CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions

[ImmersedBoundary] Problem with immersed boundary mesh and geometry

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 21, 2016, 04:18
Default Problem with immersed boundary mesh and geometry
  #1
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
Dear All,
I work with immersed boundary to develop new class of dynamic mesh.
The problem that I have is previously reported on the forum. The immersed boundary is not robust and with small changes in the *.stl file will crash.
The Fatal Error that I receive is mainly:
"Can't find nearest triSurface point for cell ... "

I tried all tutorials available in the latest versions, they working well, while small change in the geometry, like replacing the cylinder with an airfoil, or sphere with a vane leads to an Fatal Error.

I changed the solver, codes, radiusFactor and etc, the outcome was not interesting.

Is there anybody who has debugged the code and knows anything more than me!
Bests
Ardalan
Ardali is offline   Reply With Quote

Old   November 21, 2016, 04:46
Default
  #2
Senior Member
 
Join Date: Jan 2014
Posts: 163
Rep Power: 8
hxaxtma is on a distinguished road
From my experience this is only caused by a too coarse background mesh. Just try to create a more densed mesh in your area of interest and try it again.
hxaxtma is offline   Reply With Quote

Old   November 21, 2016, 04:59
Default
  #3
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
Thanks for your reply,
As you know, "refineImmersedBoundaryMesh.H" is available and a utility can be written to make the resolution finer locally, or an other way, make it finer globally using "BlockMeshDict".

I went up to more than 2.5 million cells , but still it does not work!!
In which cases you succeeded to run the simulations? I mean how complex was your *.stl file.

For double checking, I generate *.stl file from surface mesh in ICEM and convert it to *.ftr whit surfaceConvert!
Bests
Ardalan
Ardali is offline   Reply With Quote

Old   November 21, 2016, 05:07
Default
  #4
Senior Member
 
Join Date: Jan 2014
Posts: 163
Rep Power: 8
hxaxtma is on a distinguished road
If you send me your stl file and your blockMeshDict I will have a look
hxaxtma is offline   Reply With Quote

Old   November 21, 2016, 05:17
Default
  #5
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
Thanks,
Please download the case:
https://www.dropbox.com/s/fux08tj0gv...annel.zip?dl=0

I use constant/triSurface/body3D.stl
Ardalan
Ardali is offline   Reply With Quote

Old   November 21, 2016, 08:10
Default
  #6
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,334
Blog Entries: 6
Rep Power: 39
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,

you are using immersedBoundary in which version? I think foamExtend. Last week in the PFAU in Vienna we had a talk about a new implementation of the immersedBoundary theory in OpenFOAM. The guys were from Graz (Austria). Maybe it is possible to get the source code. As far as I understood, they do not have any problems.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   November 21, 2016, 08:47
Default
  #7
Senior Member
 
Join Date: Jan 2014
Posts: 163
Rep Power: 8
hxaxtma is on a distinguished road
Well I checked your case and it worked for me,
so maybe you are missing some step in the pre processing,

1) Convert your stl to ftr with surfaceFeatureEdges *.stl *.ftr -angle 30
2) Run blockMesh
3) Add
ibSphere
{
type immersedBoundary;
nFaces 0;
startFace 263100;
internalFlow no;
}

to boundary file, note startFace must be equal to your first BC when running blockMesh
4) As I already mentioned, your basemesh resolution near the IB Area is too low, so improve your blockMeshDict

5) Run potentialIbFoam
6) Run your Ib Solver

The picture below shows the refined IBCells with refineImmersedBoundary -ibCells, of course the resolution is still not adequat
Attached Images
File Type: png ib.png (16.5 KB, 63 views)
hxaxtma is offline   Reply With Quote

Old   November 21, 2016, 08:48
Default
  #8
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
Hi Tobias,
Thank you.
Yes I use FOAM_Extended-4.0 and the latest release.
It sounds great if their code works fine.
Is there any possibility to have access to the code?
What is the problem with current code?
Bests
Ardalan
Ardali is offline   Reply With Quote

Old   November 21, 2016, 08:48
Default
  #9
Senior Member
 
Join Date: Jan 2014
Posts: 163
Rep Power: 8
hxaxtma is on a distinguished road
Quote:
Originally Posted by Tobi View Post
Hi,

you are using immersedBoundary in which version? I think foamExtend. Last week in the PFAU in Vienna we had a talk about a new implementation of the immersedBoundary theory in OpenFOAM. The guys were from Graz (Austria). Maybe it is possible to get the source code. As far as I understood, they do not have any problems.
@Tobi,
who exactly pronounced the IB solver? I am highly interested in*g*
hxaxtma is offline   Reply With Quote

Old   November 21, 2016, 09:15
Default
  #10
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,334
Blog Entries: 6
Rep Power: 39
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

I don't know if there is any problem in the IB from the extend project. However, Federico Municchi from TUGraz hold some presentation about Fictitious Domain and immersed Boundary methods in OpenFOAM.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   November 21, 2016, 10:17
Default
  #11
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
Quote:
Originally Posted by hxaxtma View Post
Well I checked your case and it worked for me,
so maybe you are missing some step in the pre processing,

1) Convert your stl to ftr with surfaceFeatureEdges *.stl *.ftr -angle 30
2) Run blockMesh
3) Add
ibSphere
{
type immersedBoundary;
nFaces 0;
startFace 263100;
internalFlow no;
}

to boundary file, note startFace must be equal to your first BC when running blockMesh
4) As I already mentioned, your basemesh resolution near the IB Area is too low, so improve your blockMeshDict

5) Run potentialIbFoam
6) Run your Ib Solver

The picture below shows the refined IBCells with refineImmersedBoundary -ibCells, of course the resolution is still not adequat
Thank you for your time,
Would you please send me the blockMeshDict that you made?
I could not run the case even with 4 times finer resolution.
Bests
Ardalan
Ardali is offline   Reply With Quote

Old   November 21, 2016, 12:52
Default
  #12
Senior Member
 
Join Date: Jan 2014
Posts: 163
Rep Power: 8
hxaxtma is on a distinguished road
Here is your working case
1) run blockMesh
2) copy boundary from case folder to polyMesh folder
3) run refineImmersedBoundary -ibCells
4) run potentialIbFoam
5) Have fun!
Attached Files
File Type: gz sphereInChannel_ibrunshere.tar.gz (76.1 KB, 30 views)
hxaxtma is offline   Reply With Quote

Old   November 22, 2016, 09:57
Default
  #13
New Member
 
Ardalan
Join Date: Jul 2012
Location: Gothenburg, Sweden
Posts: 29
Rep Power: 9
Ardali is on a distinguished road
The problem was the compilation of Foam-extended-4.0. If you use the latest version you might have a problem with immersed boundary. Even some tutorials do not work properly. That is safer to stick to the previous version, Foam-Extended-3.2.
If you are going to use the latest version, there is an update released last week. consider it.
The problem is reported and discussed with administration!

Thank you all to replay and let us find the problem.
One more problem that still exists, is IbMask does not correspond with the geometry. Please follow the case shared in previous message.

Ardalan
Ardali 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
Question about adaptive timestepping Guille1811 CFX 25 November 12, 2017 18:38
Problem in setting Boundary Condition Madhatter92 CFX 12 January 12, 2016 05:39
Problem with geometry - concentric cylinders Rhoddwen OpenFOAM Running, Solving & CFD 0 December 15, 2014 10:22
[Gmsh] 2D Mesh Generation Tutorial for GMSH aeroslacker OpenFOAM Meshing & Mesh Conversion 12 January 19, 2012 04:52
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 16:32.