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

InterFoam mesh dependency

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2012, 15:01
Default InterFoam mesh dependency
  #1
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Hello Friends
i made a simulation by InterFoam for bubble rising in stagnant liquid,
it seems solvers result is mesh dependent and make mesh refined does not make it free from mesh?
has any body similar experience with interFoam?
nimasam is offline   Reply With Quote

Old   October 4, 2012, 02:45
Default
  #2
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hi
Do you have contact angle?
ata is offline   Reply With Quote

Old   October 4, 2012, 03:45
Default
  #3
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
This is probably due to spurious currents. It is known that they get worse on mesh refinement.
Bernhard is offline   Reply With Quote

Old   October 4, 2012, 07:16
Default
  #4
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Quote:
Originally Posted by ata View Post
Hi
Do you have contact angle?
no i dont have

however to make it much more clear i put here the result of an spherical bubble rising in stagnant liquid for different mesh,shape is the same but final position in the same time is deferent!

Also, to calculate the terminal velocity of bubble, i calculate the mass gravity of bubble center, then i calculate the slope of mass gravity position in different time,

terminal velocity for different mesh is:
case: terminal velocity (m/s)
40: 0.036
80: 0.030
160: 0.024
320: 0.016
Attached Images
File Type: jpg 40.jpg (8.5 KB, 75 views)
File Type: jpg 80.jpg (8.6 KB, 57 views)
File Type: jpg 160.jpg (8.6 KB, 54 views)
File Type: jpg 320.jpg (8.8 KB, 63 views)
Attached Files
File Type: zip spherical40.zip (24.7 KB, 13 views)
nimasam is offline   Reply With Quote

Old   October 4, 2012, 08:39
Default
  #5
Member
 
Nicklas Linder
Join Date: Jul 2012
Location: Germany
Posts: 33
Rep Power: 5
nlinder is on a distinguished road
Hi Nima,

I have several (!) cases where I experience the same problems. Droplets, bubbles with or without contact to the wall, hex tet or poly mesh, you name it.

I did not yet find out where it exactly comes from, but I hope to figure it out some time

Just want to let you know, that you are not the only person having these problems! I'll let you know if I have anything new.

Edit: Check also the pressure-field in some cases, they differed extremely from each other due to mesh refinement!

regards
Nicklas

Last edited by nlinder; October 4, 2012 at 11:13.
nlinder is offline   Reply With Quote

Old   October 6, 2012, 06:31
Default
  #6
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hi Nima
Is this a symmetry BC? If yes this is numerically similar to normal contact angle.Would you please examine with the complete 2-D domain and let me know the results.
ata is offline   Reply With Quote

Old   October 6, 2012, 08:08
Default
  #7
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
nope it is axisymetric modeling, so frontAndBack are wedge and axis is empty!
you can find the case in above attachment, but i will try it with 2D simulation
nimasam is offline   Reply With Quote

Old   October 7, 2012, 03:32
Default
  #8
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
As suggested by Ata, could you try your case considering a planar 2D simulation with the whole bubble, and see if the problem persists?
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 8, 2012, 18:45
Default
  #9
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Hello
i made a simulation of 2D bubble rising, it seems problem is there:
case: terminal velocity {m/s}
40: 0.0486
80: 0.0411
160: 0.0377
Attached Images
File Type: jpg 40.jpg (11.2 KB, 33 views)
File Type: jpg 80.jpg (9.0 KB, 29 views)
File Type: jpg 160.jpg (11.1 KB, 27 views)
nimasam is offline   Reply With Quote

Old   October 9, 2012, 06:57
Default
  #10
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hi
Would you please attach picture of bubbles on the mesh simultaneously.
ata is offline   Reply With Quote

Old   October 9, 2012, 08:38
Default
  #11
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
whats your mean ata? do you want surface plot with edge to see mesh?
the mesh is uniform hexahedral
nimasam is offline   Reply With Quote

Old   October 9, 2012, 08:44
Default
  #12
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hi
Yes. I want to see your mesh resolution.
An other issue. How much is your density and viscosity ratio? How much is the capillary number?
ata is offline   Reply With Quote

Old   October 9, 2012, 10:33
Default
  #13
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,123
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
Hi
it has been solved with finer mesh for 2D case, this time i examined (320x1600) and terminal velocity was 0.0362 {m/s}, so based on previous result in above post, the geometry with 160x800 is suitable for simulation, so the cell size is about 2.8e-5 {m} but question is remained,
1-why axisymetric modeling shows dependent result?
2-is there any way to solve this problem for axisymetric domain?
3-is there any method which can avoid us from this very fine mesh and give us reasonable result in coarser mesh?
Attached Images
File Type: jpg 320.jpg (7.8 KB, 31 views)
Attached Files
File Type: zip 2Dspherical40.zip (11.8 KB, 13 views)
nimasam is offline   Reply With Quote

Old   October 10, 2012, 05:18
Default
  #14
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hi
1-Because in the axisymetric case you really simulate a bubble near the wall with 90 degree contact angle.
2-AFAIK nope.
3-Use a more precise scheme.
ata is offline   Reply With Quote

Reply

Tags
interfoam, mesh dependency

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
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
Problem: tetrahedral mesh and interFoam = bad results ? querdynamik OpenFOAM Running, Solving & CFD 0 June 4, 2010 09:43
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
interFoam with irregular Mesh luther OpenFOAM 9 August 14, 2009 07:43
DxFoam reader update hjasak OpenFOAM Post-Processing 69 April 24, 2008 01:24


All times are GMT -4. The time now is 06:53.