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

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

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 6, 2018, 13:24
Default periodic straight tube flow, no mesh independent solution for pressure gradient
  #1
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8
thijs1909 is on a distinguished road
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 hagen-poiseuille parabolic velocity profile, but the pressure gradient is not converging. All residuals are nicely converging to 1e-5.

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 z-axis, 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
thijs1909 is offline   Reply With Quote

Old   May 6, 2018, 22:35
Default
  #2
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,683
Rep Power: 66
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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.
LuckyTran is offline   Reply With Quote

Old   May 7, 2018, 09:20
Default
  #3
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8
thijs1909 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
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.
I contacted ANSYS again while it is a very strange observation for a Hagen-poiseuille flow. If this very famous problem cannot be solved, I think it is very alarming.
thijs1909 is offline   Reply With Quote

Old   May 7, 2018, 09:45
Default
  #4
Senior Member
 
Kushal Puri
Join Date: Nov 2013
Posts: 182
Rep Power: 12
Kushal Puri is on a distinguished road
Quote:
Originally Posted by thijs1909 View Post
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 hagen-poiseuille parabolic velocity profile, but the pressure gradient is not converging. All residuals are nicely converging to 1e-5.

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 z-axis, 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
Sometimes with the refinement, specially in the structured mesh, quality of the mesh start degrading, that is also sometimes cause change in results with refinement. hope you have checked all the quality parameters for all the meshes and maintained same kind of quality in all meshes.
Kushal Puri is offline   Reply With Quote

Old   May 16, 2018, 03:25
Default
  #5
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 8
thijs1909 is on a distinguished road
Quote:
Originally Posted by Kushal Puri View Post
Sometimes with the refinement, specially in the structured mesh, quality of the mesh start degrading, that is also sometimes cause change in results with refinement. hope you have checked all the quality parameters for all the meshes and maintained same kind of quality in all meshes.
Hi,

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
thijs1909 is offline   Reply With Quote

Old   May 16, 2018, 09:04
Default
  #6
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,683
Rep Power: 66
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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.
LuckyTran is offline   Reply With Quote

Reply

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
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


All times are GMT -4. The time now is 07:12.