CFD Simulations AC1-05

From QNET
Jump to navigation Jump to search

Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice

Contents

Ahmed body

Application Challenge 1-05 © copyright ERCOFTAC 2004


Overview of CFD Simulations

CFD simulations have developed rapidly during the writing of the present document, during the MOVA consortium and in the frame of the 9th and 10th ERCOFTAC-IAHR Workshop on Refined Turbulence Modeling organized in Darmstad, Germany and Poitiers, France, in 2001 and 2002, respectively. These workshops were organized under the auspices of the Special Interest Group 15 on Turbulence Modeling of ERCOFTAC. The proceedings of the 10th ERCOFTAC-IAHR Workshop can be found at:

http://www.ercoftac.nl/workshop10/index.html

For the 10th ERCOFTAC-IAHR Workshop, several recommendations were made to the groups participating in the CFD calculations. Among them the recommendation to extend the computational domain up to 5 times the car length downstream of the body, and the possibility to omit the stilts.

Many of the CFD results are considered by the authors themselves as preliminary computations and were therefore not inserted into the knowledge base.

The geometry is simple enough to be satisfactorily represented.

Simulation Case CFD1

Solution strategy CFD1

RANS modelling.

Commercial FLUENT 4.2 code, based on unstructured finite volume discretization.

Reynolds number: 4.29x106 (see EXP1). Steady state computation.

The slant angle is varied from 0 to 50 degrees.


Computational Domain CFD1

Symmetry is used to compute half the domain.

Domain: [-3L;5L]x[0;2L]x[0;2L]

Mesh : 450,000 cells

Approximate value of y+ on solid surfaces : 30.


Boundary Conditions CFD1

Inlet: turbulence level 0.5% with a mixing length of 5x10-3m.

Outlet: constant pressure.

Solid boundaries: wall functions

Symmetry plane: symmetry

Other boundaries: no details


Application of Physical Models CFD1

Standard K-ε model with standard wall functions.


Numerical Accuracy CFD1

Mesh refinement is performed until the drag reaches a constant value.

Convection scheme : 2nd order.


CFD Results CFD1

Friction lines, pressure iso-contours at the model surface, velocity vector fields, drag coefficient.

References CFD1

Modelling of stationnary three-dimensional separated flows around an Ahmed reference model.

P. Gilliéron, F. Chometon, ESAIM proc., vol 7, 173-182, 1999


Simulation Case CFD2

Solution strategy CFD2

RANS modeling.

Commercial FLUENT 5 code based on unstructured finite volume discretization.

Reynolds number: 4.29x106 (see EXP1). Steady state computation.

Slant angle: 30°.

Computational Domain CFD2

Symmetry is used to compute half the domain. Stilts are included.

Domain: no details.

Mesh : 704,000 cells.

y+ at the first grid point from the wall of order of 50 - 350.

Boundary Conditions CFD2

No details.

Application of Physical Models CFD2

- Standard k-ε model with non-equilibrium wall functions.

- RSM (no details) with non-equilibrium wall functions.

Numerical Accuracy CFD2

No details.

CFD Results CFD2

Pathlines and velocities.

Aerodynamic drag coefficient.

References CFD2

Advances in external-aero simulation of ground vehicles using the steady RANS equation.

Makowski F.T and Kim S.E., SAE Conf 2000-01-0484


Simulation Case CFD3

Solution strategy CFD3

Large-eddy simulation.

In house code PRICELES, based on unstructured second-order finite-element discretization.

Reynolds number= 4.29 x106

Slant angle: 28°.

Computational Domain CFD3

Domain: [-3L;5L]x[-L;L]x[-LxL] (the ground plate is NOT included: the body is suspended in the middle of the domain).

Mesh: 1.6x106 cells.

y+ at the first grid point from the wall is about 80 (averaged value).

Boundary Conditions CFD3

Inlet: constant velocity.

Outlet: constant pressure conditions.

Solid boundaries: wall functions

Other boundaries : symmetry.

Application of Physical Models CFD3

Sub-grid model: standard Smagorinsky.

Numerical Accuracy CFD3

Second-order convection scheme and time marching (CFL number=3).

CFD Results CFD3

Pressure, pressure coef., velocity, drag coef, Q-criterion contours, vorticity.

