SlideShare a Scribd company logo
1 of 18
Download to read offline
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Simulation of Flow over Ahmed Body using OpenFoam -
Visual CFD software
Introduction
The aim of this study is to validate the Drag Coefficient of steady-state incompressible
turbulent flow around the Ahmed Body
The aerodynamic behavior of the Ahmed body with slant angle 250
is investigated
numerically.
The Reynolds number Re of the flow is 2.8*106
The open source CFD tool OpenFoam 2.3.1 is tested for its ability to reproduce the
aerodynamic drag coefficient of the body.
External aero case setup is done using ESI’s software Visual-CFD 12.0
Drag coefficient is compared with the experimental results from literature.
Geometry
The generic Ahmed Body reference model has been chosen as the benchmark for
carrying out computations for studying of the aerodynamic parameters. The body
was first proposed by Ahmed et al., (1984).The Ahmed body is a very simple bluff
body which has its shape simple enough to allow for accurate flow simulation but
retains some important practical features relevant to automobile bodies. It has a
slant on its rear end, whose angle can be manipulated and the corresponding drag
and lift coefficients calculated.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Geometry of Ahmed Body
Wind Tunnel
STL format of 3D CAD model of Ahmed Body geometry with 250
slant angle is used
for the analysis. Geometry is placed in wind tunnel of dimensions
(15mX1.4mX1.87m) with respect to X, Y and Z directions respectively.
Front space length is kept equal to 3 times the length of geometry and rear space
length is kept 6 times length of geometry.
Wind tunnel has 6 faces namely XMin, XMax, YMin, YMax, ZMin and ZMax.
Geometry is located at ground YMin.
Geometry is mounted on 4 stilts.
Projected area of geometry along positive X direction including stilts is 0.115 m2
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Wind Tunnel of dimensions (15mX1.4mX1.87m)
Flow Physics
Fluid Properties:
Fluid is Air
Density of the fluid rho = 1.225 kg/m3
Dynamic Viscosity of fluid µ = 1.84*10-5
Ns/m2
Kinematic Viscosity = Dynamic Viscosity/Density = 1.502*10-5
m2
/s
Reynolds number of the flow Re = U*L/ = 2.8*106
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Boundary Conditions:
Inlet (XMin): Fluid Velocity, U = 40 m/s
Outlet (XMax): No external pressure applied with zeroGradient Velocity
Wall: Geometry Surfaces and Ground (YMin)
Symmetry: ZMin, ZMax and YMax
Time dependence: Steady State analysis.
Turbulence Modelling
Turbulence quantities can be calculated by following formula
Turbulent Kinetic Energy
k = 1.5(UI) 2
I is turbulent intensity in percentage
U is free stream velocity
Energy Dissipation
omega= k0.5
/ (Cu
0.25
*l)
Where Cu is model constant = 0.09
l = length scale which can be estimated as 0.07L.
L is characteristic length
Turbulence quantities used for study are mentioned below
k = 0.287 m2
/s2
, omega = 0.215 s-1
Turbulence model used is kOmegaSST
Spalding Wall functions (nutUSpaldingWallFunction in OpenFoam) is used on Walls.
Y-plus, First cell height and Boundary layers
The near wall region is meshed using the calculated first cell height value with
gradual growth in the mesh so that the viscous effects are captured and avoiding
overall heavy mesh count.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Yplus value should be in range 30-300 when Reynolds Average Stress turbulence
(RAS) models are used. There are various Yplus online calculators available. We
have used the one from CFD Online
Mesh definition in Visual CFD
YPlus of 50 was chosen for this study and obtained first cell height (FCH) of 0.478
mm (~0.5mm). This is minimum cell size to be created near walls to accurately
capture viscous effects. This given initial guess for user about the smallest cell size
to be created in computational domain to fairly capture the effects of fluid flow.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Boundary layer thickness can be calculated from below formula
δ = x*0.382/Rex
0.2
, where x is the distance in downstream where turbulent boundary
layer starts. Transition to turbulence will be at Re = 10*105
. We have taken total
length of the geometry L = 1.044m and calculated total boundary layer thickness
equal to 15mm.
So, in order to capture turbulent flow accurately, FCH should be within δ=15mm.
Meshing
Base cell size (bsc) is set to 100mm.
‘blockMesh’ utility of OpenFOAM will create a structured hexahedral grid of 100 mm
(bsc) throughout wind tunnel. Output of blockMesh is input to ‘snappyHexMesh’
utility. This creates unstructured polyhedral meshes.
snappyHexMesh works in 3 stages.
1. Snapping: In this stage, fluid mesh is attached to geometry surfaces.
2. Castellation: In this stage, grid refinement occurs.
3. Layer addition: Snapped and Castellated mesh will be projected outwards
from geometry and boundary layers are created near walls.
Total drag force is the summation of Pressure force and Viscous force.
To capture drag due to viscous forces, we have to resolve by creating fine meshes
and boundary layers near walls.
To capture drag due to pressure forces, we have to refine fluid cells in front and
rear part of the geometry. This is done by creating refinement regions
Boundary layers creation
Surface mesh size on walls are set to 3.125mm. FCH in OpenFOAM is based on
surface mesh size. With relative mesh size on, FCH is set to 0.08. This means the
first cell height will be equal to 0.08*3.125 = 0.25mm. Final layer thickness is
1.85mm
12 boundary layers are created with expansion ratio of 1.2. Total boundary
thickness is calculated from geometry progression and equal to 9.89mm. This
