
[Sponsors] 
June 29, 2003, 20:48 
How to apply gravity to flow in CFX?

#1 
Guest
Posts: n/a

Hi all!
I have to consider the effect of gravity, but I don't know how. Can anybody tell me how to put it into practice? Thank you! Best regards! Miko 

June 29, 2003, 21:21 
Re: How to apply gravity to flow in CFX?

#2 
Guest
Posts: n/a

Hi Miko In order to incorporate gravity effects you will have to choose the flow to be buoyant. Then you can specify the gravity components.


June 29, 2003, 23:05 
Re: How to apply gravity to flow in CFX?

#3 
Guest
Posts: n/a

Hi Zahid!
Yes, but when I want to enable buoyant, it seems that only if domain model is multiphases or the fluid temperature is not constant the option is available. But what I need is only gravity, and I can ignore the change of temperature. What should I do? Thank you! Best regards! Miko 

June 30, 2003, 08:38 
Re: How to apply gravity to flow in CFX?

#4 
Guest
Posts: n/a

Miko, what exactly are you trying to model ? If you could give a little more detail then I'm sure people would be able to help. Bob


June 30, 2003, 10:38 
Re: How to apply gravity to flow in CFX?

#5 
Guest
Posts: n/a

Because buoyancy is temperature and pressure dependent, you can't enable buoyancy when your fluid is isothermal.
unless your flow is highspeed, use the thermal energy heat tranfer model. This will enable you to activate buoyancy and specify the gravity vector. Since you don't care about the temperature of the fluid, just specify the inlet temperature and make sure your boundaries are adiabatic. 

June 30, 2003, 10:43 
Re: How to apply gravity to flow in CFX?

#6 
Guest
Posts: n/a

u mean u dont want to solve energy eqn and wants the flow to be isothermal but still u want to specify gravity component.
if this is the situation, then when u specify let it take nonisothermal thing, but u can always modify parameter file. like in CFXTASCflow, if you specify TMPTRE = F in parameter file then inspite of specifying temperature change in GUI during problem specification, solver wont solve temperature and it would assume constant temperature. J 

June 30, 2003, 21:40 
Re: How to apply gravity to flow in CFX?

#7 
Guest
Posts: n/a

Dear Zahid, Bob, Louwrens and Centaur_ks,
Thank you all for giving me suggestion. In fact, what I am modeling is duct flow. The fluid is liquil metal, and besides Lorentz force concerned, I have to consider the effect of gravity. Liquid metal is single phase, so I needn't two or more phase. The physical image is as followed: liquid metal whose conductivity (denoted by c) is 2.878E+6 (ohm^1 m^1), flows in the insulator duct along Z axle, and the direction of external magnetic field (denoted by B) is X axle. We can know that in the Momentum equation Lorentz force Z component is c*B^2*w and Y component c*B^2*v where w and v mean the value of velocity along Z and Y axle, respectively, and B is equal to 1 (T). As for gravity, its form is density*g and direction is Y axle. In CFX, in order to add body force, I use CEL to creat values and expressions. For instance, I created bodyforce_z=c*B^2*w and bodyforce_y=c*B^2*vdensity*g with CEL, then I created a Fluid Subdomain named Bodyforce, enabled source of momentum in the subdomain, and specified it in the following way: Momentum: xcomp 0 kg m^2 s^2 Momentum: ycomp bodyforce_y Momentum: zcomp bodyforce_z After doing this, I run Solver, but I found it's difficult to converge. Can somebody give me some guideline and tell me how to add body force properly? 

July 4, 2003, 04:03 
Nearly the same problem as my one

#8 
Guest
Posts: n/a

Actually, I try to implement gravity to my diffusionconvection problem  without this force, the solver converges  with gravity  no chance at the moment. Let's wait and see  maybe I can give You an advice tomorrow.


July 4, 2003, 04:10 
Re: Nearly the same problem as my one

#9 
Guest
Posts: n/a

Hi Volker!
How did you implement the gravity? I think if the gravity is the only body force should be considered, it's easy. The only thing you should do to do is to creat a Fluid Subdomain and enable the Momentum source. You can use CEL or input the value of gravity there directly, I think. 

July 4, 2003, 12:11 
Re: How to apply gravity to flow in CFX?

#10 
Guest
Posts: n/a

Miko:
If you have a singlephase constantdensity flow, gravity is irrelevant and can be excluded from the simulation. The pressure then represents the 'motion pressure' which drives the flow. If for whatever reason you really want to include it, you can trick CFX into doing so by defining your density to be an expression, eg, 'Density = C*T/T', where C is the density you want. This will allow you to activate the buoyancy model. The interpretation of pressure then depends on your choice of buoyancy reference density; if you choose C, then you get exactly the same answer as if you excluded gravity. If you choose something other than C, then pressure will have a hydrostatic variation imposed on it. To get decent convergence, you will need to set pressure initial/boundary conditions which include the effect of this linear gradient. 

July 8, 2003, 05:33 
Re: How to apply gravity to flow in CFX?

#11 
Guest
Posts: n/a

Hi Phil!
Thank you! I think your suggestion is so useful. If gravity doesn't influence the velocity profile of the fluid when the fluid flows horizontally and gravity is vertical , I can ignore it. Right? 

November 21, 2017, 13:03 

#12  
Member
VB
Join Date: Jul 2016
Posts: 35
Rep Power: 3 
Quote:
Hi Phil, In the case of my fluid density varying over temperature, How do I avoid hydrostatic variation imposed when activating buoyancy model? I can give only one value for ref. buoyancy density but my fluid density is temperature dependent. I see (rho  rho_ref)g as the formula of the source term when we activate buoyancy model. 

November 22, 2017, 23:43 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,311
Rep Power: 110 
This thread is 14 years old. Phil is long since deceased.
But I can answer your question. If you have variable density then you inherently will have issues dealing with the hydrostatic component as the reference density cannot remove it. This is a fundamental implication of using variable density in a buoyant simulation. You are going to have to ensure that your simulation can handle the fact that the hydrostatic component will remain to some extent. This may affect your choice of boundary conditions. 

November 23, 2017, 04:05 

#14  
Member
VB
Join Date: Jul 2016
Posts: 35
Rep Power: 3 
Quote:


November 24, 2017, 05:09 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,311
Rep Power: 110 
Oh yes, you posted on that other thread on the streamlines at the outlet.
You had not correctly implemented the buoyancy reference condition if I remember correctly, so the hydrostatic component was not removed properly and was causing the strange streamlines. If you corrected your buoyancy model it should work. 

November 29, 2017, 16:17 

#16 
Member
VB
Join Date: Jul 2016
Posts: 35
Rep Power: 3 
Hi. Update: I could'nt fully resolve or remove the hydrostatic terms influence on the streamline. I could not adapt the reference buoyancy density to neutralize this term (rho  rho_ref)g. However I tried the simulation with deactivating it and it dosent have problem so I reduced my fluid region in a way it does not influence the result. Thank you for the suggestions. I appreciate it


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Different flow pattern between OpenFOAM and CFX  AirS  OpenFOAM  0  January 12, 2010 08:08 
mass flow in is not equal to mass flow out  saii  CFX  2  September 18, 2009 08:07 
Mass flow and UMom flow in CFX  Zhihua Xie  CFX  0  September 3, 2007 09:49 
Gravity flow  Sadhna  FLUENT  9  May 30, 2005 12:41 
Help: CFX for granular flow  Dejun Jing  CFX  3  July 16, 2002 04:45 