For a subsonic external flow of an object of length L, what could the suggested computational domain to capture the velocity and flow profiles well.

The inlet I thought we could define thru' velocity and outlet thru pressure conditions. Is it OK.

What is the suggested approach to compute the lift, drag, moment coefficients.

(1). When a bird is flying in the air, are you able to detect the movement of air around you? (2). It is nearly impossible to feel the air movement or the pressure change, unless you are the kung-fu master in the TV show series. (3). When a bird is flying south, does the bird also question how and where to set the boundary conditions, so that the lift, drag and moment coefficients can be computed? (4). Naturally, the bird is not going to be flying a few inches above the ground, because that is the special capability of a stealth fighter or bomber. It is not the nature of a bird. (5). So, if a bird is flying over the tree top, say 50 feet tall, and the bird is about 10 inches long, then the distance from the ground to the bird will be 50x12/10=60. (6). I would suggest that you set the ground boundary condition to the fixed wall condition, that is velocity=0, and place the bird at the height 60 times the bird length above the ground. (7). To simulate the bird motion, you can fix the bird in the air and move the air instead. This can be done be setting a uniform free stream condition at a distance 60 times the bird length. And also using the same condition at the outer boundary 60 times the bird length above the bird, should keep the air un-affected by the bird motion. (8). You see, if the boundary condition is changing as the bird is flying, then it is really hard to compute the lift and the drag. And if the bird motion is also affecting the position of a small tree branch, it is going to be very hard for the bird to land on that small branch of the tree. (that is, it is going to be very hard for the bird to compute the lift and the drag so that the bird can land exactly at the right time on that branch.) (9). Well, the only boundary condition left is the exit boundary condition. You can use the paralle downstream condition, or the inlet fixed condition, as long as it is set at 60 times the bird length downstream of the bird. (to be on the safe side, I guess) (10). Since a bird can never fly at the transonic or supersonic speed, the above computational domain and boundary condition should be adequate from the observation of a bird flying. (11). If for some reason, you have to build a smaller cage to keep the bird in, so that you can study the lift and the drag, then you will have a lot of trouble in figuring out the right boundary conditions around the bird cage. (12). For human to fly, one needs a very, very long wing, and also a very, very big field to fly. The same is true, to feel a peaceful Christmas, you will have to be very far away from the center of the middle east.

This answer depends on several things, probably the Mach number of the flow is most important. For supersonic flow, you only need to enclose the shock wave system and ensure that no waves from the model which strike the outer boundary can reflect back to the region of interest on the model. This is a simple question of wave angles and geometry.

For incompressible, subsonic and transonic flow, you need a much larger distance to the outer boundary. How much distance depends on the precision you are seeking. If you are looking for qualitative data only, 5-10 body lengths' distance (L) could be enough. If you are looking for the best possible accuracy, then even the difference between 10L and 40L can be detected in the results. This distance can be reduced if you are using a higher-order boundary condition on the outer boundary.

So, like most things in CFD, there is no simple answer.

Dear John:

The bird illustration for the external flow computations was really very wonderful.

Many great ideas can be obtained from nature and this is one nice example. Thanks.

let us say we enclose the bird in a cage of 60 times dia. Lets say we solve only half the bird (not possible in real life of the bird) and simulate 180 deg hemisphere around the bird. and specify a symmetry condition in the mid plane. and one half of hemisphere with velocity condition in upstream. and one half of hemisphere with pressure condition in downstream.

would that be OK

(1). I think, it should be all right to do so. (2). Because at a distance 60 times the object length, the boundary condition or the flow field will be essential uniform (even the wake will be very weak). (3). But you will have to be careful so that the velocity and the pressure boundary conditions are consistent with your numerical formulation.(that is, the formulation allows you to do so.) (4). Once you have converged solutions, you can try to reduce the size of the computational domain, to see the effect on the lift and drag. The nice thing about the CFD is that, you can easily change the size of the domain in simulation, while it is very difficult to do so using wind tunnel approach. It is always to your advantage to move the boundary conditions far away from the point of interest, regardless of whether it is subsonic, transonic or supersonic. And I am going to make this the first principle of boundary condition in CFD. This is because, as you move the boundary conditions closer to the area of interest, the boundary conditions will gradually become the unknown solutions you are looking for. At that point, you can't setup the problem properly.

Dear CFD experts, With reference to the external flow computations, The replies are really very good. This brings to light: 1. The way the code will handle the boundary condition 2. The effect of boundary conditions on the results 3. The type of scheme used in the space and temporal discretisation 4. The extent of domain would be based on the type of the body, the velocities, density, compressibility, etc

How to get good results using Navier stokes based solvers for supersonic / hypersonic flow computations.

1. Does the euler based codes have an advantage ?

2. Using NS based Finite volume codes, what are the modeling and analysis considerations ?

> I would suggest that you set the ground boundary
: condition to the fixed wall condition, that is
: velocity=0, and place the bird at the height 60 times
: the bird length above the ground.

Assigning a fixed-wall (no-slip) boundary condition is unphysical. I understand that a large separation is recommended between the body and the "wall"; however, a no-slip boundary condition generates a boundary layer at the two walls with its negative consequences on the accuracy of the solution. There is good experimental evidence (unfortunately, I don't have the paper with me) that no matter how far the walls are from the body, the effect of the boundary layer eventually creeps in toward the body (after a "long" time).