covers around 66% of total boundary layer thickness. This should be sufficient to
capture near wall viscous effects.
Another important parameter in creating boundary layers correctly is final layer
ratio which is equal to final layer thickness/surface cell size. This ratio is equal to
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
0.592 in this case. For proper layers to be created, this ratio should be within range
of 0.2 to 0.6.
Boundary layers are created as shown below
Boundary layers generated from snappyHexMesh
Refinement Regions
Cell sizes at a given refinement level ‘n’ is obtained from following equation written
below
CellSize@nth
level = bsc/2n
Say n = 4, then cell size will be equal to 100/24
= 6.25mm
Four refinement regions are created with different levels of refinement as shown in
figure below
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Refinement Regions
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Meshing started with 12 cores, 32GB RAM machine.
snappyHexMesh completed meshing within 10 minutes by generating ~4.7 million
cells.
OpenFoam mesh quality criteria is cleared and grid points are transformed to m.
Mesh renumbering is done to reduce band with. This will lead to faster calculation.
Numerical Solver Attributes
For velocity Gauss linearUpwindV scheme is used. For the rest of the variables
upwind schemes are used.
All other attributes are kept with default value of Visual CFD.
Automatic switching of first order schemes to second order is used. Switching is
done after 200 iterations.
First order schemes are numerically stable but less accurate. Second order schemes
are numerically unstable but more accurate. Hence first 200 iterations are run with
first order and switched to second order schemes.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Numerical Solver attributes
Force Coefficients Calculation
Force coefficients are calculated by formula
Cd = 2Fd/(rho*A*U2
), where Fd is Drag force and Cd is drag coefficient
Cl= 2Fl/(rho*A*U2
), where Fl is Lift force and Cl is lift coefficient
A is projected area along flow direction.
Force Coefficients inputs
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Simulation
Flow is initialized using potentialFlow solution. This is done by executing
potentialFoam solver.
simpleFoam solver is run for 5000 iterations.
Results
Velocity Contour
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Velocity at x=1.244 m (behind slant)
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Pressure Contour
Total Pressure Coefficient (Cp) distribution in flow field
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Pressure Contour at x=1.244 m (behind slant)
Pressure Coefficient distribution at x=1.244m (behind slant)
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Pressure Distribution on Surfaces
Pressure Coefficient Cp distribution on surfaces.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
Cp = 1 indicates point of stagnation pressure
Cp = 0 indicates that pressure at a point is same as free stream pressure
Cp <1 indicates negative pressure or vacuum
Drag Coefficient (Cd)
Average Drag Coefficient value of last 500 iterations is 0.309.
Experimental Cd value = 0.300.
3% variation is found between experimental Cd and simulation Cd.
Drag Forces
Total force acting on geometry = 34.94 N
Drag Force due to Pressure forces = 29.41 N
Drag Force due to Viscous forces = 5.53 N
From above values is it estimated that approximately 84.17% of total drag forces are
contributed by Pressure Forces and 15.83% of total drag forces are contributed by
Viscous Forces.
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
References
 https://www.learncax.com/knowledge-base/blog/by-category/cfd/basics-of-
y-plus-boundary-layer-and-wall-function-in-turbulent-flows
 http://www.iosrjournals.org/iosr-jmce/papers/vol12-issue4/Version-
3/M012438794.pdf
 http://www.computationalfluiddynamics.com.au/tag/wall-functions/
 http://www.engr.uconn.edu/~wchiu/ME3250FluidDynamicsI/lecture%20note
s/ch09.pdf
 http://www.cfd-online.com/Tools/yplus.php
 http://www.cfd-online.com/Wiki/Y_plus_wall_distance_estimation
 https://en.wikipedia.org/wiki/Boundary_layer_thickness
 https://www.simscale.com/docs/content/validation/AhmedBody/AhmedBody.
html#id7
 CFD Simulation of Flow around External Vehicle: Ahmed Body Saurabh
Banga1, Md. Zunaid2*, Naushad Ahmad Ansari3, Sagar Sharma4, Rohit Singh
Dungriyal5
Pressure and Viscous force contribution on Total Drag
Pressure forces
Viscous Forces
Srinivas Nag H.V QA &Central Support - CFD June16th, 2016
 https://en.wikipedia.org/wiki/Turbulence_kinetic_energy
 http://www.cd-
adapco.com/sites/default/files/conference_proceeding/pdf/Ahmed%20Body-
50thAIAA.pdf
 http://www.ijettjournal.org/volume-18/number-7/IJETT-V18P262.pdf
 ERCOFTAC - Ahmed Body experimental values
 http://cfd.mace.manchester.ac.uk/cgi-
bin/cfddb/prpage.cgi?82&EXP&database/cases/case82/Case_data&database/
cases/case82&cas82_head.html&cas82_desc.html&cas82_meth.html&cas82_
data.html&cas82_refs.html&cas82_rsol.html&1&0&0&0&0
 http://cfd.mace.manchester.ac.uk/cgi-
bin/cfddb/prpage.cgi?82&EXP&database/cases/case82/Case_data&database/
cases/case82&cas82_head.html&cas82_desc.html&cas82_meth.html&cas82_
data.html&cas82_refs.html&cas82_rsol.html&1&1&1&1&0&unknown
 http://user.engineering.uiowa.edu/~me_160/lab/cfdefdahmed.pdf
 http://www.taoxing.net/web_documents/cfd_lab4.pdf
 https://www.researchgate.net/publication/282272911_OpenFOAM_step_by_
step_tutorial
 http://cfd.mace.manchester.ac.uk/twiki/pub/Main/TimCraftNotes_All_Access/
advtm-wallfns.pdf
 http://www.cfd-online.com/Wiki/Y_plus_wall_distance_estimation

