CFX wather hammer capacity
 

Hi,

I have to evaluate the wather hammer effect on a pipe of 2m of diameter on 600m. The fluid is wather.

I read on previous post that it's possible and that I have to make the density function of pressure. But, I have other questions:

1. What type of mesh does I need to correctly simulate the phenomena?
2. Is CFX able to considere cavitation in water hammer problem?
3. To correctly simulate cavitation and water hammer problem, does I need a fine mesh?
4. Is it preferable that I look for an other software like Autopipe or Ceasar II?

Thank you,

Michael Page, ing.
Le Groupe Genitique inc.

Any will do. High quality is always better, but any mesh will do.

Yes.

Depends what "correctly" means. You will need to do your own mesh sensitivity study and find out. Everybody is looking for different results so there is no universal answer.

I have never heard of these softwares before so have no idea whether they are better or worse.

With your informations, I think that I can use CFX for my proble.

Thank you,

I would not recommend trying to simulate cavitation that is induced by an expansion wave (i.e. a pressure wave due to water hammer that gets reflected at a closed end producing low pressure). In theory all the models are in CFX to simulate this, but the timestep that would be required would make it impractical (it would need a much smaller timestep than that needed to just resolve the pressure wave). Solver stability would likely be a problem too. Using a Navier-Stokes code to solve water hammer is an expensive way to do things. A method of characteristics code should be your first choice (I would assume the codes you mention are based on the method of characteristics).

Thank you Stumpy for your advice.

But, is it a good aproximation to verify if there is somewhere in the model that the absolute pressure fall below the vapor pressure to see if there is a chance of cavitation?

I agree that modelling water hammer induced cavitation on your large model is likely to be very difficult. But I do not agree with stumpy that modelling water hammer in CFX is impractical - I have done it and it works fine. Admittedly I used a smaller geometry than yours but it works fine. It will be slow simulations as you need to be careful with time step size.

But if simpler approaches like method of characteristics is applicable (especially if a 1D assumption is appropriate) then other approaches will be far more efficient than CFX.

As a first order approximation assuming it cavitates when the pressure drops below the vapour pressure is good. There are all sorts of delays and non-linearities in the real process but on large scale stuff these become small.

Ok,

So, here is the procedure that I will use.

Firstly, I will simulate the water hammer effect with a software who use 1D assumption (the name of the software is Hitrans). I will be able to have rapidly some results.

After, I will do a CFX model. With a mesh sensitivity study, I will also be able to evaluate the precision of results with 1D assumption. I want to make a CFX mesh for coupling possibility.

Finaly, I will use CFX results to evaluate the stress in the pipe (with the inclusion of temperature effect) and the stress in anchors.

Thank you again for your help.

CFX is only going to be able to give you better information if 2D or 3D effects are significant. If it is just a long pipe so the 1D assumption is pretty good then it is unlikely CFX will add much. Even the pipe stress stuff is then better done from the 1D model.

Agreed that modelling water hammer is not impractical (I only said directly simulating the cavitation was impractical), but it's just more expensive than a 1D code. It can become impractical if the transient duration is long and a fine mesh is needed in the wave propagation direction (see below). Looking to see if the pressure drops below the vapour pressure without simulating the cavitation is a good approach. Be careful with a mesh dependency study. The important thing for water hammer simulations is the Courant Number, based on the wave speed, not the fluid velocity. For accurate results ideally this should be 2 or less, but 5 or less seems to be reasonably accurate. If you refine your mesh in the axial direction then you will increase your Courant Number for a given timestep size, which could make the results less accurate. So if you use a high aspect ratio mesh to give a coarser mesh in the axial direction you'll be able to use a larger timestep. However, your mesh still needs to accurately resolve the geometry (bends, junctions, etc). As Glenn said and I said earlier, a 1D code should be your first choice. I'm not sure if you can include the temperature effect or not in these codes but I'm sure stresses can be obtained based on the fluid pressure. If you do need to use CFX then it can solve the problem fine, it just takes longer. If you are going to couple this to ANSYS to get the stresses, then this is a 1-way transient FSI simulation (assuming pipe deformations don't significantly relieve the fluid pressure). This is best ran using the 2-way coupling approach, but only sending data in one direction.

Thank you for your help.

I will use the 1-way approach because our 1D code doesn't have any option to get the stress in the pipe and we need to evaluate the stress in anchorages (with thermal stress and water hammer effect).

Also, you seems to say that the 1D code may be more precise for water hammer effect. So, I will make my sensitivity model until the result in CFX and the 1D code are similar.

Thank you again, your help is really appreciated.

Well, there is also dedicated software to calculate the pressure transients due to pressure waves such as 'WANDA', which makes things like this much easier. (automatic 'mesh' generation, correct wave speed based on pipe diameter, fluid properties, wall thickness and Youngs modulus).
(google for 'WANDA water hammer')