A free-slip boundary condition or a velocity boundary condition based on the potential flow solution will yield more reasonable results (assigning the free-stream velocity at the "walls" may suffice)

> This can be done be setting a uniform free stream
: condition at a distance 60 times the bird length.
: And also using the same condition at the outer
: boundary 60 times the bird length above the bird,
: should keep the air un-affected by the bird motion.

Agree with the entry boundary condition but not the exit boundary condition. The wake behind the body can extend for miles (as I'm sure John knows quite well). If the solution is transient and we are evaluating the flow at the early stages, then setting a uniform free-stream exit boundary condition may/will make sense, because the exit cannot feel the effect of the near wake (as significantly). But as the wake proceeds further downstream, so should the extent of the exit boundary condition, IF we are to use the free-stream boundary condition. That is, the number 60 for the position of the exit may be valid up to a certain time, but as the wake grows, that number should grow as well (e.g., to 80, 100, 120, ...).

A more complicated, but not necessarily any better, solution will be to impose a wake profile at the exit. The difficulty here, as in other exit BCs, is that one has to know something about the flow conditions there to assign the proper profile. Hint: the wake is not steady, and it will "oscillate" up and down at the exit.

Adrin Gharakhani

(1). After reading the detailed answer, I am glad that I have been saying CFD is still a research field. (2). What I was trying to say was, if you decided to follow my suggestions, you are likely to get an answer, regardless of the type of boundary conditions used. (3). And I am sure that if you take a finite difference code or finite volume code with my suggestions, the result is not going to affect the lift and the drag of the object. In other words, the upstream effect of the downstream conditions at 60 body length can safely ignored. (this is not the case, if the boundary condition is located only a few body lengths away.) (4). AT a distance of 60 body lengths, the wake will be essentially steady-state. (And if someone is trying to capture the unsteady motion accurately at 60 body length away, he/she is probably using the analytical solution method.) (5). I tried very hard to make the picture as aimple as possible for the newcomers, but apparently, as they become advanced user of CFD, they definitely will have to take the more cautious approach you just mentioned. (6). The question really is: if another bird is also flying at the wake location 60 body lengths behind the first bird, is it going to affect the speed of the first bird? or is the first bird going to detect the existance of the second bird? And also in this case, if one is trying to compute the lift and the drag of the second bird, what should be the proper free stream (inlet) condition and location? (7). By the way, the second bird probably can detect the presence of the first bird through the wake motion (although I don't have any proof for that so far), but its lift and the drag are not going to be affected by the wake at 60 body lenghts from the first bird. For a second racing car to take advantage of the wake of the car ahead of him, it must be just a few car lengths behind, ideally inside the near wake of the first car. (but this is something else, because the wake of a car is always a large separated bubble.)

> For a second racing car to take advantage of the wake of the car ahead of him, it must be just a few car lengths behind, ideally inside the near wake of the first car. (but this is something else, because the wake of a car is always a large separated bubble.)

You should have continued with your bird analogy here Taking advantage of the near wake effect is why we see birds forming their V-shaped "squadrons". And these birds don't even have a BS in Aero or Mech. Engineering, let alone experience in CFD! But we digress

Adrin Gharakhani

(1). Yes you are right. As a mattter of fact I was expecting to get the example of the bird formation. (2). Next time, I will check whether the distance between two birds in formation exceeds the 60 bird lengths. It's already winter, except in sothern California (by the way, I am back in Westminster already), so we will have to wait till the next fall season. (3). Back to the lift and the drag issue. By the way, in order to get the lift and the drag values validated, the only practical way to do is to measure it in wind tunnel. So, naturally, one must simulate the wind tunnel conditions. In that case, the boundary conditions will be walls. (4). And I am sure that all of the NACA wings data were taken in wind tunnels. No one seems to have any doubt about the results up to now. Normally, there is a compressor fan in the wind tunnel, so, this is likely to cause some uncertainties about the measurement. (5). So, for the validation purposes, the wall boundary conditions in calculation and testing would be the ideal selection. Otherwise, self updating boundary conditions are hard to match between the calculations and the testings. (6). Well, as you can see, CFD is not just setting the boundary conditions. If the boundary condition is self updating, then it will become part of the solution. Then in order to match the test data, we also have to validate the solution along the boundaries. This is required, but it can be a very tough job to do. Along this line, I think, it is important to document the inlet conditions in detail when doing the testing. A uniform condition simply is not adequate. We also have to worry about the wake generated by the honeycomb ahead of the test section. Anyway, no one can afford to place the model 60 body lengths behind the screen, unless it is a real small model in a wind tunnel. (7). I think, in real life, one has to optimize the use of the computer hardware usage, and the simplest way to achieve this is to reduce the total size of the mesh or the computational domain. When this is a constraint, there would be need to find more accurate boundary conditions to obtain the same accurate result as the case using larger computational domain. And using the simple minded boundary conditions for the crowded space definitely will affect the result of lift and drag. (8). Anyway, it is unlikely to find a PhD from MIT sitting behind you to give you advice when you are running a case using a commercial code. This is because the need for an accurate solution is always far less important than that for a quick cost reduction solution.