Hello.

uhm. I want to simulate this.

Flowfield includes object is moving in pipe. ------------------------------------------- wall

--- (flowfield) | | <-- object

--- ------------------------------------------- wall

--> x

I appled wall boundary condition to the object, The U velocity was applied to the wall of object. but according to result, U velocity at the vertical face of object to flow is zero.

Can you tell me how to apply BC for moving object, or another methods?

(1). You can change the coordinate system from the stationary one to the one moving with the body (assuming that you are dealing with a simple problem of a body moving at a constant speed,Vx) (2). In this new coordinate system the physics will be the same, except that the boundary conditions must be changed to the new system by adding a negative velocity term (-Vx) to the original wall , and inlet condition. (3). After transformation, the wall will be moving at (-Vx) speed. And the original inlet condition will become (V,inlet) + (-Vx). If this resultant velocity change sign, the original outlet will become the new inlet. If the original inlet velocity (V,inlet) is greater than the body speed (Vx), then the inlet will remain the inlet ,except the velocity will be reduced.

yes this is an easy problem as john said just change coords from abolute (fixed with pipe) to relative (fixed on the obstruction in the pipe). if your problem is compressible don't forget to adjust your stagnation pressure and temperature at the upstream boundary. if not then forget what i just said

I think you can set the wall velocity with the moving velocity of the object.

If you use moving grids, you have to consider that the grids have a velocity, that means a cell helding the flow field values changes its position from time to time and it's position is then not the same position as in the flow field in the coordinate system. Therefore, you have to introduce some additional terms in the governing equations to reflect the change of the cell position. You can look into the paper:

J. Steger: Implicit finite-Difference simulation of flow about arbitrary two-dimensional geometries, AIAA Journal, Vol. 16, No. 7, July, 1978

X. Ye

If one goes to moving grids, you not only have to introduce the grid velocities in the convective flux function (arbitrary eulerian lagrangian approach), but consider the geometric conservation law (GCL) as well, which presents a relation between the grid velocities and the temporal change of the volumes of the grid cells. Neglecting the GCL leads to unavoidable errors in the solution, which are not to neglect.

Are you meaning the change of mass and energy caused by the change of the cell volume? Yes, this a very important point. Generally there are two types of moving grids: 1. the total grids move with a velocity and there is no change of grid size; 2. Only some grids chnage it's size or grid lines will be removed or added. For the 1. type of moving grids you don't need to consider the implicit change of mass and energy since there is no change of cell volume. For the 2. type of moving grids you have to consider to correct the mass and energy.

To see whether your moving grids formulation is correct or not, you can do a simple test calculation such as cylinder compresion and compare with the theory of thermodynamics.

X. Ye

yes. The GCL has to be applied if the grid cells change their volumes. The first test would be to move some grid points within the domain and e.g. keep the boundaries fixed. If the flow is uniform (simplest is to set u=v=0, such that the is in rest) nothing should happen. If violatin the GCL one will see something is happening, which is unphisical. But this basic test only gives the free-stream capturing property. It does not say anything about the correct temporal discrtisation of the GCL. Many authors choose a second order scheme in time, but just discretise the GCL first order in time, approximating the grid velocity by (delta x)/(delta t), which is only first order in time. I think this is very doubtful and not to recommend. Of course, it is the easiest and maybe one can live with it any many applications.

if computing navier-stokes and you indicate boundary conditions at the walls, one (of course) has to set the relative velocity of the fluid particle with reference to the object to zero and not the absolute velocity. At the wall, the fluid is moving at the same speed as the object moves. Maybe your code simply sets it to zero, not knowing that the object is moving ?!

Yes, I see also that this is the most probable error, because the value on wall will be set but not be calculated.

X. Ye

Thanks a lot for your comments. I understand what you said.

May I ask another questions? if object is moving along the Y axis or velocity of object includes y component, How can I apply BC?

I wait for your comments? Thanks

It would be useful to know what equations you try to solve ?! Euler or Navier Stokes ?! Otherwise it is impossible to suggest any boundary conditions to apply.If solving Navier Stokes, one has to set the velocity at the wall according to the velocity of the object at the considered point at the wall. No matter how the object moves.

it'd be done similarly. but you have to remember that the object cant move across the pipe forever