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

I can't break FLUENT

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 17, 2016, 01:04
Question I can't break FLUENT
  #1
New Member
 
Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 2
treem22 is on a distinguished road
I cannot seem to force FLUENT to diverge. I realize this is a bit counter-intuitive, so let me explain.

I have a pipe flow for which I have specified a mass flow inlet boundary condition at one end and wall boundary conditions everywhere else, including what would normally be the pipe outflow. Running a steady pressure-based solver with coupled pressure-velocity coupling with least squares cell based, second order, and second order upwind for gradient, pressure, and momentum spatial discretizations, respectively, results in a CONVERGED SOLUTION!

Of course, a converged solution doesn't guarantee a physically accurate solution. I explored the solution with some monitors which verified that my mass flow inlet boundary condition is as defined, the mass of the entire fluid volume is steady, and the spatially mean velocity magnitude of the fluid volume is steady as well. Plotting the velocity vectors shows zero velocity at the far wall (where the pipe outlet should normally be).

Now, no one in their right mind would accept the solution I receive because it makes no sense. I am simply confused that FLUENT gives a solution at all. What am I not understanding about FLUENT'S continuity convergence? Shouldn't my fluid volume mass grow continually and prevent continuity convergence?

Ultimately, I ran this simulation as a misguided effort to initialize a 2-way FSI case with FLUENT and ANSYS Mechanical via system coupling, but now my very understanding of fluid dynamics is crumbling. Any help will be appreciated.
treem22 is offline   Reply With Quote

Old   February 17, 2016, 05:00
Default
  #2
Senior Member
 
Join Date: Nov 2013
Posts: 943
Rep Power: 13
pakk will become famous soon enough
Interesting situation... What does your mass flux report say? I hope there the net mass flux is not close to zero, but (almost) equal to your inflow, but it is good to check.

And what do you call "converged solution"? The standard fluent settings for continuity residual < 0.001? In my opinion, for simple problems this number should be much smaller.
pakk is offline   Reply With Quote

Old   February 17, 2016, 10:42
Default
  #3
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
LuckyTran will become famous soon enough
One thing to note is that the mass-flow inlet does not enforce a uniform mass flux so it's possible to have some outflow (which may be doing some funny things to save the simulation).

Try using a velocity inlet instead of a mass-flow inlet to see if you can get the velocity inlet to diverge.
LuckyTran is offline   Reply With Quote

Old   February 17, 2016, 11:00
Default
  #4
New Member
 
Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 2
treem22 is on a distinguished road
Quote:
Originally Posted by pakk View Post
Interesting situation... What does your mass flux report say? I hope there the net mass flux is not close to zero, but (almost) equal to your inflow, but it is good to check.

And what do you call "converged solution"? The standard fluent settings for continuity residual < 0.001? In my opinion, for simple problems this number should be much smaller.
My mesh has three boundary surfaces (pipe inlet, pipe outlet, pipe wall) and one interior volume (int_fluid). A surface monitor of the pipe inlet shows steady 0.01 kg/s. A surface monitor of the pipe outlet (set as a wall bc) shows a steady 0.0 kg/s. A surface monitor of the pipe wall (set as a wall bc) shows a steady 0.0 kg/s. A surface monitor of the int_fluid surface converges to a mass flow of -0.025 kg/s. This last surface monitor seems fishy...

My convergence criteria are set at absolute residuals <1e-07 for continuity and all three velocity directions.

For reference, my total mesh volume is 2.206e-05 m3 and my fluid density is 1060 kg/m3, so the total mesh mass should be around 0.0234 kg.
treem22 is offline   Reply With Quote

Old   February 17, 2016, 11:16
Default
  #5
New Member
 
Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 2
treem22 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
One thing to note is that the mass-flow inlet does not enforce a uniform mass flux so it's possible to have some outflow (which may be doing some funny things to save the simulation).

Try using a velocity inlet instead of a mass-flow inlet to see if you can get the velocity inlet to diverge.
Ran the same simulation with a constant velocity inlet of ~1.86e-03 m/s to match the mass flux inlet condition based on fluid density and inlet area. This simulation converges (< 1e-07) in fewer iterations. It's mass flux report is as follows:

Mass Flow Rate (kg/s)
-------------------------------- --------------------
inlet_vel 0.00099999993
interior-fluid -0.0029626614
outlet_wall -0
wall -0
---------------- --------------------
Net 0.00099999993
treem22 is offline   Reply With Quote

Old   February 17, 2016, 11:47
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,372
Rep Power: 20
LuckyTran will become famous soon enough
I am concerned that your simulation actually calculated and didn't throw some type of floating point error or divergence error or divergence in amg solver error

However, I am not surprised that continuity residual criteria is met because of the way the continuity residual is calculated. The continuity residual is normalized by the worst residual in the first 5 iterations, and if the worst residual is very bad then the continuity residual can decrease, slightly better than very bad is still better. Dividing a large number by a very very large number results in a small number.

I would focus on the detailed velocity field and figuring out what doesn't make sense and I wouldn't give any attention to the residual.
LuckyTran is offline   Reply With Quote

Old   February 17, 2016, 11:58
Default
  #7
New Member
 
Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 2
treem22 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
I am concerned that your simulation actually calculated and didn't throw some type of floating point error or divergence error or divergence in amg solver error

However, I am not surprised that continuity residual criteria is met because of the way the continuity residual is calculated. The continuity residual is normalized by the worst residual in the first 5 iterations, and if the worst residual is very bad then the continuity residual can decrease, slightly better than very bad is still better. Dividing a large number by a very very large number results in a small number.

I would focus on the detailed velocity field and figuring out what doesn't make sense and I wouldn't give any attention to the residual.
I read up on the continuity residual and realized the default was to normalize by the worst residual in the first 5 iterations, so I turned off normalization. My residuals are also not scaled. Re-running the simulation with normalized, unscaled residuals means I converge at 5e-06 instead of 1e-07. Re-running the simulation with normalize, globally scaled residuals means I converge at 3e-04. Can anyone provide any more insight based off this information?
treem22 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fluent crash on writing data file after thousand iterations Chuck87 FLUENT 0 September 2, 2015 16:17
heat transfer with RANS wall function, over a flat plate (validation with fluent) bruce OpenFOAM Running, Solving & CFD 5 September 25, 2013 04:40
Two questions on Fluent UDF Steven Fluent UDF and Scheme Programming 4 September 20, 2013 16:30
Fluent 12.0 is worst then Fluent 6.2 herntan FLUENT 5 December 14, 2009 03:57
Problems in lauching FLUENT Lourival FLUENT 3 January 16, 2008 17:48


All times are GMT -4. The time now is 10:09.