Week 3 - External flow simulation over an Ahmed body.
Aim -
To perform external flow simulation over an Ahmed body.
Objective -
* Describe Ahmed's body and its importance.
* Explain the reason for the negative pressure in the wake region and show the vector plot clearly showing the wake region.
* Explain the significance of the point of separation.
* Show velocity and pressure contours & the drag coefficient plot for a refined case.
* Perform the grid independency test and provide the values of drag and lift with each case.
Introduction -
*In fluid mechanics, external flow is a flow in which boundary layers develop freely, without constraints imposed by adjacent surfaces. It can be defined as the flow of a fluid around a body that is completely submerged in it.
*In comparison to internal flow, entrance flows and external flows feature highly viscous effects confined to rapidly growing “boundary layers” in the entrance region, or to thin shear layers along the solid surface
* External flows in general can be classified as flows over immersed bodies where flow features(such as boundary layers)arond the body can develop freely without constraints of adjacent surfaces :
- Airflow over aircraft and ground vehicles
- Water flow over a submersible vessel
- Flying footballs,golf balls and baseballs
* One of the most important areas of interest in studying external flows are,fluid forces acting on the body,as they define dynamics of an object travelling through the fluid.
*Unlike internal flows which could be solved analytically for the entire range of laminar Re,analytical solutions to flows over even simple shapes are only possible for very low reynolds number Re~1,which are of little interest in practical applications.
*Even at modest laminar regime rgions Re~10,external flows starts developing separation regions and wakes which can not be described analytically.
*An external flow is,indeed.a challenging problem even in present day fluid dynamics.
*In external flow problems,the flow either moves over a stationary body(e.g.a wind tunnel experiment) or a body moves ia a quiescent fluid(e.g.a flying airplane).
* In fluid dynamics it is common to describe the flowin the reference frame fixed to the body,i.e. fluid is moving over a stationary body.
*Upstream conditions(velocity,pressure,density)are normally used as inputs to characterize the flow upsteam of the body at a location where is the flow is not affected by the body's presence.In most cases constant upstream conditions are used.
*The vast majority of practical exterrnal flows are turbulent, in a sense that the flow is turbulent in a part of the domain around the flow.
* As an object travels through the fluid,it's dynamics are affected by pressure and viscous forces.
* Hence,for external flow analysis,our primary objectives are prediction of fluid forces actiong on the object and understanding the flow physics defining these forces.
Ahmed's Body And It's Importance -
Ahmed body is a simplified car body used to study the impact of the flow pattern on the drag.It is representative of standard model of passenger car.The external aerodynamics of the car defines many major traits of an automobile like ,stability and fuel consumption. The Ahmed body,described originally by S.A.Ahmed in 1984 is a simplified car made of round front part,movable Z slant plane in the rear end to study the flow separation at different angles and a rectanular box which link the front and rear ends.
Ahmed body is a benchmark for aerodynamic simulation in the automotive industry.It's shape is simple enough to allow for accurate flow simulation but retains some important practical features.In the experiment,3 main features were seen in it's wake :
* recirculation region is formed as the flow deparates at the top of the vertical back surface of the model
* recirculation region is formed due to the separation at the base of the model.
* pillar vortices form as the vorticity in the boundary layers on the sides roll up over slant edges.
THe wake is dependent on the slant angle.When the slant angle is less than 12deg,the flow remains attached over the slant.In other words, the flow is 2D and has low drag Between 12 deg and 30 deg th eflow becomes much more 3D as C-pillar vortices form.These reach maximum strength at 30 deg.The drag increases significantly as the low pressure cores act on the rear surfaces,Beyond 30 deg, the flow separates full off the slant.The results in a sudden decrease in drag and weaker C-pillar vortices.
The aim of this project is to develop,refine,and validate the latest generation of turbulence models for selected examples encountered in vehicle aerodynamics. The validation of turbulence models requires the availablity of detailed experimental data.This is also used in validating CFD codes.If you have tour code, before trusting it oe validating your code you need to make sure that the results are comparable with the experiment data of Ahmed body.If it matches then we can trust our code and use the code to teest other geometries.This is research nodel which was built in real life and lot of experimental analysis has been done on it. So it can be useful in validating CFD codes.