More Related Content

What's hot

Vortex lattice implementation of propeller sections for OpenFoam 2.3x
Vortex lattice implementation of propeller sections for OpenFoam 2.3xVortex lattice implementation of propeller sections for OpenFoam 2.3x
Vortex lattice implementation of propeller sections for OpenFoam 2.3xSuryakiran Peravali
 
Cfx12 12 moving_zones
Cfx12 12 moving_zonesCfx12 12 moving_zones
Cfx12 12 moving_zonesMarcushuynh66
 
Airfoil Analysis(NACA 0012 ) Ansys Fluent
Airfoil Analysis(NACA 0012 ) Ansys FluentAirfoil Analysis(NACA 0012 ) Ansys Fluent
Airfoil Analysis(NACA 0012 ) Ansys Fluentshivam choubey
 
CFD for Rotating Machinery using OpenFOAM
CFD for Rotating Machinery using OpenFOAMCFD for Rotating Machinery using OpenFOAM
CFD for Rotating Machinery using OpenFOAMFumiya Nozaki
 
Aircraft design initial_sizing_2
Aircraft design initial_sizing_2Aircraft design initial_sizing_2
Aircraft design initial_sizing_2Roopam Choudhury
 
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)Malik Abdul Wahab
 
AERODYNAMICS FORCES AND MOMENTS.ppt
AERODYNAMICS FORCES AND MOMENTS.pptAERODYNAMICS FORCES AND MOMENTS.ppt
AERODYNAMICS FORCES AND MOMENTS.ppttauraimamire
 
Q923+rrl+l04
Q923+rrl+l04Q923+rrl+l04
Q923+rrl+l04AFATous
 
boundarylayertheory.pptx
boundarylayertheory.pptxboundarylayertheory.pptx
boundarylayertheory.pptxreenarana28
 
Subsonic and supersonic air intakes
Subsonic and supersonic air intakesSubsonic and supersonic air intakes
Subsonic and supersonic air intakesSanjay Singh
 
Proulsion I - SOLVED QUESTION BANK - RAMJET ENGINE
Proulsion  I - SOLVED QUESTION BANK - RAMJET ENGINEProulsion  I - SOLVED QUESTION BANK - RAMJET ENGINE
Proulsion I - SOLVED QUESTION BANK - RAMJET ENGINESanjay Singh
 

What's hot (20)

