
[Sponsors] 
periodic straight tube flow, no mesh independent solution for pressure gradient 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 6, 2018, 13:24 
periodic straight tube flow, no mesh independent solution for pressure gradient

#1 
New Member
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8 
Dear all,
For a while I am struggeling to obtain a mesh independent solution using translational periodic boundary conditions for a straight 3d pipe, both laminar and turbulent. The goal is to invesigate by specifying a certain mass flow rate for a pipe with a helix structure (spiral offset) and study the pressure gradient for different helix geometries. For that I want to use periodic boundaries and only simulate a few pitches. But before that, I am struggeling to obtain an mesh independent solutions for a laminar and also a turbulent pipe flow. My diameter is D=5,3mm and the periodic length is L=10mm. I have an incompressible fluid (water) and use the SIMPLEC algorithm. I notice that for a constant mass flow rate and mesh refinement (1,5x in every direction) I do not obtain a mesh independent solution for the pressure gradient. My mesh is structured (O grid butterfly topology) and low Reynolds. For a laminar pipe flow I do obtain a hagenpoiseuille parabolic velocity profile, but the pressure gradient is not converging. All residuals are nicely converging to 1e5. For momentum I use second order upwind, second order for pressure, second order upwind for turbulence, Least squares cell based for gradient. Laminar periodic pipe flow: Turbulent periodic pipe flow using RNGkepsilon: I can not seem to find out what is the problem for the pressure gradient. I also checked for different partition setup, first I used metis decomposition and next I use decomposition along zaxis, so each processor only has two neighbors. It seem to influence the result, more osscilation, but still no assymptotic value. My definition of a mesh independent solution is that with increasing number of cells, the value of interest converge to an asymptotic value. Kind regards, Thijs 

May 6, 2018, 22:35 

#2 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,683
Rep Power: 66 
First, fits also my experience with turbulent flow in straight ribbed pipes.
However, I noticed that I was not achieving iterative convergence. That is, letting the simulation run for 100k or 1M iterations, the pressure gradient had very low frequency oscillations and the amplitude of these oscillations was more than the deviation in the pressure gradient vs mesh count. I think you have to give up the mindset that you are looking for mesh independence & instead call it by its proper name, mesh dependence. That is, you want monotonically asymptotic behavior where it doesn't exist. You should recalibrate your thinking in terms of asymptotic +/. I see people running into these situations more often nowadays, even at the AIAA CFD benchmarking workshops. 

May 7, 2018, 09:20 

#3  
New Member
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8 
Quote:


May 7, 2018, 09:45 

#4 
Senior Member
Kushal Puri
Join Date: Nov 2013
Posts: 182
Rep Power: 12 
Quote:


May 16, 2018, 03:25 

#5  
New Member
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8 
Quote:
I want to reply that I fixed the issue. The problem was in the SIMPLE algorithm to simulate a translational periodic flow. Mesh refinement did not result in a converging solution for the variable of interest. In my case the pressure gradient for simple pipe flow. I switched to a coupled solver, with the pseudo transient option and now I do get a converged solution for the pressure gradient in translational periodic flow. It is not clear to why the SIMPLE algorithm is not working properly and I do not have an clear answer for that. Notice that this result is just my observation and the used version of Fluent was v19.0 . With the coupled solver I also ran in a memory error:P But luckily running on multiple nodes fixed the issue. Kind regards, Thijs 

May 16, 2018, 09:04 

#6 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,683
Rep Power: 66 
You pulled a Millikan and you got lucky. If I change enough settings and collect enough eventually I find a bunch of data points that on a curve I've already drawn.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to set periodic boundary conditions  Ganesh  FLUENT  15  November 18, 2020 06:09 
pimpleFoam in OF1612 shows same time step twice in log file  shang  OpenFOAM Bugs  10  January 24, 2018 10:43 
[ANSYS Meshing] Solution to periodic boundary problem  SophieLee  ANSYS Meshing & Geometry  1  June 28, 2017 01:51 
Future CFD Research  Jas  Main CFD Forum  10  March 30, 2013 12:26 
no mesh independency of turbulent flow across tube bank  rasko  CFX  4  July 7, 2012 02:45 