|
[Sponsors] |
October 2, 2012, 16:01 |
InterFoam mesh dependency
|
#1 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
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? |
|
October 4, 2012, 03:45 |
|
#2 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
Hi
Do you have contact angle? |
|
October 4, 2012, 04:45 |
|
#3 |
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 22 |
This is probably due to spurious currents. It is known that they get worse on mesh refinement.
|
|
October 4, 2012, 08:16 |
|
#4 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
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 |
|
October 4, 2012, 09:39 |
|
#5 |
Member
Nicklas Linder
Join Date: Jul 2012
Location: Germany
Posts: 35
Rep Power: 14 |
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 12:13. |
|
October 6, 2012, 07:31 |
|
#6 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
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. |
|
October 6, 2012, 09:08 |
|
#7 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
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 |
|
October 7, 2012, 04:32 |
|
#8 |
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 |
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 in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM - An open-source implementation of quadrature-based moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. |
|
October 9, 2012, 07:57 |
|
#10 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
Hi
Would you please attach picture of bubbles on the mesh simultaneously. |
|
October 9, 2012, 09:44 |
|
#12 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
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? |
|
October 9, 2012, 11:33 |
|
#13 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
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? |
|
October 10, 2012, 06:18 |
|
#14 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
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. |
|
November 10, 2015, 15:42 |
|
#15 |
Member
Arsalan
Join Date: Jul 2014
Posts: 74
Rep Power: 12 |
Dear Nima,
I got same problem with interFoam, did you solve it ? please advise me. Thanks. |
|
Tags |
interfoam, mesh dependency |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Add Mesh Layers doesnt work on the whole surface | Kryo | OpenFOAM Meshing & Mesh Conversion | 13 | February 17, 2022 08:34 |
Problem: tetrahedral mesh and interFoam = bad results ? | querdynamik | OpenFOAM Running, Solving & CFD | 1 | October 10, 2015 15:17 |
[snappyHexMesh] external flow with snappyHexMesh | chelvistero | OpenFOAM Meshing & Mesh Conversion | 11 | January 15, 2010 20:43 |
interFoam with irregular Mesh | luther | OpenFOAM | 9 | August 14, 2009 08:43 |
DxFoam reader update | hjasak | OpenFOAM Post-Processing | 69 | April 24, 2008 02:24 |