
[Sponsors] 
November 20, 2001, 06:42 
On gravity modelling...

#1 
Guest
Posts: n/a

Sponsored Links
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 

Sponsored Links 
November 20, 2001, 18:26 
Re: On gravity modelling...

#2 
Guest
Posts: n/a

1) What is your question/point?
2) You don't have to add rho*g*h. Previous discussions have made that clear. Pascale Fonteijn 

November 20, 2001, 21:37 
Re: On gravity modelling...

#3 
Guest
Posts: n/a

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 

November 21, 2001, 05:44 
Re: On gravity modelling...

#4 
Guest
Posts: n/a

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 

November 21, 2001, 22:36 
Re: On gravity modelling...

#5 
Guest
Posts: n/a

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*(ZREFZ) This will create a new scalar, P_HYDROSTATIC, which you may postprocess to all your hearts desire. Best regards, Robin 

November 22, 2001, 05:21 
Re: On gravity modelling...

#6 
Guest
Posts: n/a

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 

November 22, 2001, 09:34 
Re: On gravity modelling...

#7 
Guest
Posts: n/a

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 

November 22, 2001, 11:28 
Re: On gravity modelling...

#8 
Guest
Posts: n/a

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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
gravity current modelling  asistas  FLUENT  10  September 24, 2011 22:43 
Urgent....Help on modelling variable gravity  sabbasi_mr  Main CFD Forum  0  December 2, 2009 01:03 
how to consider gravity in CFX  shrimp  CFX  4  September 8, 2008 20:41 
Help: gravity in CFX  Dejun Jing  CFX  2  July 22, 2002 08:58 
Gravity modelling  Drona  CFX  7  August 10, 2001 07:00 
Sponsored Links 