References CFD3

Large eddy simulation of an Ahmed reference model.

R.J.A. Howard, M. Pourquie.

Journal of Turbulence, 2002


Simulation Case CFD4

Solution strategy CFD4

RANS modelling.

Commercial AVL SWIFT code, based on unstructured finite volume discretization.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25° and 35°.

Computational Domain CFD4

Symmetry is used to compute half the domain.

Domain: Inlet at -1.5L. No other details.

Mesh : 530,000 cells.

y+ on solid surfaces < 100.

Boundary Conditions CFD4

Inlet: interpolated experimental profile at –1.4L used at –1.5L.

Solid boundaries: wall functions

Symmetry plane: symmetry

Other boundaries: no details

Application of Physical Models CFD4

- Standard k-ε model with standard wall functions.

- SSG Reynolds stress model with standard wall functions

- Hybrid k-ε/Reynolds stress model (coefficient Cm of the k-ε model obtained from Reynolds stress transport equations) with standard wall functions

Numerical Accuracy CFD4

Grid sensitivity study.

Study of the influence of the convection scheme.

CFD Results CFD4

Cp, velocity profiles in the boundary layer over the slant part.

References CFD4

B. Basara, S. Jakirlic, Flow Around a simplified car body (Ahmed body) : description of numerical methodology, in : S. Jakirlic, R. Jester-Zürker, C. Tropea, editors, 9th ERCOFTAC/IAHR/COST Workshop on Refined Turbulence Modelling, Oct. 4-5, 2001, Darmstadt University of Technology, Germany.


Simulation Case CFD5

Solution strategy CFD5

RANS modelling.

In-house code Saturne, based on unstructured finite volume discretization.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25° and 35°.

Computational Domain CFD5

Full body (no symmetry used)

Domain: no details

Mesh : 300,000 cells

y+ on solid surfaces : no details.

Boundary Conditions CFD5

Inlet: no details.

Solid boundaries: wall functions

Other boundaries: no details

Application of Physical Models CFD5

- Standard k-ε model with standard wall functions

- Launder, Reece, Rodi (IP) Reynolds stress model with standard wall functions

- Linearized production k-ε model with standard wall functions


Numerical Accuracy CFD5

Convection scheme : 80% central differencing (2nd order), 20% upwind differencing (1st order).

CFD Results CFD5

Cp, velocity profiles in the boundary layer over the slant part.

Vector plots, turbulent energy contours, streamlines.

References CFD5

S. Tekam, D. Laurence, T. Buchal, Flow around the Ahmed body, in : S. Jakirlic, R. Jester-Zürker, C. Tropea, editors, 9th ERCOFTAC/ IAHR/ COST Workshop on Refined Turbulence Modelling, Oct. 4-5, 2001, Darmstadt University of Technology, Germany.


Simulation Case CFD6

Solution strategy CFD6

RANS modelling.

Commercial FLUENT code, based on unstructured finite volume discretization.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25°.

Computational Domain CFD6

Domain: no details

Mesh : 2.3x106 cells

y+ on solid surfaces : no details

Boundary Conditions CFD6

Solid boundaries:

- non-equilibrium wall functions for the k-ε model

- no slip walls for the SST model


Inlet, outlet and other boundaries: no details

Application of Physical Models CFD6

- Realizable k-ε model with non-equilibrium wall functions

- SST model

Numerical Accuracy CFD6

No details

CFD Results CFD6

Cp, velocity profiles in the boundary layer over the slant part.

References CFD6

M. Lanfrit, M. Braun, D. Cokljat, Contribution to case 9.4: Ahmed body, in : S. Jakirlic, R. Jester-Zürker, C. Tropea, editors, 9th ERCOFTAC/ IAHR/ COST Workshop on Refined Turbulence Modelling, Oct. 4-5, 2001, Darmstadt University of Technology, Germany.


Simulation Case CFD7

Solution strategy CFD7

RANS modelling in unsteady mode.

In-house X-Stream code, based on finite volume solver for multi block structured non-orthogonal, curvilinear grid with collocated data arrangement. The convection terms are discretized using hybrid scheme with more than 60% central differencing. The diffusion terms are approximated with central differences. The SIMPLE method is used for the pressure-velocity coupling.