Solution Procedure -
For solving the exteral flow over the ahmed body we will follow the below procedure :-
Geometry Creation --> Meshing --> Setup --> Solution & Post Processing
Geometry Creation -
* Launch the Ansys workbench.First drag and drop the Fluid Flow(Fluent)model into project schematic and double click on geometry to launch the SpaceClaim.
* Import the geometry in to the ansys spaceclaim.
*As the body is perfectly symmetric, we can run the simulation by considering the only half body. This is the best practice where you can save on the number of cells and get the results faster as well.
* We can use the split body command,which is unnder design,to split the geometry into two parts and delete the other part.
* Now since,this the external flow problem, we want to simulate the flow over the Ahmed body and so we need flow outside of the Ahmed body and not inside it.
*First we need to create an enclosure covering the entire geometry by enclosure command.
*To create enclosure,select geometry -->under prepare --> select enclosure,then give the dimensions to the enclosure as shown in the below figure & hit ok.Make sure to turn off the symmetric dimension.
*Also,since we want to observe the wake around the body,we need to create another small encloure around the Ahmed body to capture the wake region.Follow the same producedure to create the enclosure as mentioned above with different dimensions.
*Need to suppress the Ahmed body for physics,to make sure that there is no mesh generation inside it,as we only need to simulate the external flow.This reduces the number of elements created.
*Now if we directly go to meshing we will get interference error and the mesh from one enclosure will get mixed up with other enclosure.But we want separate mesh for each enclosure and only want proper mesh connectivity at the enclosure boundary.
*To resolve in SpaceClaim click pn interference.This will highlight the interference area ,then click ok to resolve it.
*Now if we cut the geometry ,we can see different hashing pattern for each enclosure and the Ahmed bod.Now close the SpaceClaim.
Meshing -
*In project schematic double click on mesh to open ANSYS meshing.
*First provide the named selection,which will be use by fluent to as boundary names to assign proper boundary conditions.
*Select face selection tool,click on the front face of the outer enclosure,press N,give name as inlet.Simillarly define outlet.
*Select all side walls and name them symmetry.Select ahmed body and name it carwall.
*First generate the basic mesh.After we will look at the regions where,we want to refine the mesh.
Mesh Refinement -
Outer Enclosure -
* We can see that,outside the inner region there is a perfect structure made of straight lines i.e.,no complex shapes and is in 3D, made up of a box.In such scenarios it's better to use hexahederal mesh.Hexahederal mesh has the highest quality of all mesh types.
* Clock right click on mesh => insert => method => select outermost body for geometry => apply.For method =>multizone.Whenever we use multizone,it creates hexa meshes where ever possible and the regions where there are different types of meshes,it's goingto have perfect connectivity.
*For main global mesh,give size 100 mm & maximum size as 100 mm,so as to have evenly sized meshes in the outer region.
*Generate mesh.We will get nice boxes of hexahederal mesh,wich nicely connects with inner tetrahedral meshes.
Inner Enclosure -
*To make finer mesh for inner enclosure, click mesh => sizing => for geometry select inner enclosure & give size 40mm.
*Generate mesh.We will getrefined mesh for inner enclosure.
Ahmed Body -
Body Sizing
*Right click mesh => sizing => for geometry select ahmed body & give size 20 mm.
*Generate mesh.
Edge Sizing
*Now ,if we observe the ahmed body,we can se that the cylinderical pillers are approxiamted as polygons,because element size is quite big over there.
*To fix it ,will select only those faces and give size of 5mm. Generate mesh.This will give us nice looking mesh for every part of the Ahmed body.
Inflation
*In this project flow around Ahmed body is critical for observation.So we need refinement near the walls of the Ahmed body.We can achive this by using inflation.Iflation helps us to create body fitted meshes,which capture flow around the conserned body effectively.
*Right click mesh => sizing => in geometry select small enclosure and for boundary select ahmed body boundary layer.
