boundary conditions and turbulence intensity
 

Dear all. I am modeling a rectangular channel with water. At the present moment I am dealing with 2 difficulties.

1) I have created the following expressions for the initial settings:
DenWater= 997;
DownH = 0.14[m](height of water at downstream);
DownPres= DenWater*g*DownVFWater*(DownH-y) (hydrostatic distribution at outlet)
DownVFWater= if(y<DownH1,0)
UpH=0.14[m](height of water at upstream)
UpPres=DenWater*g*UpVFwater*(UpH-y)(hydrostatic distribution at inlet)
UpVFWater= if(y<UpH,1,0).

Basically I have set the DownH=UpH because I want to have an uniform regime so the water height should be constant along the domain. The problem is that the solver is creating artificial walls( I have already pushed the outlet boundary far away the recirculation zone). In this context I had analyzed the results in the CFX-Post and I have seen that the pressure in the outlet is larger than inlet!!!How is this possible (I have set reference pressure equal to 1 atm)?I really don´t know why the program is doing this.

2) It is possible to set different turbulence intensities in the 3 directions using the k-epsilon model?

Best Regards

Try using a velocity boundary at the inlet rather than a pressure inlet. Do you know the flow rate? If so then this approach makes sense.

No. k-e is an isotropic turbulence model and therefore the turbulence is assumed equal in all directions. If you have anisotropic turbulence then you have to use a Reynolds Stress model or LES/DES.

Hi Horrocks.

I have done precisely that (by the way my channel has a width of 0.14 m a length of 1.7 m and a height of 0.14 m and an inclination of 9*10^-4). What you see above are the expressions that I have used in the "expressions field" in the CFX-Pre. However when I defined the boundary conditions for the inlet boundary I have used also the option cartesian velocity components. As the documentation say (and you also say that) defining a velocity at the inlet and the pressure at the outlet is usually the most robust way of defining the boundary conditions. Is the expression that I have used for the distribution of the pressure at inlet unnecessary (I think/thought that the solver need this information).

In what concerns the question related to turbulence intensities thanks for the answer..that what I was thinking but it always good to check.

Best regards

Hi Antonio,

What you should do is set velocity at the inlet (as you are doing with the cartesian components) and then set free surface level using the volume fractions (the UpVFWater expression you have there).

At the outlet prescribe the static pressure (not the average static pressure) and use the expression you have for hidrostatic pressure.

That should do the job. But you should check the tutorial CFX has on free surface over a bump.

Cheers.

Dear All.

Analyzing the results that I have I can see that I have an adverse pressure gradient in the bottom of my channel.I think that this is what is causing the recirculation of the flow. How can I control this?Any suggestion?

I am thinking changing the boundaries conditions (at the present moment I have a velocity at inlet and Static Pressure at Outlet):specifying the total pressure at Inlet and the velocity of the flow at Outlet.

Best Regards

I have found the same problem with my model.
Im working with air flowing trough a conveying line forced by vacuum.
The inlet its located at a large enclosure who works as a plenum slowing down the air. The the air flows to a bucket conveyor, where the outlet its located. The inlet is set up with a static pressure while at the outlet i set up a mass flow.
I have move both the inlet and outlet far away from my interest enclosure. That works well to avoid errors at the outlet.
The pressure at the inlet is greater than the pressure at the outlet, but the interface between the large encolosure (plenum) and the conveying line is greater than the presure at the inlet.

The problem seems to be solved by changing the turbulence option at the inlet, from 5% to zero gradient. I understand this option wors well with fully developed flow.

How do i check if the turbulence option selected match the one its expected at the inlet duct? wich reynolds and length scale should i use?

Thanks,

The best solution is to measure the turbulence length scale at the inlet of the device and then you know exactly what length scale to use. If you can't do that then you can guess by assuming it is a function of the size of the geometry, for instance half the step height, or the turbulent length scale from turbulent flow in a pipe.

An alternate way of doing it is to try the number you are currently using, and then do a simulation with double the value. If it does not change results significantly then the length scale does not matter.