Axial velocity problem in 2D axisymmetrical flow
 

Hi everyone,
I am simulating the flow over a rotating disk in 2D axisymmetrical geometry. The problem is that there is nearly no axial velocity occurs on the disk. Radial and swirl velocity components are fit completely with the data in literature (von Karman solution) but axial velocity component is too small. It cannot be even compared with the Karman solution. For example, it suppose to be about 100 unit but I report it about 1 unit. It is really weird when the other two components look perfect.
Can someone provide any explanation?
Many thanks in advance.

Musa

If you are willing to give some information about your setup, maybe someone can help.

Well, the geometry is so simple as in attachment. Boundary conditions are as follows;
Disk: moving wall, constant rotation speed, no slip
Walls: no shear stress
Velocity inlet: radial and swirl components are zero and the axial velocity gradient in z direction (axis direction) is zero.

Velocity inlet boundary at top was wall at first and I got the same weird results for axial velocities. I decided to change it to zero gradient condition but it didn't affect results much.

Velocities are read at created points in domain with 'vertex average' choice.
Radial and swirl components are perfect but there is a problem with axial.

Many thanks!

Since you have no outlet in your domain, I dont see how an axial veloxity could be established.
The fluid simply has no way to go.
Maybe the right wall is supposed to be some kind of outlet in the benchmark you are comparing your data to?

Dear Alex,
Thank you very much for your suggestion. Actually because of centrifugal force created by disk rotation, there should be a suction over the disk towards disk surface. This model is a water tank and the rotating disk is mounted at the bottom of this tank. This is a usual experimental rig in literature for rotating disks which hasn't got any inlet or outlet. Fluid is supposed to be circulated in tank with coming towards the disk and centrifugal force pushes it out above the disk and so on. I did try your suggestion anyway but the result hasn't been changed.

The problem can be reporting the results, I guess, but not sure really. Since two velocity components are fit very well the last component should be fit for momentum conservation. I mean there may be an axial flow in my solution which I cannot succeed to see in 2D axisymmetric swirl domain. Is this possible?

Musa,

Alex is right, I think you need to check the underlying physics you are trying to model.

There is something fundamentally wrong in your simulation because if you have one inlet and no outlet, d(rho)/dt > 0. So as t->infinity, your vessel will turn into a black-hole....

Stu

Thanks Stuart, you are both absolutely right. But what I am telling is that the results are not changed in these conditions:
1st try: there is neither inlet nor outlet, all are wall except axis.
2nd try: top is inlet, others are wall.
3rd try: top is inlet, side is outlet.

In other words, I do not have any inflow or outflow (they are really small, I can say zero!) even though I define the boundary layers as inlet and outlet.

Musa,

How do you get axial velocity at the disk then? Wouldn't the axial vector be pointing through the disk?

Stu

Dear Stuart,

I am reading all the velocity components at several created points just above the disk, in the boundary layer. How can we explain fundamentally, if two velocity components (radial, azimuthal) are totally perfect in this boundary layer, why there is nearly no third (axial) velocity component?

Musa

It depends where the point is in your geometry. This could be a mesh refinement issue...? Are you using wall functions?

Stu

Are you really sure about the position of the monitor points? The axial velocity is supposed to be zero in the vicinity of the wall.
This could explain why the values you get are too low.

The mesh resolution is another issue, especially since the monitor points in fluent are vertex-averaged.

Another boundary condition worth trying is a pressure inlet at the top boundary.

Basically, this means that the velocity field is not divergence-free. My first guess is that the solution is not converged.

My viscous model is laminar and I am using very fine boundary layer mesh (there are 20 cells inside the boundary layer thickness, which is known theoretically). I have 45 points above the disk from the disk surface to 10 times BL thickness. I thought as Alex said near the disk axial flow getting closer to zero and I plotted the axial velocity component on a line which is between disk surface to upper boundary in whole domain but still I read silly values in that xy plot. Also vector plotting in this 2D plain doesn't show really a 'strong' axial vector. I can see the flow coming towards the disk but the values are just funny.

It is converging finely.

Do you trust the axisymetric swirl model in fluent? Maybe it is a good idea to set up the case in 3D.

In this case I can't I am afraid. I've been struggling with this problem for about a week and it drives me crazy :) If the other two component were look like a disaster, I wouldn't keep trying. I could say easily this solution is rubbish. But in this case it is difficult to make any comment. I should try 3D case and see what will happen. Thank you very much again for all of your replies and time you spent for me.

Musa

:eek::eek::eek:

I hope the axis is the z-direction only in your drawings.

In Fluent, the axis in an axisymetric case HAS TO BE the x-axis.


Different topic: Would you mind telling me how you created a velocity-gradient boundary condition in Fluent?

Yes, it is just in drawings. Axis in simulations is x-axis, I know that.
I created velocity-gradient (zero gradient) with a udf which looks like this;

#include "udf.h"

DEFINE_PROFILE(axialVelocity,t,i)
{
real xf[ND_ND], xc[ND_ND];
face_t f;
cell_t c0;
Thread*t0;
begin_f_loop(f,t)
{
F_CENTROID(xf,f,t);
c0=F_C0(f,t);
t0=THREAD_T0(t);
C_CENTROID(xc,c0,t0);
F_PROFILE(f,t,i)=C_U(c0,t0);
}
end_f_loop(f,t)
}

Oh dear!!!
I found my mistake, there is nothing about Fluent/simulation. It is about the scale of data which I compared. I nondimesionalized velocity components with dividing (rotation speed*radius) but only for axial one, I also need to multiply this nondimensional velocity with Reynolds. Now the axial profile looks fine too. Simulation works very well actually, sorry again for taking your time.

Musa

Musa, did you ever get around to doing the 3-d version of this case? I am doing something very similar and having a bit of an issue defining/figuring out my boundary layer. I have rotational flow inside of a geometry that is defined to be air, I am trying to find the boundary layer created around the disk, should I just create some points and then bring them closer and closer to the geometry until the velocity no longer changes significantly?

Hi John, I didn't try 3-d, after I found my problem. If you are asking the boundary layer thickness above the disk, theoretical thickness in the literature is 5.5*sqrt(kinematic viscosity of fluid/rotational speed).

And yes, you can see that boundary layer thickness with creating points above the disk and plotting the swirl component of velocity from these points (as I did and saw the theoretical thickness in my case.)