Compressible Flow in Ansys CFX
 

Hello,

My original problem is FSI simulation but I have a basic problem with CFX compressible flow. I have removed the structure part from my fsi simulation and set up the fluid domain with walls at structural locations to match the static pressure with the matlab code that is close to my experimental results. I am also using flotran to verify that I get similar results from flotran and cfx.

I get same pressure in matlab, flotran and cfx when I use constant air properties at 25C for input velocities as high as 50 m/s and my max velocities are around 100 to 300 m/s. I know that my max velocities are close to speed of sound but I just had to check the static pressures.

To do near compressible flow (which is enough to do my fsi simulation) I gave bulk modulus in flotran and changed material to air ideal gas (total energy option) in cfx. The flotran gives very similar results to that of my matlab code and I am able to notice the difference in pressure due to change in density. In cfx, the problem is that there is a very high change in pressure and density as soon as I shift to air ideal gas. The pressures and densities are 100 times higher than what I get from flotran or cfx with air at 25 C.

I did check my reference pressure which is 1 atm. I could not find what was my mistake and why is there so much difference between cfx results when changing material to air ideal gas. I appreciate any help from you and also will be glad to provide more rinformation if needed.

Waiting for some help from you guys. Thanks.

You have some sort of setup problem. Please post a drawing and boundary condition details.

Thanks Glenn.

I am interested in the pressure applied on the structure by the fluid flowing from the pipe. I am attaching the pictures to describe my domain. The pipe is 1m*1m*1m (only 1 element thick in z-direction), the fluid is flowing out through the gaps above and below the structure (looks like plate in 3D but is a beam in 2D) modeled as walls for fluid analysis. I place openings far away from the pipe outlet around 15m away.

Domain - Air Ideal Gas Ref Pressure 1 atm Total Energy

Wall - No slip Adiabatic

Inlet - 50 m/s Normal velocity Static Temperature 25C

Opening - 0 Pa Opening Pres. and Drim Flow Normal to Boundary Opening Temp 25 C

Symmetry - In Z direction

The max pressure is around 60000 Pa for air at 25C but when I use Air Ideal Gas the pressure is almost 100 times higher. I tried to refine my mesh but it did not help.

Once again I thank you for your help.

I have no idea what your diagrams are showing. As clear as mud comes to mind. Please label a diagram.

Sorry for previous images. I am attaching 2D pictures of my setup because I have only 1 element and symmetry conditions in z-direction. Thank you.

The flow has choked in the constrictions. You have not done physically possible boundary conditions. CFX is giving rubbish results because you set up rubbish boundary conditions.

If flotran's compressible solver says this flow is possible then I doubt you have set that up correctly either.

Could you please explain a little more about which of my boundary conditions are wrong.

In flotran, I did not use compressible flow. I just gave bulk modulus of air.

Are these boundary conditions not possible for compressible or for both compressible and incompressible flow. I get similar pressures (same as my analytical results) when I solve incompressible flow.

I am attaching a drawing of my domain. I am trying to give a clear picture of my problem so that you can help me find my mistake.

I have a pipe with small opening area above and below the structure attached to the end of the pipe. I am interested in solving for pressure and velocity of the fluid.

I model the pipe with small thickness. I am using the boundary conditions as shown in the picture. I do not have any boundary conditions at openings and place outlets far away from the pipe.

I am unable to find which of these boundary conditions are wrong. I have the same setup in my lab. A plate attached to the end of a pipe with small openings to allow fluid flow.

Thank you for your help.

Sorry. I forgot to attach the image.

I already told you what your problem is, your flow is choked and you have exceeded the physically possible flow rate through your little slits.

If you do not know what choked flow is you had better look it up, you won't get far without knowing the basics. It is a compressible flow thing which puts a maximum limit on the flow rate which can go through an cross section as the flow goes sonic.

Thank you Glenn. I posted those replies only to make sure that I am at least doing it right for incompressible flow and compressible flow within the limits.

I read the choked flow and also the effect of compressibility and understood my problem.

I lowered my input velocities and now I am getting similar results for both compressible flow and incompressible flow in both flotran and cfx.

Thank you once again.

Dear Mr. bcheruk
Thank you for you information. I know you used compressible flow in you case, you set air to be compressible. would you please help me how to set liquid (like water) to be compressible. thanks a lot.

For a compressible gas you need to have density as a function of pressure, temperature or other parameters. So to make it incompressible simply select a constant density in the material properties.

Dear Mr. Ghorrocks,

I would like to ask you that if i use the fuel density in high pressure pump as a function of pressure (it dose not change to much (804-808[kg m^-3])) and in isothermal option in CFX. Is it the compressible flow or incompresible flow in my simulation?

Thank you in advance!
Tung

It is compressible as the fluid can be compressed. But note that you don't have an energy equation so you do not have an ideal gas or anything like that. This means you can form density waves, but you cannot form shock waves.