*For inflation option we will use total tickness and we give this based on y+ value and the turbulence model we use.Here we use k-epsilon turbulence model,hence y+ should be in between 30 to 300.
Total Thickness -
1) `U_infty` = freestream velocity = 25 m/s
2)`rho` = freestream density = 1.225 `(kg)/m^3`
3) `mu` = dynamic viscosity = 0.000017894 `(kg)/(ms)`
4) L = length of Ahmed body (m)
5) desired y+ = 100
Reynolds number = `Re (rho*U_infty*L)/mu`
= `(1.225*251.044)/0.000017894`
=1786772.1023806867
Skin friction coefficient =`C_f = 0.026/R_e^(1/7)`
= `0.026/(1786772.1023806867)^(1/7)`
= 0.00332522173
Wall shear stress = Tau_wall = `(C_f*rho*U_infty^2)/2`
= `(0.00332522173*1.225*(25)^2)/2`
= 1.27293644352
Friction velocity = `U_(f) = (tau_(wall)/rho)^(1/2)`
= `(1.27293644352/1.225)^(1/2)`
= 1.01937813918
Hence,
First layer thickness, Deltas = `(y+*mu)/(U_f*rho)`
=`(100*0.000017894/( 1.01937813918*1.225))`
= 0.001432966 m
Therefore,Total Thickness = `0.001432966*(1.2)^5`
= 0.003565m = 3.56 mm
* Insert the calculated total thickness,and maximum of 6 growth layers with growth ratio of 1.2.
* Generate mesh & will get inflation layers generated.
* Now lets check our mesh quality.Our minimum mesh quality is good enough.
* This concludes our meshing procedure.
* Now close the mesh & update.
Setup -
* Double click setup in project schematic.This will open ansys fluent.
*Click on check mesh and make sure there are no errors.
Setting up Physics
Our solution method will be SIMPLE.
General -
*Solver type - pressure based
*time - Steady state
*velocity formulation - absolute
Models -
*viscous model - k-epsilon standard
Material -
*Air
Zones -
Cell zone - In cell zone we can see our internal volume ,which is basically our mesh.Set it to fluid type.
Boundary conditions - We can see all the named selections which,we generated above being used as boundary conditions.
* Inlet -
Type - velocity inlet
velocity magnitude - 25 m/sec
* Outlet -
Type - pressure outlet
gauge pressure - 0 Pa
* carwall -
Type - wall
* symmetry -
Type -symmetry
*Now initialize the domain.We will use hybrid initialization,this provides very good initial conditions.
*We want to moniter different flow quantities as the solution is being generated,will use definitions for this.We want to see howvthe velocity and pressure variation looks over the ahmed body.
*Since the flow is going along x-axis ,we need to create plane which has it's normal in z-axis.
*click => results => create => plane => select point & normal => give point values (0,0,0) & nomal along z-axis(0,0,1) => give name as -cutplane-z
* To create pressure and velocity contour,click-postprocessing => contour => create => contour of =>velocity & under that velocity magnitude => select cutplane-z => save/display.Will get initial values of velocity,these are not the final values and will get washed up during iteration.In the same way create pressure contour.
*To create animation,go to activities => solution animation => select velocity contour => preview => set desired view => give name as velocity animation. Simillarly create animation for pressure contour plot.
*Also we need to moniter coefficient of drag and lift for Ahmed body.To create plot of drag coefficient,click => definitions => new => force report => drag => select carwall as zones => check report file & report plot => ok.
Simillarly set up coefficient of lift plot.
Solving -
* We will run the simulation for 800 iterations.We can see from the lift,drag and residual plot that our solution has converged.
Results -
Residual Plot -
*It can be observed from the residual plot that solution remain unchanged after 600 iterations.
Drag Plot -
*It can be observed that the coefficient of drag reached the steady state value after 400 iterations.
Lift Plot -
*It can be observed that the coefficient of lift reached the steady state value after 600 iterations.
