{\infty }}$ . Turbulence statistics have been collected for $26$ CTU.

Data provided

Data provided here are from RANS as well as DNS simulations. All quantities are non-dimensionalised with the step height $H$ and the freestream velocity ${U_{\infty }}$ :