Hello Everyone:

I am trying to get the flow field over a car. I am having some trouble in understanding certain boundary conditions. The problem is as follows:

The flow is incompressible I have a computational mesh over the surface of the car. I could apply velocity boundary condition at the inlet and pressure boundary condition at the outlet (I will make sure the exit length is long enough to make this boundary condition valid). I will apply wall boundary condition at the bottom.

I have problem in understanding the rest of the boundary conditions. I have been recommended to use symmetry boundary conditions on the sides and the top. I know that when symmetry boundary condition is applied, the gradient across that boundary is zero. It acts as a mirror. This does not answer my question completely. My question is: What it physically means? Does it help to reduce the near wall effects?

All your insights and advise is appreciated, Thomas

Hi Thomas,

I might be stating the obvious here, and you might already be knowing this.

(1) When you use symmetry conditions at the sides you make the problem two dimensional. So by using symmetry conditions on the sides you imply that you are assuming that flow variables show no variation along that direction and you believe that end effects are negligible. Consider a loaf of bread, all the bread pieces in the center are the same, except at the edges. So you are studying aslice of bread, in the center assuming that the shape of bread remains the same. This is true except at the last slice of bread.

(2) As the flow over the car develops, you start having a boundary layer like phenomena, where the change in velocities and pressure occurs near the car surface. But far away from the car the changes in the variables are small ( like outside a boundary layer). So you use a gradient bc.

hope this helps

Anil

(1). A car can be a cube or a sphere, a car can be a wedge or a streamlined body. Anyway, a car is a body with wheels attached to it, and it can move in any direction. (2). When a car moves, the wall boundary condition remains the same, that is non-slip boundary condition. (3). The wall boundary condition on the wheels and tires remain the same, except that it rotates about its own shaft. But you can assume that the wheels are locked, and the car is sliding. (4). When a car is moving at a constant speed, sitting inside the car, the ground is moving at the same speed except in the opposite direction. You definitely would like to work in this coordinate system because it is easier to move the ground and the air. So the ground is moving toward the back of the car at the car speed. (5). Since you rarely drive the car in the wind direction, you must figure out the direction of the relative wind in addition to the car speed. This will determine the free stream boundary conditions, that is relative to the car. (6). Now, you need to define the far-field boundary. For this, you can create a large box to cover the car and specify the far-field boundary condition on it. This basically amounts to specifying the relative velocity along the boundary surface. Since the box is large enough, the wake of the car eventually will return to the free-stream condition. If you are not sure, you can apply a down stream condition at the rear end of the large box. (7). This is all you need. As for the symmetry condition, you really do not need it. In this way, you can compute real 3-D flow over a car. (8). But , if you are interested in the flow field over a car driving at no wind condition straight ahead, then you can save the computing time by using the symmetry condition at the center plane of the car. In this way, you compute only one half of the flow field. The symmetry condition in this case simply means that the normal gradient of flow variables on this surface is zero.(9). So, you have now, the moving ground boundary condition, the car wall boundary condition, the far field boundary condition and the downstream boundary condition. The key in this case is to make the far-field boundary very large so that the free stream relative condition applies. As for the size, you can try out some to check out the difference in results.

Hello Anil and John, Your insights were appreciated.

Thanks, Thomas

I think, that Thomas wanted to know what it means if he uses a symmetrie plane as far field bc if there is no other far-field-bc-type available.

It is very interesting. Sure, you can use the symmetry condition on both sides of the car. Have you watched the Daytona-500 NASCAR racing ? This is the case when there are cars on both sides. On either side of the symmetry plane,the flow fields are symmetric. In this case, the far-field is really not very far from the car. As for the symmetry condition on the top, it is not a very good idea at all. Just move the top of the box to about ten times the car height and place the far-field boundary condition there with fixed free stream conditions. ( By the way, this height is a function of the Mach number of the car. To simulate the far-field condition for a car breaking the speed of sound, it has to be very far from the car .) If you are simulating a model car in a wind tunnel, you can also use the symmetry condition to replace the wall. In this case, you are really in the cyber space ,that is there are invisible cars on both sides of the wind tunnel. Even in the wind tunnel case, you can still use far field condition at the location of the wind tunnel walls, as long as the model car is not very large to block the flow. If you have to be very precise about the wind tunnel wall conditions, then just use the wall condition there. The existence of the wall boundary layer is not going to change the flow field at all. ( if the wind tunnel and the model are designed properly.)

Hi Thomas,

just a short note on the far-field conditions: Have you tried to use non-reflecting boundary conditions at the exit. There are lots of references about this subject. This "technique" is often used in calculations of airflow around a wing section, to reduce the "size" of the computational domain and therefor the computational time.

Good luck.

Ridwan

Hi Ridwan, I have read about non-reflecting boundary conditions being used in aeronautical applications to reduce the computational domain size.

I am using FLUENT to run the analysis. From what I know, I do not think FLUENT supports this boundary condition. In case this boundary condition is supported by FLUENT, it would be useful for my case.

All your feedbacks are appreciated, Thomas

Very funny, but ...

The condition for symmetry planes is that the normal velocity and the normal gradients of all other variables are zero.

So it is an approximation of a free-stream boundary. The question now is, how good or bad this approximation will work.

Also the manual of a popular cfd-code tells you to use symmetrie planes this way.

A free-stream condition is a condition which is known and fixed. Therefore, the flow variables, say, the velocity components are known and fixed. A symmetry plane condition controls only the zero normal gradient of all flow variable. Therefore, all flow variables which are on this plane or vectors which are parallel to this plane are not fixed and are floating. When the flow variables are floating ( as part of the solution , therefore are not fixed ) , it is not the so-called free stream condition. The free-stream condition is always fixed and can not be changed. Since the flow variables on the symmetry plane change from place to place, the symmetry plane condition can not be considered as the free-stream condition. The free-stream condition simply can not be part of the solution. ( symmetry plane solution is part of the solution of the problem.) Therefore, symmetry plane condition can not be used to replace or to simulate the free-stream condition.

