CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: snappyHexMesh and Others

multiple regions

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

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 15, 2013, 10:33
Default
  #21
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by wyldckat View Post
Hi Tobi,

My guess is that the base mesh needs a little bump in one of the directions, because an edge might be in the wrong place, leading snappy to have difficulties aligning the final mesh onto the surface of the pipes.

Best regards,
Bruno
Hi Bruno

thanks for your answer. Can you explain the quoted sentence of you in a other way? What do you mean with "bump" ?

Tobi
Tobi is offline   Reply With Quote

Old   February 15, 2013, 11:24
Default
  #22
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,525
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Tobi,

Quote:
Originally Posted by Tobi View Post
thanks for your answer. Can you explain the quoted sentence of you in a other way? What do you mean with "bump" ?
Sorry, I should have been more clearer. I meant "by bump" that you should try and shift the edges a few millimetres or centimetres.
You can do this, for example:
  • By adding 1 more cell on each direction in blockMesh.
  • And/or extending or reducing the length of the limits of the base mesh.
Best regards,
Bruno

PS: Moved aerogt3's post to here: Multiple regions with a porous zone

Last edited by wyldckat; February 15, 2013 at 11:28. Reason: added PS...
wyldckat is offline   Reply With Quote

Old   February 15, 2013, 14:50
Default
  #23
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno

I played a bit with the whole thing.
Here are three pics of the problem zones (red).

Tomorrow I ll try:

- refine the mesh there more
- refine the STL more
- changing snap controls (but what setting?)
- changing mesh quality parameters (but what parameter?)

Tobi
Attached Images
File Type: jpg 1.jpg (51.4 KB, 57 views)
File Type: jpg 2.jpg (86.1 KB, 52 views)
File Type: jpg 3.jpg (58.2 KB, 44 views)

Last edited by Tobi; February 16, 2013 at 12:07. Reason: forget pictures
Tobi is offline   Reply With Quote

Old   February 17, 2013, 07:05
Default
  #24
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno


I played a bit with the s ettings but the problem still exists.

To refine the STL does not make any difference. Further more using a accurate cell refinement from (3 3) to (4 4) does not make any differences.

I also tried so make the background cell one or a few cells more to change the lines in that section ... welll - that does not work too.


I played a bit with the snapControls but the problem still occures.
Now I am trying to make a new case in which I am trying something.

If its working I ll let you know it.
Tobi is offline   Reply With Quote

Old   February 17, 2013, 07:41
Default
  #25
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,525
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Tobi,

I forgot to mention this here, but have you tried using SwiftBlock and SwiftSnap to help prepare the mesh? And have you check the presentation "A Comprehensive Tour of snappyHexMesh" for more ideas?

Since yesterday I've been playing around with snappyHexMesh and porous zones and I haven't managed to get very far as well. But I did things manually, i.e. without the help of SwiftBlock and SwiftSnap...

Good luck!
Bruno
wyldckat is offline   Reply With Quote

Old   February 17, 2013, 08:09
Default
  #26
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by wyldckat View Post
Hi Tobi,

I forgot to mention this here, but have you tried using SwiftBlock and SwiftSnap to help prepare the mesh? And have you check the presentation "A Comprehensive Tour of snappyHexMesh" for more ideas?

Since yesterday I've been playing around with snappyHexMesh and porous zones and I haven't managed to get very far as well. But I did things manually, i.e. without the help of SwiftBlock and SwiftSnap...

Good luck!
Bruno
Hi Bruno,

I ll have a look at switft* and share my results.
The new case and my new idea is not working. But the meshing in my testcase is been very far ... still there is the problem with the single cells and the additional regions I get.

I know the documentation of sHM and the slides are very good.
Tobi is offline   Reply With Quote

Old   February 19, 2013, 11:46
Default
  #27
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno,

1. I make my backgroundmesh with Salome Meco.
2. I tried everything in:
- changing snapping parameters
- changing all quality parameters
- changing backgroundmesh
- changing refinement levels

- - - - - - - - - - - - - - - - - - - - - - - - - - -
Problem still persists.

