[D2Net15]

Hello everybody,

I have a question regarding moving solids inside a tube:

The problem
In the tube is a flow regime with the velocity Vt (say from left to right).
In the tube i have a rectangular shaped body, which moves with the velocity Vb (from right ot left) in the tube.
I want to know the pressure field around the body with a steady state simulation (This point is very important!).

First solution
I already have the following substitute model:
The idea is, that i "drive with the body".
For this, i change the velocity at the inlet of the tube to Vb+Vt. Then i apply a moving wall bc of -Vt to the tube wall, to simulate a no-slip bc at the tube wall.

The question
The substitute model works pretty well as long as there is only one body in the tube.
But i want a more complex model: In the tube a second body shall flow with the speed Vb2, which can be different to Vb and Vt but moves in the same direction as the flow.
Now, i can´t work with the substitute model anymore.
Further, if i consider a stationary frame, i have to apply a moving wall bc to body1 and body2, but this is not possible, because the normal faces get a velocity which is normal to it´s face.

So, do you think it´s possible in CFX to model this in steady state?

I hope, i have explained the problem good enough.
In case of questions i will be more clearly

Thanks in advance!

PS:
Two more things to consider:
1. I know, that the pressure field is strongly transient, because of the passing of the two bodies.

2. One of my ideas was to model a moving wall on the parallel side surfaces + to change the normal faces to an inlet at the front (with the respective body velocities) and an outlet at the rear (again with the respective body velocities).
Sadly, the solution was strongly different to my substitute model and the flow field looked weird.

[evcelica]

I would do exactly what you are doing, model in the bodies reference frame.
To be more clear, instead of left/right velocities, always use one direction, and just use negative values for velocity to specify direction.

You made a mistake/typo though, as the wall should have a wall velocity of -Vb, not -Vt.
Starting with reference frame of the wall:
V.wall = 0
V fluid = Vt
V.body = Vb


Moving to reference frame of body: subtract Vb from each.
V.wall = 0 - Vb
V fluid = Vt - Vb
V.body = Vb - Vb = 0.

As far as doing 2 bodies, this doesn't make sense to solve in steady state since it is a transient problem. You could run a transient simulation though.
I would:
Simulate the two bodies with the same velocity Vb, just like you did one body. Save these results for initial conditions for the transient model.
Second model will be transient, and include the additional velocity of the second block using mesh deformation to move the second block at a velocity of Vb2 - Vb. Initial conditions will be from the previous model.

Of course this won't be fully correct until the block has moved enough for the flow to develop around its new velocity, so start it further back than the area you are interested in.

[D2Net15]

Thanks for your reply.

You made a mistake/typo though, as the wall should have a wall velocity of -Vb, not -Vt.

Yes it was a typo. Of course, I meant -Vb.


Second model will be transient, and include the additional velocity of the second block using mesh deformation to move the second block at a velocity of Vb2 - Vb.

As is said, i only want to simulate it as a steady state (for now).
Maybe i have to accept, that this is not possible

Regarding mesh deformation: I experimented with this concept several times, but i only got solutions with small deformations (i remember the cfx guide, that this is meant to be so).
Therefore, i will use the concept of sliding meshes in case of a transient simulation.

[evcelica]

If you only want to do stead state models, what about using two models. the first original one, then a second one with the second moving block. The second block would have the outlet velocity profile from the first model used as the inlet, but with the adjustments made to the velocity profile (Inlet and wall) for Vb2 vs Vb.

Export The outlet velocity or outlet mass flux of the boundary from the first model in CFD post. Then use that as a 3D interpolation function in CFX Pre for your inlet. Format it something like (x,y,1,Velocity) so that the Z location is just 1 and does not matter.


I don't know if it would be possible to do some sort if interface that would change the velocity for you across this interface. but it could be done manually as I described.