Drag & Lift Value -
Velocity Contour -
*Below is the plot for velocity contour.We can clearly see the formation of wake region behind the ahmed body.
Pressure Contour -
*Below is the plot for pressure contour for Ahmed body.
Vector Plot -
*Below is the plot for vector contour.We can clearly see the formation of wake behind the ahmed body and can see the recirculating vectors in the wake region.
Boundary Layer Separation -
*In general wall bounded flows are suject to pressure variations due to surface curvature or an external forcing.Whenever there is relative movement between a fluid and a solid surface, whether externally round a body, or internally in an enclosed passage,a boundary layer exists with viscous forces present in the layer of fluid close to the surface.
*Flow separation or boundary layer separation is the detachment of a boundary layer from a surface into a wake.[1] Separation occurs in flow that is slowing down, with pressure increasing, after passing the thickest part of a streamline body or passing through a widening passage, for example.
*Flowing against an increasing pressure is known as flowing in an adverse pressure gradient.Adverse pressure gradient cause
the flow to slow down.
*Increasing the fluid pressure is akin to increasing the potential energy of the fluid, leading to a reduced kinetic energy and
a deceleration of the fluid. Since the fluid in the inner part of the boundary layer is slower, it is more greatly affected by
the increasing pressure gradient. For a large enough pressure increase, this fluid may slow to zero velocity or even become
reversed causing a flow separation
*When the boundary layer becomes separated ,the boundary layer equations are no longer valid.However we can predict the point of sepation by moniterng the velocity gradient(or shear stress) at the wall in our solution and noting where it becomes close to zero.
*THe separation point is defined as a location between forward and inverse flow where the wall shear stress is zero.
*The thickness of the boundary layer abruptly increases at the separation point,the layer is forced off the surface by reverse
flow near the wall.
*Detached flow takes the form of verticle structures,which can be laminar of turbulent depending on the flow regimes.
Significance of the point of separation -
*So at the separation point the air stops "sticking" to an object that is moving through the air.
*In our study,we can clearly see that at sharp corners and turns the flow naturally separates,as can be easily understood
from the conservation of momentum.
*This effect is same as flow in a backward step problem.
*At the corner boundary layer maintains it's momentum in the direction of flow,and simply can not stay attached in the absence of external pressure gradient forcing it to turn around the corner.As the flow tends to go straight,then due to this,it forms a low pressure region at that point and back of the ahmed body.Then this low pressure sucks the flow which is going straight and forms a recirculation zone.
*This leads to wake formation behind the ahmed body,which is evident from velocity contour.
*In prticular formation of weak zone of disturbed fluid on the down stream,in which pressure is approximately constant and much less than that on the upstream,gives rise to boundary forces.Which in turn causes more resistance.
Reason for negative pressure in the wake region -
*The air hits the bodyat front,causing kinetic energy to be converted into pressure energy.This results in high pressure at the front.As the air passes over the Ahmed body it gets accelerated.When the air reaches the rear part of the vehicle,the fluid gets detached causing turbulent flow behind the body.Since the flow is accelerated and turbulent ,we know from bernoulis principle that velocity and pressure are inversely proportional to each other.So accelerated flow causes low pressure in back region.This leads to wake formation behind the ahmed body,which is evident from velocity contour.
Grid Independency -
*From the below table we can observe that,as the mesh becomes refined, the closer we are getting to the experimental coefficient of drag value.
*Also we can observe that all the values are almost equal.This proves grid independency.
| Global Mesh Element Size | 60 & 60 | 80 & 40 | 100 & 50 |
| No. of Elements | 354541 | 157803 | 98245 |
| Total Thickness | 3.56 | 3.56 | 3.56 |
| Coefficient of Drag | 0.311 | 0.302 | 0.301 |
| Coefficient of Lift | 0.215 | 0.205 | 0.209 |
Conclusion -
*Refined mesh with apropriate y+ value results in more accurate Cd value.
*The smooth curves around the front region are causing wakes,which creates low pressure in those region.
*The flow almost becomes stagnant at the front side of the Ahmed body ,causing pressure to reach maximum value.