Hello everyone,

I have been reading with interest all the posts on effects of gravity and its modelling by CFX. I had posted a similar topic earlier. What I understood from the discussion was one doesn't need to be worried about gravity if the flow is single phase, and there are no temperature and density variations. I understood that CXF(I assume all the solvers TASCflow, CFX 5, 4) takes care of it and adjusts the pressure. I also read somewhere that for a gravity driven flow, one needs to add the pressure due to gravity(rho*g*h) to the pressure as solved by the code. I was a bit confused, and thought should write to this forum. If it takes care of gravity, how one should tell the code which way the gravity acts? I know if we use the buoyancy models, there is a place where we can specify the vectors, but I am not talking about buoyancy as there are no temperature or density variations in my flow which is, you guessed it, gravity driven.

Thanks and looking forward to hearing from you

Drona

1) What is your question/point?

2) You don't have to add rho*g*h. Previous discussions have made that clear.

Pascale Fonteijn

Hi Drona,

If your flow is gravity driven, there must be a density variation or multiple phases involved. Otherwise there is no force to drive the fluid.

What is the problem you are trying to solve?

Robin

Response to Pascale and Robin'n postings;

My problem is a water turbine. There is no density difference(at least not significant- i assume it's incompressible flow and no temperature variations either) and there is only one phase(liquid - at least that's the assumption I make for water flow). But water does flow. So are my assumptions wrong? I seem to be terribly confused here.

I want to simplify my question/point: How can I get the TASCflow to take into account the level difference (inlet at a higher level that outlet - normal for any water turbine case) withought having to use pressure difference based boundary conditions? I want to use mass flow as inlet condition to meet the design criteria.

Pacale, you say you don't need to add rho*g*h. But I quote the following from the discussions in this forum. It was in turn quoted from one of CFX manuals.

"Note that the Results File does not contain the hydrostatic contribution to pressure, and this should be added to obtain actual values of pressure relative to the Reference Pressure in these cases". I should be terribly mistaken somewhere.

Sorry, it's become a long messege again. I find it difficult to explain in very short messege. I am not sure if I am able to explain my problem.

Thanks for your responses and looking forward to hearing from you

Drona

Hi Drona,

You will not require buoyancy to model your flow through the turbine unless you are modeling cavitation (which implies a density/phase variation). You don't need the hydrostatic pressure contribution because it will not affect the turbine performance (again, unless you are accounting for cavitation).

To account for the level difference, set the total pressure at the inlet equal to...

<bi>PtotalIn = rho*g*(h_inlet - h_outlet) + PstaticOut</bi>

use an average static pressure outlet set to PstaticOut. This will give you the correct pressure drop to drive your flow.

When you post process your results, you may prefer to see the hydrostatic pressure included. The following TASCtool command will create the pressure field.

(assuming z is up and ZREF is a reference height of your choosing)

calc P_HYDROSTATIC = P + RHO*G*(ZREF-Z)

This will create a new scalar, P_HYDROSTATIC, which you may post-process to all your hearts desire.

Best regards, Robin

Hi Robin,

Thanks for the suggestion. I may have to add additional pressure due to velocity at the inlet(rho*v*v/2), as the acual inlet(which I am not modelling) is further away at a higher level(but is only contains a pipe, which can be calculated manually) and water is already at a certain velocity. That way I can also constrain the mass flow I guess. So I might have to add more rho*g*h(h is the additional height). Am I right?

Also, do I put PstaticOut as zero, because it opens to atmosphere?

Thanks a lot

Drona

Drona,

If you use the total pressure as I suggested, the inlet dynamics will already be included. If you have an additional length of pipe preceding your inlet you can account for it by providing the necessary drop in total pressure.

As for the velocity at the inlet, if your mass flow is constrained, then you will want to use a mass flow (or velocity) specified inlet or outlet (mass flow outlet is usually better than inlet).

If you are running Ptotal in -> Pstatic out, the important thing is the pressure drop. If you add atmospheric pressure to your outlet, just make sure you do the same to your inlet.

Remember: It's all relative!

Regards, Robin

Thanks Robin,

I will try to solve the problem and see what I get. I will let you know.

Thanks again for help. I may come back with more questions though!

Drona