If I make a finer mesh in the region of the pipes I get more and more "domains*". A coarsar mesh works better (i dont know why).

I have a setting now in which I only get one cell into a other domain. With these setting I played with the snap and quality parameters. The one cell is there all the time.

At the moment I am out of ideas and `ll leave that topic open.
Maybe I find a day when god tells me the solution

Thanks for all your help!
Tobi is offline   Reply With Quote

Old   February 19, 2013, 13:37
Default
  #28
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno and all other guys,

I think I have solved the problem.

If you are using a complex geometry like I do you have to declare all walls which belong to a interface with the same refinement level.

So you have to use STL with regions. I ll test it now with a complexer mesh system but I think its working ...

Last edited by Tobi; February 19, 2013 at 14:36.
Tobi is offline   Reply With Quote

Old   February 19, 2013, 15:48
Default
  #29
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Perfect!

Code:
created 'test.OpenFOAM'
created 'test{domain0}.OpenFOAM' 
created 'test{kanal1}.OpenFOAM'
created 'test{kanal2}.OpenFOAM'
created 'test{luftkanal}.OpenFOAM'
created 'test{rohr1}.OpenFOAM'
created 'test{rohr2}.OpenFOAM'
created 'test{rohr3}.OpenFOAM'
created 'test{rohr4}.OpenFOAM'
created 'test{rohr5}.OpenFOAM'
created 'test{rohr6}.OpenFOAM'
wyldckat likes this.

Last edited by Tobi; February 19, 2013 at 16:54.
Tobi is offline   Reply With Quote

Old   February 19, 2013, 17:40
Default
  #30
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

I ll tell you how to mesh a complex geomety with several and seperated regions with snappyHexMesh.


Very important
- - - - - - - - - - - - - - - - - -
like in the snappyMultiRegion tutorial you have to build your STL files with regions. Therefor you should have the interfaces named as a single region in the STL file (e.g. in the attachement).

- The picture I added is important for the "splitMeshRegion -cellZone" command. If you are using one whole STL its possible that you `ll get 10 or more other regions named domain** after splitting.

It doesn't matter to change the snap or quality control settings. To get only the domains you want to have you have to use the STL as region STL.

After that you should set the refinement of the interface to the same levels. With that knowledge you are able to mesh complex gemoetries with snappyHexMesh without creating other domains.

For more information have a look at that complete thread.
My case is avaiable on my homepage soon.


Thanks for all the infos bruno!
Tobi
Attached Images
File Type: jpg stl.jpg (20.9 KB, 64 views)
wyldckat likes this.

Last edited by Tobi; February 19, 2013 at 18:01.
Tobi is offline   Reply With Quote

Old   February 20, 2013, 11:01
Default
  #31
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi everybody & bruno,

I share my complex geometric meshing case with you. In the case you are meshing:

- a hot air pipe
- two cold water channels
- the connection between air/water with solids (steel) by six pipes

At the end you have nine regions and a case you can solve with chtMultiRegionSimpleFoam. Just execute the Run.sh file to build everything by the script (Attachement).


Warning | Important
- - - - - - - - - - - - - - - - - -
My maschine works with 20 GB memory space and while meshing that case I get a total load of about 75%. I reduced the cellrefinement just to see how the meshing process is working but the mesh is not very accurate then.

Anyway be sure you have more then 8 GB memory on your computer to be sure that everything is working fine. Otherwise your computer get overloaded by sHM and I think you know what that means



Unfortunately the script is written in germany but I think everyone understand the things I have done.


I will add that tutorial into the OpenFOAM-Wiki SnappyHexMesh for downloading


Thanks to all. New experiance and good work.

Download [activated]: http://www.holzmann-cfd.de/index.php...waermetauscher

Tobi
Attached Images
File Type: jpg wt.jpg (19.3 KB, 40 views)

Last edited by Tobi; February 22, 2013 at 12:05.
Tobi is offline   Reply With Quote

Old   February 20, 2013, 13:58
Default
  #32
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi all,

at least there is one problem left. I realised that the last few minutes.

Have a look at the picture. Can someone imagine why that is happening?