Multiphase models
Multiphase models Multiphase models
Multiphase models
 
Vortex lattice implementation of propeller sections for OpenFoam 2.3x
Vortex lattice implementation of propeller sections for OpenFoam 2.3xVortex lattice implementation of propeller sections for OpenFoam 2.3x
Vortex lattice implementation of propeller sections for OpenFoam 2.3x
 
ME438 Aerodynamics (week 8)
ME438 Aerodynamics (week 8)ME438 Aerodynamics (week 8)
ME438 Aerodynamics (week 8)
 
Computational Fluid Dynamics
Computational Fluid DynamicsComputational Fluid Dynamics
Computational Fluid Dynamics
 
Gas permeater
Gas permeaterGas permeater
Gas permeater
 
Cfx12 12 moving_zones
Cfx12 12 moving_zonesCfx12 12 moving_zones
Cfx12 12 moving_zones
 
Airfoil Analysis(NACA 0012 ) Ansys Fluent
Airfoil Analysis(NACA 0012 ) Ansys FluentAirfoil Analysis(NACA 0012 ) Ansys Fluent
Airfoil Analysis(NACA 0012 ) Ansys Fluent
 
CFD for Rotating Machinery using OpenFOAM
CFD for Rotating Machinery using OpenFOAMCFD for Rotating Machinery using OpenFOAM
CFD for Rotating Machinery using OpenFOAM
 
Aircraft design initial_sizing_2
Aircraft design initial_sizing_2Aircraft design initial_sizing_2
Aircraft design initial_sizing_2
 
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)
WHAT IS COMPUTATIONAL FLUID DYNAMICS (CFD)
 
Tcas
TcasTcas
Tcas
 
6 heat transfer modeling
6 heat transfer modeling6 heat transfer modeling
6 heat transfer modeling
 
AERODYNAMICS FORCES AND MOMENTS.ppt
AERODYNAMICS FORCES AND MOMENTS.pptAERODYNAMICS FORCES AND MOMENTS.ppt
AERODYNAMICS FORCES AND MOMENTS.ppt
 
Q923+rrl+l04
Q923+rrl+l04Q923+rrl+l04
Q923+rrl+l04
 
boundarylayertheory.pptx
boundarylayertheory.pptxboundarylayertheory.pptx
boundarylayertheory.pptx
 
Air Plane Flap Mechanism
Air Plane Flap MechanismAir Plane Flap Mechanism
Air Plane Flap Mechanism
 
Subsonic and supersonic air intakes
Subsonic and supersonic air intakesSubsonic and supersonic air intakes
Subsonic and supersonic air intakes
 
Wind Tunnel Ex
Wind Tunnel ExWind Tunnel Ex
Wind Tunnel Ex
 
Proulsion I - SOLVED QUESTION BANK - RAMJET ENGINE
Proulsion  I - SOLVED QUESTION BANK - RAMJET ENGINEProulsion  I - SOLVED QUESTION BANK - RAMJET ENGINE
Proulsion I - SOLVED QUESTION BANK - RAMJET ENGINE
 
Flying car ppt.
Flying car ppt.Flying car ppt.
Flying car ppt.
 

Viewers also liked

Basic Boundary Conditions in OpenFOAM v2.4
Basic Boundary Conditions in OpenFOAM v2.4Basic Boundary Conditions in OpenFOAM v2.4
Basic Boundary Conditions in OpenFOAM v2.4Fumiya Nozaki
 
Adjoint Shape Optimization using OpenFOAM
Adjoint Shape Optimization using OpenFOAMAdjoint Shape Optimization using OpenFOAM
Adjoint Shape Optimization using OpenFOAMFumiya Nozaki
 
OpenFOAM Programming Tips
OpenFOAM Programming TipsOpenFOAM Programming Tips
OpenFOAM Programming TipsFumiya Nozaki
 
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみた
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみたオープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみた
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみたFumiya Nozaki
 
OpenFOAM for beginners: Hands-on training
OpenFOAM for beginners: Hands-on trainingOpenFOAM for beginners: Hands-on training
OpenFOAM for beginners: Hands-on trainingJibran Haider
 
OpenFOAMの壁関数
OpenFOAMの壁関数OpenFOAMの壁関数
OpenFOAMの壁関数Fumiya Nozaki
 
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-Fumiya Nozaki
 
Spatial Interpolation Schemes in OpenFOAM
Spatial Interpolation Schemes in OpenFOAMSpatial Interpolation Schemes in OpenFOAM
Spatial Interpolation Schemes in OpenFOAMFumiya Nozaki
 
