CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

simpleFoam problem validating 3D pipe flow

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

Like Tree1Likes
  • 1 Post By romant

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 8, 2013, 04:14
Default simpleFoam problem validating 3D pipe flow
  #1
Member
 
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 9
inf.vish is on a distinguished road
Hi all,
I am facing difficulty in validating openfoam for a flow in a 3D pipe. The flow is laminar and the fluid is water. Inlet velocity is 1E-4 m/s. Length of pipe = 100mm and Diameter = 10mm. I am pretty sure my boundary conditions are correct since i am able to solve the same problem using 2D axisymmetric wedge (and the results conform with the Poiseuille's law).

I am attaching both the files. Please tell me where i am going wrong.
Use fluent3dMeshToFoam for converting the .msh mesh.

2D axisymmetric - https://docs.google.com/file/d/0B8wx...it?usp=sharing
3D pipe - https://docs.google.com/file/d/0B8wx...it?usp=sharing
inf.vish is offline   Reply With Quote

Old   August 8, 2013, 04:45
Default
  #2
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 371
Rep Power: 17
romant is on a distinguished road
could you please provide more information? maybe the problem can already be solved not having to run your cases.

1. What doesn't work?
2. What are your boundary conditions on the walls?


One thing you can do is build a pipe with blockmesh and validate the case there. It gives you good control over the mesh. I even remember someone posting a script or tool to make a simple pipe in blockmesh if you don't know how to make one yourself. Otherwise you can use swiftblock (help threads are here in the forum) http://openfoamwiki.net/index.php/Contrib/SwiftBlock to make a pipe.
__________________
~roman
romant is offline   Reply With Quote

Old   August 8, 2013, 04:57
Default
  #3
Member
 
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 9
inf.vish is on a distinguished road
Everything works. The solution even converges but the answers don't match with the theoretical values. The results i obtain from 2D axisymmetric case match the theoretical results. The results i obtain from 3D case do not. The problem is that the dimensions and transport properties are the same. so the solution shown by the two should be close.
The boundary conditions are as follow
U - inlet 10^-4 m/s, outlet zeroGradient, wall fixedValue uniform (0 0 0)
p - inlet zeroGradient, outlet fixedValue uniform 0, wall zeroGradient.
inf.vish is offline   Reply With Quote

Old   August 8, 2013, 05:03
Default
  #4
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Eindhoven, NL
Posts: 371
Rep Power: 17
romant is on a distinguished road
Do you mean theoretical values for a fully developed laminar flow? Have a look at your dimensions, the pipe is only 100 mm long and 10 mm in diameter, this means that even at the end of the 100 mm you only had 10 diameters development length.

If your velocity profile is flat at the entrance, you might not have a fully developed profile at the outlet, meaning that there will be discrepancies between theory and CFD. http://www.engineeringtoolbox.com/en...low-d_615.html
badwalgurpreet likes this.
__________________
~roman
romant is offline   Reply With Quote

Old   August 8, 2013, 05:09
Default
  #5
Member
 
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 9
inf.vish is on a distinguished road
Yes for a fully developed laminar flow. But the velocity is very small and if you look at the entrance region length given by the equation l_entrance = 0.06*Diameter*Re which gives me an entrance region length of 60mm which is less than 100mm and i get a fully developed flow at the outlet.
I am getting theoretically correct answers with 2D axisymmetric case if you can just open and see that file. The max velocity is 1.97e-4 and the corresponding pressure difference comes out to be around 3.2e-6 (kinematic pressure) which conforms with poiseuilles law.

Correct me if i am wrong.
inf.vish is offline   Reply With Quote

Old   August 9, 2013, 04:49
Default
  #6
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 526
Rep Power: 23
linnemann will become famous soon enough
Hi

Please run

Code:
transformPoints -scale "(0.001 0.001 0.001)"
on the 3d case.

The dimensions are 5x5x100m which should be 0.005x0.005x0.1m

Maybe also run

Code:
refineWallLayer -overwrite WALL 0.5
a few time to get better BL resolution at the wall.
Attached Images
File Type: jpg 2013-08-09-58-28-000051.jpg (23.9 KB, 90 views)
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   August 12, 2013, 00:18
Default
  #7
Member
 
Vishal
Join Date: Jul 2013
Posts: 73
Rep Power: 9
inf.vish is on a distinguished road
Thanks for pointing out the mistake Niels Nielsen!
The case is running properly now
inf.vish 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
Pipe flow with obstacle - HELP Min FLUENT 6 January 31, 2017 15:28
3D Swirl flow in the pipe: convergence problem Sachin U. Nimbalkar FLUENT 5 December 22, 2016 02:34
High speed compressible flow through pipe Munni Main CFD Forum 6 December 7, 2015 12:33
setup problems - LES pipe flow with cyclic BC (1) and direct mapped inlet (2) florian_krause OpenFOAM 22 June 13, 2013 22:25
problem on Laminar flow in a pipe Goutam OpenFOAM Running, Solving & CFD 4 March 20, 2012 11:13


All times are GMT -4. The time now is 15:23.