CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > General Forums > Main CFD Forum

Mass Flux Issues

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By sbaffini
  • 1 Post By arjun

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 26, 2019, 17:21
Post Mass Flux Issues
  #1
New Member
 
Join Date: Sep 2019
Posts: 3
Rep Power: 6
syotyy is on a distinguished road
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 k-Omega 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.
syotyy is offline   Reply With Quote

Old   September 27, 2019, 03:41
Default
  #2
New Member
 
Join Date: Jan 2015
Posts: 19
Rep Power: 11
el_mojito is on a distinguished road
Quote:
Originally Posted by syotyy View Post
I am wondering if my original assumption is correct or if there is something else I am missing here.

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.
el_mojito is offline   Reply With Quote

Old   September 27, 2019, 03:45
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,764
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by el_mojito View Post
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.



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.
FMDenaro is offline   Reply With Quote

Old   September 27, 2019, 08:04
Default
  #4
New Member
 
Join Date: Jan 2015
Posts: 19
Rep Power: 11
el_mojito is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
Be careful, syotyy wrote that the integral of the mass flux is zero, a fact that is definitely true!

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?



Quote:
Originally Posted by syotyy View Post
This means then, for any control surface within the domain, the mass flux integrated over that surface should always be zero.
el_mojito is offline   Reply With Quote

Old   September 27, 2019, 08:23
Default
  #5
New Member
 
Join Date: Sep 2019
Posts: 3
Rep Power: 6
syotyy is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
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.
Hi, thanks for your reply!
So based on your answer, I might have a couple of problems here.
1) I used exported cell-centered values and took the average flux between two adjacent cells as an approximate for the face value. Since I have a node-based solution, I have essentially interpolated (face) from an interpolant (my grid) of an interpolant (cell-centered) 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.
syotyy is offline   Reply With Quote

Old   September 27, 2019, 08:25
Default
  #6
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,764
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by el_mojito View Post
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?
I assumed a closed surface that is the boundary of a control volume, not an arbitrary single surface.
Let we wait for the details
FMDenaro is offline   Reply With Quote

Old   September 27, 2019, 08:29
Default
  #7
New Member
 
Join Date: Sep 2019
Posts: 3
Rep Power: 6
syotyy is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
I assumed a closed surface that is the boundary of a control volume, not an arbitrary single surface.
Yes, that is what I forgot to mention. The type of CS I am referring to will always enclose a finite volume in the domain.
syotyy is offline   Reply With Quote

Old   September 27, 2019, 08:39
Default
  #8
New Member
 
Join Date: Jan 2015
Posts: 19
Rep Power: 11
el_mojito is on a distinguished road
Quote:
Originally Posted by syotyy View Post
Yes, that is what I forgot to mention. The type of CS I am referring to will always enclose a finite volume in the domain.
Quote:
Originally Posted by FMDenaro View Post
I assumed a closed surface that is the boundary of a control volume, not an arbitrary single surface.
Let we wait for the details

Ah, I see. Then I simply misinterpreted your question.
el_mojito is offline   Reply With Quote

Old   September 27, 2019, 11:12
Default
  #9
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,764
Rep Power: 71
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by syotyy View Post
Hi, thanks for your reply!
So based on your answer, I might have a couple of problems here.
1) I used exported cell-centered values and took the average flux between two adjacent cells as an approximate for the face value. Since I have a node-based solution, I have essentially interpolated (face) from an interpolant (my grid) of an interpolant (cell-centered) 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.



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 post-processing code. You have to apply the same interpolant and numerical integral used in the code.
FMDenaro is offline   Reply With Quote

Old   September 30, 2019, 05:08
Default
  #10
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 2,152
Blog Entries: 29
Rep Power: 39
sbaffini will become famous soon enoughsbaffini will become famous soon enough
Send a message via Skype™ to sbaffini
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).
FMDenaro likes this.
sbaffini is offline   Reply With Quote

Old   September 30, 2019, 08:23
Default
  #11
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,273
Rep Power: 34
arjun will become famous soon enougharjun will become famous soon enough
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:
Originally Posted by sbaffini View Post
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).
FMDenaro likes this.
arjun is offline   Reply With Quote

Reply

Tags
rans modelling, reacting flow, steady state rans

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 07:34.