Boundary Conditions in OpenFOAM
Boundary Conditions in OpenFOAMBoundary Conditions in OpenFOAM
Boundary Conditions in OpenFOAMFumiya Nozaki
 
Dynamic Mesh in OpenFOAM
Dynamic Mesh in OpenFOAMDynamic Mesh in OpenFOAM
Dynamic Mesh in OpenFOAMFumiya Nozaki
 

Viewers also liked (11)

Basic Boundary Conditions in OpenFOAM v2.4
Basic Boundary Conditions in OpenFOAM v2.4Basic Boundary Conditions in OpenFOAM v2.4
Basic Boundary Conditions in OpenFOAM v2.4
 
Verteidigung
VerteidigungVerteidigung
Verteidigung
 
Adjoint Shape Optimization using OpenFOAM
Adjoint Shape Optimization using OpenFOAMAdjoint Shape Optimization using OpenFOAM
Adjoint Shape Optimization using OpenFOAM
 
OpenFOAM Programming Tips
OpenFOAM Programming TipsOpenFOAM Programming Tips
OpenFOAM Programming Tips
 
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみた
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみたオープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみた
オープンソースの CFD ソフトウェア SU2 のチュートリアルをやってみた
 
OpenFOAM for beginners: Hands-on training
OpenFOAM for beginners: Hands-on trainingOpenFOAM for beginners: Hands-on training
OpenFOAM for beginners: Hands-on training
 
OpenFOAMの壁関数
OpenFOAMの壁関数OpenFOAMの壁関数
OpenFOAMの壁関数
 
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-
OpenFOAM -空間の離散化と係数行列の取り扱い(Spatial Discretization and Coefficient Matrix)-
 
Spatial Interpolation Schemes in OpenFOAM
Spatial Interpolation Schemes in OpenFOAMSpatial Interpolation Schemes in OpenFOAM
Spatial Interpolation Schemes in OpenFOAM
 
Boundary Conditions in OpenFOAM
Boundary Conditions in OpenFOAMBoundary Conditions in OpenFOAM
Boundary Conditions in OpenFOAM
 
Dynamic Mesh in OpenFOAM
Dynamic Mesh in OpenFOAMDynamic Mesh in OpenFOAM
Dynamic Mesh in OpenFOAM
 

Similar to OpenFoam Simulation of Flow over Ahmed Body using Visual CFD software

Cdd mahesh dasar ijertv2 is120775
Cdd mahesh dasar ijertv2 is120775Cdd mahesh dasar ijertv2 is120775
Cdd mahesh dasar ijertv2 is120775Mahesh Dasar
 
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...Abhishek Jain
 
788072013031501802412
788072013031501802412788072013031501802412
788072013031501802412SOE
 
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...IAEME Publication
 
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSOR
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSORNUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSOR
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSORIAEME Publication
 
Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Safdar Ali
 
Determination of shock losses and pressure losses in ug mine openings
Determination of shock losses and pressure losses in ug mine openingsDetermination of shock losses and pressure losses in ug mine openings
Determination of shock losses and pressure losses in ug mine openingsSafdar Ali
 
ENG687 Aerodynamics.docx
ENG687 Aerodynamics.docxENG687 Aerodynamics.docx
ENG687 Aerodynamics.docx4934bk
 
CFD Final Report-2
CFD Final Report-2CFD Final Report-2
CFD Final Report-2Dwight Nava
 
Final course project report
Final course project reportFinal course project report
Final course project reportKaggwa Abdul
 
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCSCJournals
 
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...Abhishek Jain
 
IJREI- Analysis of Vortex Formation around a Circular Cylinder at low Reynol...
IJREI-  Analysis of Vortex Formation around a Circular Cylinder at low Reynol...IJREI-  Analysis of Vortex Formation around a Circular Cylinder at low Reynol...
IJREI- Analysis of Vortex Formation around a Circular Cylinder at low Reynol...Star Web Maker Services Pvt. Ltd.
 
Validation of dynamic relaxation (dr) method in rectangular laminates using l...
Validation of dynamic relaxation (dr) method in rectangular laminates using l...Validation of dynamic relaxation (dr) method in rectangular laminates using l...
Validation of dynamic relaxation (dr) method in rectangular laminates using l...Osama Mohammed Elmardi Suleiman
 

Similar to OpenFoam Simulation of Flow over Ahmed Body using Visual CFD software (20)

Cdd mahesh dasar ijertv2 is120775
Cdd mahesh dasar ijertv2 is120775Cdd mahesh dasar ijertv2 is120775
Cdd mahesh dasar ijertv2 is120775
 
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...
Simulations Of Unsteady Flow Around A Generic Pickup Truck Using Reynolds Ave...
 