Reynolds number: 2.78x106 (see EXP2).

Slant angle: 35°

Computational Domain CFD7

Full body (no symmetry condition used).

Domain: [-2L;5L]x[-1.2;1.2L]x[0;1.3L]

9th ERCOFTAC workshop: 500,000 cells

10th ERCOFTAC workshop: 2 meshes: 490,000 and 820,000 cells (fine mesh used for the k-ε model only)

Approximate value of y+ on solid surfaces:

- 9th workshop: 60

- 10th workshop: 17 (coarse mesh) and 11 (fine mesh).

Boundary Conditions CFD7

Inlet: turbulence intensity=2,5%

Solid boundaries: wall functions

Outlet: no details

Other boundaries: no details

Application of Physical Models CFD7

9th ERCOFTAC workshop:

- Standard k-ε model with standard wall functions

- SSG Reynolds stress model with standard wall functions

- SSS Reynolds stress model with non-equilibrium wall functions

- V2F model with wall functions

- Elliptic blending model (Reynolds stress model) with wall functions


10th ERCOFTAC workshop:

- Standard k-ε model with wall functions

- V2F model with wall functions

- SSG Reynolds stress model with modified ε equation (Hanjalic, Jakirlic) and standard wall functions

Numerical Accuracy CFD7

Convection scheme : 60% 2nd order central differencing, 40% 1st order upwind differencing.

CFD Results CFD7

Cp contours on the slant part, velocity profiles in the boundary layer over the slant part, vectors plots in 13 planes (see EXP2).

References CFD7'

O. Ouhlous, W. Khier, Y. Liu, K. Hanjalic, in: S. Jakirlic, R. Jester-Zürker, C. Tropea, editors, 9th ERCOFTAC/ IAHR/ COST Workshop on Refined Turbulence Modelling, Oct. 4-5, 2001, Darmstadt University of Technology, Germany.


M. Hadziabdic, K. Hanjalic, W. Khier, Y. Liu, O. Ouhlous, Flow around a simplified car body (Ahmed car model), in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD8

Solution strategy CFD8

RANS modelling.

In-house code STREAM, which is a finite volume solver which uses a structured, non-orthogonal curvilinear, multi block grid and a fully collocated arrangement. The SIMPLE pressure correction method and Rie & Chow interpolation are used to prevent unrealistic pressure fluctuations. The convection terms are discretized using an upwind scheme or a TVD scheme based on the third-order QUICK scheme.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25° and 35°.

Computational Domain CFD8

Symmetry is used to compute half the domain. Stilts not included.

Domain: [-2L;4L]x[0;L]x[0;L]

Mesh : 300,000 cells

Approximate value of y+ on solid surfaces : between 55 and 550.

Boundary Conditions CFD8

Inlet:

- U=38.51 m/s (based on the experimental profile at –1.4L in order to account for the flow deceleration in front of the body)

- K=6.58x10-3 m2 s-2

- nt/n=10 (influence tested)


Outflow: zero gradients for all variables

Solid boundaries: wall functions

Symmetry plane: symmetry

Other boundaries: symmetry

Application of Physical Models CFD8

- Standard k-ε model with Yap correction and SCL wall functions (see below)

- Standard k-ε model with Yap correction and UMIST-N wall functions

- Linear realizable k-ε model with SCL wall functions

- Linear realizable k-ε model with UMIST-A wall functions

- Nonlinear k-ε model (Craft et al.) with SCL wall functions

- Nonlinear k-ε model (Craft et al.) with UMIST-A wall functions


Wall functions:

- SCL = Simplified Chieng and Launder

- UMIST-A = UMIST Analytical

- UMIST-N = UMIST Numerical

Numerical Accuracy CFD8

Convection scheme : 3rd order Quick scheme (UMIST) or 1st order upwind scheme in case of numerical instability.

Tests were made to assess iteration convergence. Some unsteady calculations were made too. A coarser grid was used to obtain some information on grid dependency.

CFD Results CFD8

Cp contours on the slant part, velocity profiles in the boundary layer over the slant part, vectors plots in 13 planes (see EXP2).

References CFD8

T.J. Craft, S.E. Gant, H. Iacovides, B.E. Launder, C.M.E. Robinson, Computational methods applied to the study of flow around a simplified “Ahmed” car body, in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD9

Solution strategy CFD9

LES.

