How to make the water slightly compressible in CFX?
Dear all,
I am doing a simulation of flow in porous media and came into a problem. Someone suggest me to make the water slightly compressible. I worked on it for several days but still can not make it. Could anyone help me on it? What settings I need to do to make the water slightly compressible in CFX? Many thanks for your help. Regards John 
Why do you think slightly compressible water will help? Is it likely that the density change is going to be significant? If not then I guarantee it will not help. Your problem is just obtaining convergence.
But compressible water is easy. Get the bulk modulus from google or somewhere, and define density as a function of pressure. I have done it many times and it works fine. And this is not a simplification, you are actually adding more physics to your model so your model will get more accurate  if compressibility is important. 
Dear ghorrocks,
Thank you so much for your reply. I set the "Heat Transfer" of fluid model to "Total Energy" and defined the water density as "( 997 / (1  (Absolute Pressure  101325 [Pa] ) / 2.04e9 [Pa] )) [kg m^3]". Moreover, a minimum absolute pressure of 1000Pa and a maximum one of 1e6 Pa are set in "Table Generation". However, the model can not work at all. No information is given, even no error code. Could you please help me to figure out the problem in compressibilty setting or is there any other experience of it? Thank you for your kind help. Regards John 
Do not use Total energy, just the default isothermal is fine.
Please post your out file to help us diagnose the problem. But as I said previously, if you are doing this because you have convergence problems this will not help. It is more likely to make it worse. 
Hi ghorrocks,
I turn the total energy to isothermal as your suggestion, but a new problem comes out as bellow: ++  ****** Notice ******   While evaluating Static Enthalpy,   Absolute Pressure   went outside of its lower limit. Its minimum value was   4.3028E+10. The bounds error was handled by clipping.   If this situation persists, consider increasing the table range.  ++ ++  ERROR #001100279 has occurred in subroutine ErrAction.   Message:   Stopped in routine ENFORCE_BOUNDS            ++ I am doing a model of water flowing over a porous medium, with mesh deformation in the water domain. The model can run without mesh deformation in water domain, but can not work with the mesh deformation. Others have suggested to make the water slightly compressible to solve the problem. 
Like I have said, adding compressibility will make convergence worse, not better.
If you have convergence problems forget about compressibility and deal with the convergence problem. Do you intend to run this model incompressible? If you run it incompressible what happens? 
I have run the incompressible model. It can run without mesh deformation of water domain, but can not work with mesh deformation. That's why I would like to try the compressible model. How can I make the porous domain work together with the moving mesh water domain?

Please describe more details of the case. Total Energy with compressible water is the correct approach to resolve acoustic waves in water (e.g. water hammer), but it's not clear that this is what you want to do. If your timescale is small enough to resolve acoustic waves generated by a moving boundary then this might be a valid approach.

Quote:
Folks, the equation is similar to the linearised Tait equation, only the CFX implementation is buggy. The correct formula would be: 997[kg/m3] * ((Abs.Press  101325 [Pa]) / 2.04e9 + 1.0) 
All times are GMT 4. The time now is 19:02. 