788072013031501802412
788072013031501802412788072013031501802412
788072013031501802412
 
ASSIGNMENT
ASSIGNMENTASSIGNMENT
ASSIGNMENT
 
I1304015865
I1304015865I1304015865
I1304015865
 
Fluid Mechanics (2).pdf
Fluid Mechanics  (2).pdfFluid Mechanics  (2).pdf
Fluid Mechanics (2).pdf
 
Example_Aerodynamics
Example_AerodynamicsExample_Aerodynamics
Example_Aerodynamics
 
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...
Ijmet 08 02_029NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL ...
 
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSOR
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSORNUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSOR
NUMERICAL SOLUTIONS FOR PERFORMANCE PREDICTION OF CENTRIFUGAL COMPRESSOR
 
Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)Determination of shock losses and pressure losses in ug mine openings (1)
Determination of shock losses and pressure losses in ug mine openings (1)
 
Determination of shock losses and pressure losses in ug mine openings
Determination of shock losses and pressure losses in ug mine openingsDetermination of shock losses and pressure losses in ug mine openings
Determination of shock losses and pressure losses in ug mine openings
 
ENG687 Aerodynamics.docx
ENG687 Aerodynamics.docxENG687 Aerodynamics.docx
ENG687 Aerodynamics.docx
 
cfd ahmed body
cfd ahmed bodycfd ahmed body
cfd ahmed body
 
CFD Final Report-2
CFD Final Report-2CFD Final Report-2
CFD Final Report-2
 
Final course project report
Final course project reportFinal course project report
Final course project report
 
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion FlowsCFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
CFD and Artificial Neural Networks Analysis of Plane Sudden Expansion Flows
 
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...
AIROPT: A Multi-Objective Evolutionary Algorithm based Aerodynamic Shape Opti...
 
Cfd 0
Cfd 0Cfd 0
Cfd 0
 
IJREI- Analysis of Vortex Formation around a Circular Cylinder at low Reynol...
IJREI-  Analysis of Vortex Formation around a Circular Cylinder at low Reynol...IJREI-  Analysis of Vortex Formation around a Circular Cylinder at low Reynol...
IJREI- Analysis of Vortex Formation around a Circular Cylinder at low Reynol...
 
Validation of dynamic relaxation (dr) method in rectangular laminates using l...
Validation of dynamic relaxation (dr) method in rectangular laminates using l...Validation of dynamic relaxation (dr) method in rectangular laminates using l...
Validation of dynamic relaxation (dr) method in rectangular laminates using l...
 