Problem:

The first pipes above are refined a level more and everything is working.
If I want to refine the pipe with the cutten cells I get problems by splitting the mesh. --> more regions (domain**)...


Hmmmm
Attached Images
File Type: jpg problem.jpg (13.7 KB, 34 views)
Tobi is offline   Reply With Quote

Old   February 20, 2013, 18:00
Default
  #33
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,525
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Tobi,

Have you tried checking your STL files with OpenFOAM's surfaceCheck? It should give you some diagnostics on the validity of the STL files.

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   February 20, 2013, 19:38
Default
  #34
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
yes everything is fine!
Tobi is offline   Reply With Quote

Old   February 22, 2013, 10:41
Default
  #35
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bruno,

just set one more cell into the mesh and everything is working now.

Here my Run script:

Code:
#!/bin/bash
./Clean.sh
echo "Feature Edge erzeugen"
surfaceFeatureExtract -includedAngle 130 constant/triSurface/kanal1.stl kanal1  > log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/kanal2.stl kanal2  >> log.Run
surfaceFeatureExtract -includedAngle 120 constant/triSurface/luftkanal.stl luftkanal  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr1.stl rohr  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr2.stl rohr  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr3.stl rohr  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr4.stl rohr  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr5.stl rohr  >> log.Run
surfaceFeatureExtract -includedAngle 130 constant/triSurface/rohr6.stl rohr  >> log.Run

echo "Feature Edge für Paraview konvertieren"
surfaceFeatureConvert constant/triSurface/kanal1.eMesh constant/triSurface/kanal1FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/kanal2.eMesh constant/triSurface/kanal2FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/luftkanal.eMesh constant/triSurface/luftkanalFeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr1.eMesh constant/triSurface/rohr1FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr2.eMesh constant/triSurface/rohr2FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr3.eMesh constant/triSurface/rohr3FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr4.eMesh constant/triSurface/rohr4FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr5.eMesh constant/triSurface/rohr5FeatureEdge.obj >> log.Run
surfaceFeatureConvert constant/triSurface/rohr6.eMesh constant/triSurface/rohr6FeatureEdge.obj >> log.Run

echo "Hintergrundnetz erstellen"
ideasUnvToFoam files/blockMesh.unv >> log.Run

echo "Skaliere Hintergrundnetz"
transformPoints -scale "(1000 1000 1000)" >> log.Run

echo "Netz zerlegen"
decomposePar >> log.Run

echo "Vernetzen"
mpirun -np 8 snappyHexMesh -parallel >> log.Run

echo "Netz zusammenfügen"
reconstructParMesh -latestTime -mergeTol 1e-6 >> log.Run

echo "Prozessorordner löschen"
rm -rf processor*

echo "Netz in Regionen splitten"
splitMeshRegions -cellZones >> log.Run

echo "Nicht benötigte Zonen löschen"
rm -r 3/domain0

echo "Regionen verschieben"
mv 3/* constant 

echo "Patches der Regionen ändern"
cp files/createPatchDict.kanal1 system/kanal1/createPatchDict
cp files/createPatchDict.kanal2 system/kanal2/createPatchDict
cp files/createPatchDict.luftkanal system/luftkanal/createPatchDict
cp files/createPatchDict.rohr1 system/rohr1/createPatchDict
cp files/createPatchDict.rohr2 system/rohr2/createPatchDict
cp files/createPatchDict.rohr3 system/rohr3/createPatchDict
cp files/createPatchDict.rohr4 system/rohr4/createPatchDict
cp files/createPatchDict.rohr5 system/rohr5/createPatchDict
cp files/createPatchDict.rohr6 system/rohr6/createPatchDict

createPatch -region kanal1 -overwrite >> log.Run
createPatch -region kanal2 -overwrite >> log.Run
createPatch -region luftkanal -overwrite >> log.Run
createPatch -region rohr1 -overwrite >> log.Run
createPatch -region rohr2 -overwrite >> log.Run
createPatch -region rohr3 -overwrite >> log.Run
createPatch -region rohr4 -overwrite >> log.Run
createPatch -region rohr5 -overwrite >> log.Run
createPatch -region rohr6 -overwrite >> log.Run