In-house code LESOCC2, based on block-structured finite volume discretization. A collocated cell arrangement was used employing the Rhie and Chow momentum interpolation procedure. The SIMPLE scheme was used for the pressure-velocity coupling, and the pressure correction equation was solved using the SIP method. Fluxes were discretized in space using a second order central difference scheme. The equations were integrated in time using a second order Runge Kutta scheme with an adaptive time step, employing a maximum CFL number of 0.6.

Reynolds number: 2.78x106 (see EXP2).

Slant angle: 25°.

Computational Domain CFD9

Domain: [-2.2L;4.8L]x[-0.9L;0.9L]x[0;1.35L]. Ground plate and stilts included.

Mesh :18.5x106 cells

y+ on solid surfaces : no details

Boundary Conditions CFD9

Inlet: constant velocity

Outlet: convective outlet.

Solid boundaries: wall functions

Other boundaries: slip walls

Application of Physical Models CFD9

Subgrid scale model: Smagorinky

Numerical Accuracy CFD9

2nd order convection scheme and time marching (CFL number < 0.6)

CFD Results CFD9

Cp contours on the slant part, velocity profiles in the boundary layer over the slant part, vectors plots in 13 planes (see EXP2).

References CFD9

C. Hinterberger, M. Garcia-Villalba, W. Rodi, Flow around a simplified car body. LES with wall functions, in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD10

Solution strategy CFD10

RANS modelling.

Commercial HEXANS CFD code, based on unstructured finite volume discretization. The convective fluxes are discretized using a centered scheme with 2nd and 4th order artificial dissipation. Diffusive fluxes are computed on pyramidal elements. The equations are integrated in time using the explicit Runge Kutta scheme. Local time stepping, multi grid and low-mach number preconditioning are used to accelerate the convergence to steady state. A mesh adaptation procedure is used in which the grid cells are refined by splitting it in 2, 4 or 8 subcells. The mesh adaptation is governed by criteria based on the flow physics, geometry or error estimates.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25°.

Computational Domain CFD10

Symmetry is used to compute half the domain. Ground plate included, no stilts.

Domain: [-2L;5L]x[0;0.9L]x[0;1.35L]

Final Mesh : 815,000 cells

Approximate value of y+ on solid surfaces : 1

Boundary Conditions CFD10

Inflow: turbulence level 1%. nt/n = 1.

Solid boundaries: no-slip walls

Symmetry plane: symmetry

Other boundaries: no details

Application of Physical Models CFD10

Low-Reynolds number K-ε model (Yang-Shih).

Numerical Accuracy CFD10

Mesh adaptation applied.

Convection scheme : 2nd order.

CFD Results CFD10

Cp contours on the slant part, velocity profiles in the boundary layer over the slant part, vectors plots in 13 planes (see EXP2).

References CFD10

B. Leonard, Ch. Hirsch, K. Kovalev, M. Elsden, K. Hillewaert, A. Patel, Flow around a simplified car body (Ahmed body), in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD11

Solution strategy CFD11

RANS modelling.

Commercial CFX-5 code, based on an unstructured, vertex based finite volume method. Co-located variables are used. The solver is second order accurate in space and time. The Rhie-Chow velocity pressure coupling is used. An implicit solver with algebraic multi grid is used to converge the equations to steady state.

Reynolds number: 2.78x106 (see EXP2). Transient computation (steady solution obtained).

Slant angle: 25° and 35°.

Computational Domain CFD11

Symmetry is used to compute half the domain. No stilts included.

Domain: [-3L;6L]x[0;0.9L]x[0;1.15L]

The ground plate starts 2L in front of the body in order that the boundary layer approaching the body matches the experimental profile.

Mesh : 2,5x106 cells

Approximate value of y+ on solid surfaces : 1

Boundary Conditions CFD11

Inlet: turbulence intensity=1%, nt/n=1.

Solid boundaries:

- SST model: no slip walls

- Others: scalable wall functions

Outlet: constant pressure

Other boundaries: opening boundary conditions.

Application of Physical Models CFD11

- Standard k-ε model with scalable wall functions

- SST model

- SSG Reynolds stress model with scalable wall functions

Numerical Accuracy CFD11

Convection scheme: 2nd order.