OpenFoam Simulation of Flow over Ahmed Body using Visual CFD software

  • 1. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Simulation of Flow over Ahmed Body using OpenFoam - Visual CFD software Introduction The aim of this study is to validate the Drag Coefficient of steady-state incompressible turbulent flow around the Ahmed Body The aerodynamic behavior of the Ahmed body with slant angle 250 is investigated numerically. The Reynolds number Re of the flow is 2.8*106 The open source CFD tool OpenFoam 2.3.1 is tested for its ability to reproduce the aerodynamic drag coefficient of the body. External aero case setup is done using ESI’s software Visual-CFD 12.0 Drag coefficient is compared with the experimental results from literature. Geometry The generic Ahmed Body reference model has been chosen as the benchmark for carrying out computations for studying of the aerodynamic parameters. The body was first proposed by Ahmed et al., (1984).The Ahmed body is a very simple bluff body which has its shape simple enough to allow for accurate flow simulation but retains some important practical features relevant to automobile bodies. It has a slant on its rear end, whose angle can be manipulated and the corresponding drag and lift coefficients calculated.
  • 2. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Geometry of Ahmed Body Wind Tunnel STL format of 3D CAD model of Ahmed Body geometry with 250 slant angle is used for the analysis. Geometry is placed in wind tunnel of dimensions (15mX1.4mX1.87m) with respect to X, Y and Z directions respectively. Front space length is kept equal to 3 times the length of geometry and rear space length is kept 6 times length of geometry. Wind tunnel has 6 faces namely XMin, XMax, YMin, YMax, ZMin and ZMax. Geometry is located at ground YMin. Geometry is mounted on 4 stilts. Projected area of geometry along positive X direction including stilts is 0.115 m2
  • 3. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Wind Tunnel of dimensions (15mX1.4mX1.87m) Flow Physics Fluid Properties: Fluid is Air Density of the fluid rho = 1.225 kg/m3 Dynamic Viscosity of fluid µ = 1.84*10-5 Ns/m2 Kinematic Viscosity = Dynamic Viscosity/Density = 1.502*10-5 m2 /s Reynolds number of the flow Re = U*L/ = 2.8*106
  • 4. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Boundary Conditions: Inlet (XMin): Fluid Velocity, U = 40 m/s Outlet (XMax): No external pressure applied with zeroGradient Velocity Wall: Geometry Surfaces and Ground (YMin) Symmetry: ZMin, ZMax and YMax Time dependence: Steady State analysis. Turbulence Modelling Turbulence quantities can be calculated by following formula Turbulent Kinetic Energy k = 1.5(UI) 2 I is turbulent intensity in percentage U is free stream velocity Energy Dissipation omega= k0.5 / (Cu 0.25 *l) Where Cu is model constant = 0.09 l = length scale which can be estimated as 0.07L. L is characteristic length Turbulence quantities used for study are mentioned below k = 0.287 m2 /s2 , omega = 0.215 s-1 Turbulence model used is kOmegaSST Spalding Wall functions (nutUSpaldingWallFunction in OpenFoam) is used on Walls. Y-plus, First cell height and Boundary layers The near wall region is meshed using the calculated first cell height value with gradual growth in the mesh so that the viscous effects are captured and avoiding overall heavy mesh count.
  • 5. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Yplus value should be in range 30-300 when Reynolds Average Stress turbulence (RAS) models are used. There are various Yplus online calculators available. We have used the one from CFD Online Mesh definition in Visual CFD YPlus of 50 was chosen for this study and obtained first cell height (FCH) of 0.478 mm (~0.5mm). This is minimum cell size to be created near walls to accurately capture viscous effects. This given initial guess for user about the smallest cell size to be created in computational domain to fairly capture the effects of fluid flow.
  • 6. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Boundary layer thickness can be calculated from below formula δ = x*0.382/Rex 0.2 , where x is the distance in downstream where turbulent boundary layer starts. Transition to turbulence will be at Re = 10*105 . We have taken total length of the geometry L = 1.044m and calculated total boundary layer thickness equal to 15mm. So, in order to capture turbulent flow accurately, FCH should be within δ=15mm. Meshing Base cell size (bsc) is set to 100mm. ‘blockMesh’ utility of OpenFOAM will create a structured hexahedral grid of 100 mm (bsc) throughout wind tunnel. Output of blockMesh is input to ‘snappyHexMesh’ utility. This creates unstructured polyhedral meshes. snappyHexMesh works in 3 stages. 1. Snapping: In this stage, fluid mesh is attached to geometry surfaces. 2. Castellation: In this stage, grid refinement occurs. 3. Layer addition: Snapped and Castellated mesh will be projected outwards from geometry and boundary layers are created near walls. Total drag force is the summation of Pressure force and Viscous force. To capture drag due to viscous forces, we have to resolve by creating fine meshes and boundary layers near walls. To capture drag due to pressure forces, we have to refine fluid cells in front and rear part of the geometry. This is done by creating refinement regions Boundary layers creation Surface mesh size on walls are set to 3.125mm. FCH in OpenFOAM is based on surface mesh size. With relative mesh size on, FCH is set to 0.08. This means the first cell height will be equal to 0.08*3.125 = 0.25mm. Final layer thickness is 1.85mm 12 boundary layers are created with expansion ratio of 1.2. Total boundary thickness is calculated from geometry progression and equal to 9.89mm. This covers around 66% of total boundary layer thickness. This should be sufficient to capture near wall viscous effects. Another important parameter in creating boundary layers correctly is final layer ratio which is equal to final layer thickness/surface cell size. This ratio is equal to