echo "Patchtypen ändern"
cp files/changeDictionaryDict.kanal2 system/kanal2/changeDictionaryDict

changeDictionary -region kanal2 >> log.Run

echo "Numerische Schemen und Verfahren aktualisieren"
cp files/fvSolution.kanal system/kanal1/fvSolution
cp files/fvSolution.kanal system/kanal2/fvSolution
cp files/fvSchemes.kanal system/kanal1/fvSchemes
cp files/fvSchemes.kanal system/kanal2/fvSchemes
cp files/fvSolution.luftkanal system/luftkanal/fvSolution
cp files/fvSchemes.luftkanal system/luftkanal/fvSchemes
cp files/fvSolution.rohr system/rohr1/fvSolution
cp files/fvSolution.rohr system/rohr2/fvSolution
cp files/fvSolution.rohr system/rohr3/fvSolution
cp files/fvSolution.rohr system/rohr4/fvSolution
cp files/fvSolution.rohr system/rohr5/fvSolution
cp files/fvSolution.rohr system/rohr6/fvSolution
cp files/fvSchemes.rohr system/rohr1/fvSchemes
cp files/fvSchemes.rohr system/rohr2/fvSchemes
cp files/fvSchemes.rohr system/rohr3/fvSchemes
cp files/fvSchemes.rohr system/rohr4/fvSchemes
cp files/fvSchemes.rohr system/rohr5/fvSchemes
cp files/fvSchemes.rohr system/rohr6/fvSchemes

echo "Zeitornder vorbereiten"
rm -rf 1 2 3 
cp -r 0.org 0
cd 0
cp -r rohr rohr1
cp -r rohr rohr2
cp -r rohr rohr3
cp -r rohr rohr4
cp -r rohr rohr5
mv  rohr rohr6
cd ..

echo "Update der Einträge von rohr.*"
sed -i s/rohr_to_kanal/rohr1_to_kanal2/g 0/rohr1/T
sed -i s/rohr_to_kanal/rohr2_to_kanal1/g 0/rohr2/T
sed -i s/rohr_to_kanal/rohr3_to_kanal2/g 0/rohr3/T
sed -i s/rohr_to_kanal/rohr4_to_kanal1/g 0/rohr4/T
sed -i s/rohr_to_kanal/rohr5_to_kanal2/g 0/rohr5/T
sed -i s/rohr_to_kanal/rohr6_to_kanal1/g 0/rohr6/T
sed -i s/rohr_to_l/rohr1_to_l/g 0/rohr1/T
sed -i s/rohr_to_l/rohr2_to_l/g 0/rohr2/T
sed -i s/rohr_to_l/rohr3_to_l/g 0/rohr3/T
sed -i s/rohr_to_l/rohr4_to_l/g 0/rohr4/T
sed -i s/rohr_to_l/rohr5_to_l/g 0/rohr5/T
sed -i s/rohr_to_l/rohr6_to_l/g 0/rohr6/T

echo "Vorbereitung für Paraview"
paraFoam -touchAll

echo "Physikalische Daten vorbereiten"
cp files/g  constant/kanal1
cp files/g  constant/kanal2
cp files/g  constant/luftkanal*
cp files/RASProperties.kanal constant/kanal1/RASProperties
cp files/RASProperties.kanal constant/kanal2/RASProperties
cp files/RASProperties.luftkanal constant/luftkanal/RASProperties
cp files/turbulenc* constant/kanal1
cp files/turbulenc* constant/kanal2
cp files/turbulenc* constant/luftkanal
cp files/radiation* constant/kanal1
cp files/radiation* constant/kanal2
cp files/radiation* constant/luftkanal
cp files/solid* constant/rohr1
cp files/solid* constant/rohr2
cp files/solid* constant/rohr3
cp files/solid* constant/rohr4
cp files/solid* constant/rohr5
cp files/solid* constant/rohr6
cp files/thermophysicalProperties.kanal constant/kanal1/thermophysicalProperties
cp files/thermophysicalProperties.kanal constant/kanal2/thermophysicalProperties
cp files/thermophysicalProperties.luftkanal constant/luftkanal/thermophysicalProperties

