
[Sponsors] 
September 26, 2019, 17:21 
Mass Flux Issues

#1 
New Member
Join Date: Sep 2019
Posts: 3
Rep Power: 7 
Hi, I'm new to CFD and really confused about the result I'm getting from exported Fluent data.
This is more or less a general question and not specifically addressed at the software. I have a verified solution of a reacting flow inside a complex domain with multiple inlets. From what I understand, the RANS kOmega realizable solutions are steady. This means then, for any control surface within the domain, the mass flux integrated over that surface should always be zero. Since integration over my arbitrary volumes is easier implemented outside of Fluent, I exported the velocity and density field solutions and interpolated those values over a uniform grid. Then I summed the mass flux at each face that lies between two cells belonging to different volumes. Long story short, I am not getting zero integrated mass flux for any volume I have assigned. I am wondering if my original assumption is correct or if there is something else I am missing here. Your help would be very much appreciated. 

September 27, 2019, 03:41 

#2  
New Member
Join Date: Jan 2015
Posts: 19
Rep Power: 11 
Quote:
Your assumption is wrong. Why would the mass flux have to be zero in a stationary flow?! Mass flux is rho*u*A. This can only be zero if either rho, u, or A are zero. A = 0 is useless, the massflux over zero space is of course zero rho = 0 is physically impossibe u = 0 means the fluid is stationary So your assumption is true if the fluid is at rest everywhere in your domain. If it's not your assumption is (very) wrong. 

September 27, 2019, 03:45 

#3  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,839
Rep Power: 73 
Quote:
Be careful, syotyy wrote that the integral of the mass flux is zero, a fact that is definitely true! The problem is that the discrete conservation is verified only for the node where the computation is really performed. So the consistence check must be done according to the original method of computation. 

September 27, 2019, 08:04 

#4  
New Member
Join Date: Jan 2015
Posts: 19
Rep Power: 11 
Quote:
Am I'm misunderstanding his question? Why should the mass flux integrated over any surface be zero? If you have a uniform free stream with u=1 and rho=1 and a control surface perpendicular to the flow, the integrated mass flux is not zero? 

September 27, 2019, 08:23 

#5  
New Member
Join Date: Sep 2019
Posts: 3
Rep Power: 7 
Quote:
So based on your answer, I might have a couple of problems here. 1) I used exported cellcentered values and took the average flux between two adjacent cells as an approximate for the face value. Since I have a nodebased solution, I have essentially interpolated (face) from an interpolant (my grid) of an interpolant (cellcentered) of the node values. 2) I haven't checked the continuity residuals of my solution in a while. From what you're suggesting, should the residual have converged, my mesh node field will be steady and therefore yield the zero face flux over any surface. However, the same cannot be guaranteed if I then interpolated those values over to a coarser, uniform grid. 

September 27, 2019, 08:25 

#6  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,839
Rep Power: 73 
Quote:
Let we wait for the details 

September 27, 2019, 08:29 

#7 
New Member
Join Date: Sep 2019
Posts: 3
Rep Power: 7 

September 27, 2019, 08:39 

#8  
New Member
Join Date: Jan 2015
Posts: 19
Rep Power: 11 
Quote:
Quote:
Ah, I see. Then I simply misinterpreted your question. 

September 27, 2019, 11:12 

#9  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,839
Rep Power: 73 
Quote:
First of all, in your code you have to set the correct convergence criterion that ensures the continuity is statisfied at the steady state, that is Int[S]n.(rho v)dS =0 is satisfied in discrete sense. But that does not ensure you can have the same level of residual if you adopt a different scheme to compute the integral in a postprocessing code. You have to apply the same interpolant and numerical integral used in the code. 

September 30, 2019, 05:08 

#10 
Senior Member

As mentioned by Filippo, what in a Finite Volume (steady or incompressible) computation has a null (actually order of the residual) integral over closed surfaces is the actual mass flux used to discretize the continuity equation, because that is the entity that enters the continuity equation whose residual you eventually drive to 0 with the iterations.
Said otherwise, you know that a certain integral goes to zero exactly because you used that integral = 0 as one of your equations. So in order for you to verify this you should have access to the exact same terms composing that equation. In theory this is very hard to do because it might depend from an infinity of details you don't know of. In practice, Fluent stores these mass fluxes for every face, both interior and boundary ones, so you can export them directly (but you need to be aware of the sign convention used by Fluent to avoid mistakes). 

September 30, 2019, 08:23 

#11  
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,283
Rep Power: 34 
I add little bit to it:
1. The interpolated velocity to the fluent may not be the same as you expect them to be. 2. The flux for Fluent also accounts for Chie and Chow terms. These are pretty much always non zero in good part of the domain. Quote:


Tags 
rans modelling, reacting flow, steady state rans 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Problem with mass flux calculation in libsimpleFunctionObjects.so  BlnPhoenix  OpenFOAM Running, Solving & CFD  1  June 24, 2017 15:36 
Keeping inlet mass flux the same as outlet mass flux in an water tank  vaibhav402  Main CFD Forum  0  October 13, 2015 03:02 
Mass flux as a function of pressure  robin_dlc  Fluent UDF and Scheme Programming  2  April 13, 2014 13:15 
Instability introduced by using mutRoughWallFunctions?  AlexC  OpenFOAM Running, Solving & CFD  1  March 18, 2014 14:14 
Question about heat transfer coefficient setting for CFX  Anna Tian  CFX  1  June 16, 2013 06:28 