# I can't break FLUENT

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

 February 17, 2016, 01:04 I can't break FLUENT #1 New Member   Mike Tree Join Date: Feb 2016 Location: Atlanta, GA Posts: 5 Rep Power: 3 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.

 February 17, 2016, 05:00 #2 Senior Member   Join Date: Nov 2013 Posts: 1,085 Rep Power: 14 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.

 February 17, 2016, 10:42 #3 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 1,886 Rep Power: 26 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.

February 17, 2016, 11:00
#4
New Member

Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 3
Quote:
 Originally Posted by pakk 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.

February 17, 2016, 11:16
#5
New Member

Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 3
Quote:
 Originally Posted by LuckyTran 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

 February 17, 2016, 11:47 #6 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 1,886 Rep Power: 26 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.

February 17, 2016, 11:58
#7
New Member

Mike Tree
Join Date: Feb 2016
Location: Atlanta, GA
Posts: 5
Rep Power: 3
Quote:
 Originally Posted by LuckyTran 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?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post bruce OpenFOAM Running, Solving & CFD 6 January 20, 2017 07:22 Chuck87 FLUENT 0 September 2, 2015 16:17 Steven Fluent UDF and Scheme Programming 4 September 20, 2013 16:30 herntan FLUENT 5 December 14, 2009 03:57 Lourival FLUENT 3 January 16, 2008 17:48

All times are GMT -4. The time now is 20:21.