...wrong.

Lets assume a car moving over a plane surface with nothing around for miles (e.g. a salt lake) and we want to compute the flow field around this car.

Then we have several possibilities to do this:

1) The computational domain will be choosen 100 times bigger in every direction than the car. At this distance it should be valid to say the the car has no influence at the flow field and we can fix the boundary conditions at the top and the sides of our box (no normal component of velocity and equal static pressure over the surface) . --> we use that what you call a free-stream bc.

2) The domain is only 5-10 times of the car size. Here we are sure that the car influences the flow field at the boundaries of our box. If we want to use your free-stream bc now (known values and fixed) we have a big problem because we don't know these values. Now we can either do some measurements or use some approximations.

for example:

- the normal component of the velocity is zero and a

slightly incorrect turbulence at this distance does not

influence the flow around the car. But the pressure

should not be equal over the surface. Then we just have a

symmetry plane or slip wall.

- the pressure at the sides and the top and maybe also at

the rear end is more or less the ambient pressure. Then

we can use a pressure-bc with the option, that the mean

value over the complete boundary surface is equal to the

ambient pressure. This way we permit a pressure

variation over the boundary surface of the domain and

also the possibility of a normal velocity component.

But we are not allowed to call this a free-stream bc

because it has to be computed (and is not fixed)

Now we have to decide which way will give us the best results but I stop here because there are better things to do on friday night ... have fun.

It is very interesting to know all these info about the B.C. when simulating external flow around an object. Could any one comment on how to choose the size of the domain? Say the characteristic length is L and is subject to a flow of v. Thanks.

There is a bigger problem of replacing the free-stream condition by the symmetry condition. Once you have set up the mesh and geometry, the use of the symmetry plane condition is like a slippery wall. At this point there is no simple way to compute the case with cross-flow, that is when the wind is not aligned with the plane of symmetry. But , with the free-stream condition, you can apply any flow conditions there, at any angles. As I said, one really has to experiment with the size of the far-field condition. At a distance of 10 car width, a person, a car, or a truck, standing or moving there, is not going to affect the flow field over the car at all. ( it may disturb the sound field though)

The easiest way to do is to get hold of a lot of experimental flow field pictures ( flow field visualization, you should be able to find this types of information in the library), and try to study the detail. Pay special attention to the streamlines, smoke or oil patterns, shock wave patterns. You definitely would like to find the boundary where the conditions are known and easier to apply to your CFD problem. If you are not sure whether the size is correct, you can always run another case with size increased. The results will tell you whether you need to go a step further.

I should suppose that the use of a free-stream conditions on the all outer boundaries is impossible because of mass conservation considerations. It seems to me that such free-stream conditions can be implemented only at the inlet boundary Greetings

Shigunov

Well, you can always run a test case and check the mass conservation over the complete outer boundary, including the ground bounday and the far-field boundary by surface integration. Since the ground wall is assumed to be a non-slip condition,that is v=0, there is no mass transfer across it. And, if you specify a far-field constant condition on the far-field boundary, I think, the mass will be conserved when you perform the surface integration of the rho*v*d_normal_area. The surface integration can be decomposed into two parts, one in the v direction and the other in the -v direction. Since rho*v is constant everywhere on the boundary, the surface integration is equal to the sum of rho*v*( total projected area of the boundary in the v direction + total projected area of the boundary in the -v direction) which is rho*v*(Area - Area)=0. That means there is no net mass flow through the far-field boundary. I think, the best way to find out whether it is going to be a problem or not,is to run a test case and check out the results on your own. And in the flow over a car problem, somehow one needs to include the exhaust gas in the consideration, this can be done on the downstream side of the far-field boundary . As long as the total mass flow through the far-field boundary is equal to the total amount of the car exhaust gas, it should be o.k. In most cases, one can ignore the exhaust gas part ( set it to zero), then the far-field condition can be set equal to constant.

The crossflow is no problem at all if we keep it in mind from the start of the modelling. We just have to rotate the car in the "flow-box" .

By using an arbitrary mesh interface the rotating angle can be changed in less than 5 minutes (deleting the existend couples, rotating some verticies, recreating the couples).

This practice is not very common but works perfectly well.

This is perfectly all right when testing a model car ( or even a real car) in a wind tunnel, where the wind direction and the wind tunnel walls are all fixed, and you can rotate the model to simulate the corss-flow condition. Even though you can still obtain resonable results, the wind tunnel condition is not really the free-stream condition. As long as the results are acceptable, it really does not matter how you simulate the boundary conditions. But one of the reason why CFD is so attractive is because a free-stream condition can be easily used to obtain the result which is more realistic than the wind tunnel simulation where the size is always limited.( you almost need a wind tunnel of size 60x60FT test section to test a real size car, to simulate a free stream condition. NASA probably has one like that)

1) For inlet, the only buondary condition for most of problems, is the free-stream condition 2) For the side boundaries, the free-stream condidion seems me as more restrictiv then the symmetry condition and thus demands not smaller size of the computational domain 3) For outlet, the free-stream condition does absolutely not suit Mit best regards

[jha.kashyap]

hi, i m conducting drag force analysis over a 3d car.in this i have used boundary condition as inlet as velocity inlet ,car body as a wall,lower boundary of domain as wall,outlet as pressure outlet..now i tried to give pressure far field condition on side walls and also on upper wall of domain but i m not getting the results .rather than it diverges..can anyone help me to get the result with above mentioned boundary condition..i m using fluent as analysing software..
thanks