  • 7. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 0.592 in this case. For proper layers to be created, this ratio should be within range of 0.2 to 0.6. Boundary layers are created as shown below Boundary layers generated from snappyHexMesh Refinement Regions Cell sizes at a given refinement level ‘n’ is obtained from following equation written below CellSize@nth level = bsc/2n Say n = 4, then cell size will be equal to 100/24 = 6.25mm Four refinement regions are created with different levels of refinement as shown in figure below
  • 8. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Refinement Regions
  • 9. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Meshing started with 12 cores, 32GB RAM machine. snappyHexMesh completed meshing within 10 minutes by generating ~4.7 million cells. OpenFoam mesh quality criteria is cleared and grid points are transformed to m. Mesh renumbering is done to reduce band with. This will lead to faster calculation. Numerical Solver Attributes For velocity Gauss linearUpwindV scheme is used. For the rest of the variables upwind schemes are used. All other attributes are kept with default value of Visual CFD. Automatic switching of first order schemes to second order is used. Switching is done after 200 iterations. First order schemes are numerically stable but less accurate. Second order schemes are numerically unstable but more accurate. Hence first 200 iterations are run with first order and switched to second order schemes.
  • 10. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Numerical Solver attributes Force Coefficients Calculation Force coefficients are calculated by formula Cd = 2Fd/(rho*A*U2 ), where Fd is Drag force and Cd is drag coefficient Cl= 2Fl/(rho*A*U2 ), where Fl is Lift force and Cl is lift coefficient A is projected area along flow direction. Force Coefficients inputs
  • 11. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Simulation Flow is initialized using potentialFlow solution. This is done by executing potentialFoam solver. simpleFoam solver is run for 5000 iterations. Results Velocity Contour
  • 12. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Velocity at x=1.244 m (behind slant)
  • 13. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Pressure Contour Total Pressure Coefficient (Cp) distribution in flow field
  • 14. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Pressure Contour at x=1.244 m (behind slant) Pressure Coefficient distribution at x=1.244m (behind slant)
  • 15. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Pressure Distribution on Surfaces Pressure Coefficient Cp distribution on surfaces.
  • 16. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 Cp = 1 indicates point of stagnation pressure Cp = 0 indicates that pressure at a point is same as free stream pressure Cp <1 indicates negative pressure or vacuum Drag Coefficient (Cd) Average Drag Coefficient value of last 500 iterations is 0.309. Experimental Cd value = 0.300. 3% variation is found between experimental Cd and simulation Cd. Drag Forces Total force acting on geometry = 34.94 N Drag Force due to Pressure forces = 29.41 N Drag Force due to Viscous forces = 5.53 N From above values is it estimated that approximately 84.17% of total drag forces are contributed by Pressure Forces and 15.83% of total drag forces are contributed by Viscous Forces.
  • 17. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016 References  https://www.learncax.com/knowledge-base/blog/by-category/cfd/basics-of- y-plus-boundary-layer-and-wall-function-in-turbulent-flows  http://www.iosrjournals.org/iosr-jmce/papers/vol12-issue4/Version- 3/M012438794.pdf  http://www.computationalfluiddynamics.com.au/tag/wall-functions/  http://www.engr.uconn.edu/~wchiu/ME3250FluidDynamicsI/lecture%20note s/ch09.pdf  http://www.cfd-online.com/Tools/yplus.php  http://www.cfd-online.com/Wiki/Y_plus_wall_distance_estimation  https://en.wikipedia.org/wiki/Boundary_layer_thickness  https://www.simscale.com/docs/content/validation/AhmedBody/AhmedBody. html#id7  CFD Simulation of Flow around External Vehicle: Ahmed Body Saurabh Banga1, Md. Zunaid2*, Naushad Ahmad Ansari3, Sagar Sharma4, Rohit Singh Dungriyal5 Pressure and Viscous force contribution on Total Drag Pressure forces Viscous Forces
  • 18. Srinivas Nag H.V QA &Central Support - CFD June16th, 2016  https://en.wikipedia.org/wiki/Turbulence_kinetic_energy  http://www.cd- adapco.com/sites/default/files/conference_proceeding/pdf/Ahmed%20Body- 50thAIAA.pdf  http://www.ijettjournal.org/volume-18/number-7/IJETT-V18P262.pdf  ERCOFTAC - Ahmed Body experimental values  http://cfd.mace.manchester.ac.uk/cgi- bin/cfddb/prpage.cgi?82&EXP&database/cases/case82/Case_data&database/ cases/case82&cas82_head.html&cas82_desc.html&cas82_meth.html&cas82_ data.html&cas82_refs.html&cas82_rsol.html&1&0&0&0&0  http://cfd.mace.manchester.ac.uk/cgi- bin/cfddb/prpage.cgi?82&EXP&database/cases/case82/Case_data&database/ cases/case82&cas82_head.html&cas82_desc.html&cas82_meth.html&cas82_ data.html&cas82_refs.html&cas82_rsol.html&1&1&1&1&0&unknown  http://user.engineering.uiowa.edu/~me_160/lab/cfdefdahmed.pdf  http://www.taoxing.net/web_documents/cfd_lab4.pdf  https://www.researchgate.net/publication/282272911_OpenFOAM_step_by_ step_tutorial  http://cfd.mace.manchester.ac.uk/twiki/pub/Main/TimCraftNotes_All_Access/ advtm-wallfns.pdf  http://www.cfd-online.com/Wiki/Y_plus_wall_distance_estimation