Studies of the influence of the following parameters are performed:

Mesh refinement, formulation of the boundary conditions (opening vs. slip walls), advection scheme.

CFD Results CFD11

The same quantities (except for triple correlations) as for experiment EXP2 are available in the Knowledge Base : results for the mean velocities U, V, W, Reynolds stresses Image23.gif Image24.gif Image25.gif Image26.gif Image27.gif in some planes and profiles in the boundary layer above the slant part:



k-epsilon model

25° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


35° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


SST model

25° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


35° slant angle: planes: y=0; y=100; y=180;

y=195; z=360

x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp

References CFD11

L. Durand, M. Kuntz, F. Menter, Validation of CFX-5 for the Ahmed car body (synopsis), in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


L. Durand, M. Kuntz, F. Menter, Validation of CFX-5 for the Ahmed car body, CFX Validation report (florian.menter@ansys.com)


Simulation Case CFD12

Solution strategy CFD12

RANS modelling.

In-house code CFL3D, compressible flow solver employing multi block structured grids. An upwind finite volume formulation is used for the space discretization. An implicit approximate factorization method is used to integrate the equations in time. Local time stepping, grid sequencing, multi grid and low Mach number preconditioning are used to accelerate convergence to steady state.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25° and 35°.

Computational Domain CFD12

Symmetry is used to compute half the domain. No stilts included.

Domain: [-3L;6L]x[0;0.9L]x[0;1.15L]

Mesh : 1.3x106 cells

Approximate value of y+ on solid surfaces : 1.5

Boundary Conditions CFD12

Inlet: no details

Solid boundaries: no-slip walls

Symmetry plane: symmetry

Other boundaries: farfield Riemann-invariant conditions

Application of Physical Models CFD12

- SST model

- Explicit Algebraic Stress Model with ω-equation

Numerical Accuracy CFD12

Convection scheme : 1st order.

CFD Results CFD12

The same quantities (except for triple correlations) as for experiment EXP2 are available in the Knowledge Base : results for the mean velocities U, V, W, Reynolds stresses Image23.gif Image24.gif Image25.gif Image26.gif Image27.gif in some planes and profiles in the boundary layer above the slant part:


SST model

25° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


35° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


EASM model

25° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp


35° slant angle:

planes: y=0; y=100; y=180;

y=195; z=360

x=-794; x=-178; x=-138; x=-88; x=-38; x=0; x=80; x=200; x=500

profiles in the boundary layer: x=-243, -223, -203, -183, -163, -143, -123, -103, -83, -63, -43, -23, -3

Pressure coefficients on the rear of the body: Cp

References CFD12

C.L. Rumsey, Application of CFL3D to case 9.4 (Ahmed Body), in: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD13

Solution strategy CFD13

RANS modelling.

In-house code STREAM, which is a finite volume solver which uses a structured, non-orthogonal curvilinear, multi block grid and a fully collocated arrangement. The SIMPLE pressure correction method and Rie & Chow interpolation are used to prevent unrealistic pressure fluctuations. The convection terms are discretized using an upwind scheme or a TVD scheme based on the third-order QUICK scheme

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25°.

Computational Domain CFD13

Symmetry is used to compute half the domain. No stilts included.

Domain: [-3L;6L]x[0;0.9L]x[0;1.15L]

Mesh : 1.3x106 cells

Approximate value of y+ on solid surfaces : 1

Boundary Conditions CFD13

Inlet: no details

Solid boundaries: no-slip walls

Other boundaries: symmetry

'Application of Physical Models CFD13

All are low-Reynolds number models

- Linear k-ε model (Launder-Sharma)

- Linear k-ω model (Wilcox)

- Cubic k-ε model (Apsley, Leschziner)

- Quadratic k-ω model (Abe, Jang, Leschziner)

- Quadratic k-ε model (Abe, Jang, Leschziner)

- SSG + Chen (Abe, Jang, Leschziner)

Numerical Accuracy CFD13

No details

CFD Results CFD13

Cp contours on the slant part, velocity profiles in the boundary layer over the slant part, vectors plots in 13 planes (see EXP2).