echo "PolyMesh Ordner löschen"
rm -r constant/polyMesh

echo "Netz zurückskalieren"
transformPoints -scale "(0.001 0.001 0.001)" -region kanal1 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region kanal2 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region luftkanal >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr1 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr2 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr3 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr4 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr5 >> log.Run
transformPoints -scale "(0.001 0.001 0.001)" -region rohr6 >> log.Run

echo "Simulationsfall zur Simulation bereit 
Befehl >> chtMultiRegionSimpleFoam > log &"
Everything is build automatically in that script. I think some commands or the way I do a few things is unconfortable but in a way everyone will understand


I upload the file in a few minutes

Last edited by Tobi; February 22, 2013 at 11:55.
Tobi is offline   Reply With Quote

Old   February 22, 2013, 12:07
Default Finished
  #36
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Okay now it's gonna be a monolog


1. Download Link activated above.
http://www.holzmann-cfd.de/index.php...waermetauscher

2. Reduce the mesh refinements to reduce the memory load

3. Updated the openfoamwiki with that link


Enjoy

Kind regard
Tobi
wyldckat likes this.
Tobi is offline   Reply With Quote

Old   April 4, 2013, 06:27
Default add layers
  #37
New Member
 
David Haces
Join Date: Mar 2013
Posts: 26
Rep Power: 4
Haces is on a distinguished road
Hi!!

I need some help!

I want to add layers to a multi-region case, in the interface between the water and the pipes. You can see the geometry in the attached document. The grey parts are the pipes and the blue part is the water.

I was able to create the castellated mesh and snap it in the multi-region case. I can also add layers if I am working only with the water. The problem is that snappyHexMesh doesn't recognize the boundaries between the surfaces when is working with several STL files.

What I thought to solve this problem is to:

Option 1:
1-Create the mesh without layers using several STL files.
2-Split the mesh with splitMeshRegions.
3-Add layers only to the water.
4-Put everything again together.
5-Eliminate the domains I don't want since the geometry is complex and blockmesh is a prism.

The step number 4 I don't know how to do it. I've thought using stitchMesh or mergeMeshes but i don't know if it will work to create a multi-region mesh.

Option 2:
Adding layers using only one STL file but the result won't be a multi-region case any more. Is possible to generate a multiregion case from only one STL file?


Any suggestions in order to help me with the 2 options? Do you have another idea to add layers?

Thanks for your help!

David.
Attached Images
File Type: jpg geometry.jpg (16.2 KB, 33 views)
Haces is offline   Reply With Quote

Old   April 4, 2013, 07:01
Default
  #38
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,

why you want to put the mesh together again ?
Tobi is offline   Reply With Quote

Old   April 4, 2013, 07:13
Default
  #39
New Member
 
David Haces
Join Date: Mar 2013
Posts: 26
Rep Power: 4
Haces is on a distinguished road
Hi toby,

The problem is that if I modify the blockmesh of the water the new points are only in this blockmesh and not in the general blockmesh. Later when I run the cht this is not going to work properly, right? It is a little bit difficult to understand how works the cht solver for me...
Haces is offline   Reply With Quote

Old   April 4, 2013, 07:21
Default
  #40
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
No

You can have 1000 faces from fluid_to_solid
and 13000 faces to solid_to_fluid


A lot of people do not use snappy for using several domains.
You can mesh every domain itselfs and connecting them later with the patchType mappedWall.


The points dont have to be at the same possition from mesh1 compared to mesh2.
Tobi is offline   Reply With Quote

Reply

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
blockCoupled solver for multiple regions benk OpenFOAM 2 February 13, 2014 23:35
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
multiple regions for soild mechanics? chaz OpenFOAM Running, Solving & CFD 9 May 3, 2013 08:49
How to define multiple fluid regions in icem user0314 ANSYS Meshing & Geometry 4 May 11, 2011 10:36
OpenFOAM static build on Cray XT5 asaijo OpenFOAM Installation 9 April 6, 2011 12:21


All times are GMT -4. The time now is 06:44.