References CFD13

Y.J. Jang, M. Leschziner, Contribution of Imperial College to Test Case 9.4: Flow around a simplified car body, In: R. Manceau, J.-P. Bonnet, editors, 10th ERCOFTAC (SIG-15)/IAHR/QNET-CFD Workshop on Refined Turbulence Modelling, Oct. 10-11, 2002, Laboratoire d’études aérodynamiques, UMR CNRS 6609, Université de Poitiers, France.


Simulation Case CFD14

Solution strategy CFD14

RANS modelling.

In-house code ISIS, based on unstructured finite volume discretization.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25° and 35°.

Computational Domain CFD14

Symmetry is used to compute half the domain.

Domain: [-4L;5L]x[0;0.9L]x[0;1.35L]

Mesh : 3.8x106 cells

Approximate value of y+ on solid surfaces: 0.5

Boundary Conditions CFD14

Solid boundaries: no slip wall

Symmetry plane: symmetry

Other boundaries: no details

Application of Physical Models CFD14

SST model

Numerical Accuracy CFD14

No details

CFD Results CFD14

Velocity profiles in the boundary layer over the slant part, streamlines, turbulent energy contours.

References CFD14

E. Guilmineau, Numerical simulation of flow around a simplified car body, Proc. ASME JSME Joint Fluids Engineering Conference, July 6-10, 2003, Honolulu, Hawaii, USA


Simulation Case CFD15

Solution strategy CFD15

RANS modelling.

Commercial StarCD code, based on unstructured finite volume discretization.

Reynolds number: 2.78x106 (see EXP2). Steady state computation.

Slant angle: 25°.

Computational Domain CFD15

Symmetry is used to compute half the domain. No stilts included. The ground plate starts 2L upstream of the body in order to reproduce the experimental boundary layer.

Domain: [-5.75L;5.75L]x[0;L]x[0;1.35L]

Mesh : 1.6x106 cells

Approximate value of y+ on solid surfaces : < 3

Boundary Conditions CFD15

Inlet: turbulence level 0.1%, nt/n=10.

Outlet: convective outlet.

Solid boundaries: no-slip walls

Symmetry plane: symmetry

Other boundaries: symmetry

Application of Physical Models CFD15

Rescaled V2F model (Manceau, Carlson, Gatski)

Numerical Accuracy CFD15

No details.

CFD Results CFD15

Vector plots.

References CFD15

R. Manceau, Computation of the flow around a simplified car using the rescaled v2f model, Proc. ASME JSME Joint Fluids Engineering Conference, July 6-10, 2003, Honolulu, Hawaii, USA



Table CFD-A Summary Description of All Test Cases
NAME Re x 10-6 Slant angle (degrees) SPs
Detailed Data DOAP
CFD1 4.29 0, 10, 12, 20, 25, 30, 40, 50 Pressure Tomographies Cd, Streamlines, Friction Lines
CFD2 4.29 30 Effective Viscosity CD, Velocities
CFD3 4.29 28 Pressure Coefficient, Q-criterion Contours Cd, Velocities, Vorticity Contours
CFD4 2.78 25, 35 CP Velocity Profiles
CFD5 2.78 25, 35 CP, Turbulent Energy Contours Velocity Profiles, Vector Plots, Streamlines
CFD6 2.78 25 CP Velocity Profiles
CFD7 2.78 35 CP Velocity Profiles, Vector Plots
CFD8 2.78 25, 35 CP Velocity Profiles, Vector Plots
CFD9 2.78 25, 35 CP Velocity Profiles, Vector Plots
CFD10 2.78 25 CP Velocity Profiles, Vector Plots
CFD11 2.78 35 CP Cd, Velocity Profiles, Vector Plots
CFD12 2.78 25, 35 CP Velocity Profiles, Vector Plots
CFD13 2.78 25 CP Velocity Profiles, Vector Plots
CFD14 2.78 25, 35 Turbulent Energy Contours Velocity Profiles, Streamlines
CFD15 2.78 25 Vector Plots



© copyright ERCOFTAC 2004



Contributors: Remi Manceau; Jean-Paul Bonnet - Université de Poitiers

Site Design and Implementation:Atkins and UniS


Front Page

Description

Test Data

CFD Simulations

Evaluation

Best Practice Advice