# problem in toposet

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

 May 17, 2012, 14:21 problem in toposet #1 Senior Member     ahmed Join Date: Feb 2010 Posts: 163 Blog Entries: 1 Rep Power: 7 Hi Foamers, i'm trying to run chtMultiRegionFoam on my own case, it's a tube with outer diameter 11cm, inner diameter 10cm and length 100cm i created a cylinder in blockMesh file with outer diameter 11cm and length 100 cm asin this code Code: ```convertToMeters 0.01; vertices ( (0 0 0) // point 0 (0 11 0) // point 01 (0 16.5 1.47372) // point 02 (0 20.52628 5.5) // point 03 (0 22 11) // point 04 (0 20.52628 16.5) // point 05 (0 16.5 20.52628)// point 06 (0 11 22) // point 07 (0 5.5 20.52628)// point 08 (0 1.47372 16.5) // point 09 (0 0 11) // point 10 (0 1.47372 5.5) // point 11 (0 5.5 1.47372) // point 12 (100 11 0) // point 13 (100 16.5 1.47372) // point 14 (100 20.52628 5.5) // point 15 (100 22 11) // point 16 (100 20.52628 16.5) // point 17 (100 16.5 20.52628)// point 18 (100 11 22) // point 19 (100 5.5 20.52628)// point 20 (100 1.47372 16.5) // point 21 (100 0 11) // point 22 (100 1.47372 5.5) // point 23 (100 5.5 1.47372) // point 24 (0 11 11) // point 25 (100 11 11) // point 26 ); blocks ( hex (25 1 3 25 26 13 15 26) (10 10 10) simpleGrading (1 1 1) hex (25 3 5 25 26 15 17 26) (10 10 10) simpleGrading (1 1 1) hex (25 5 7 25 26 17 19 26) (10 10 10) simpleGrading (1 1 1) hex (25 7 9 25 26 19 21 26) (10 10 10) simpleGrading (1 1 1) hex (25 9 11 25 26 21 23 26) (10 10 10) simpleGrading (1 1 1) hex (25 11 1 25 26 23 13 26) (10 10 10) simpleGrading (1 1 1) ); edges ( arc 1 3 (0 16.5 1.47372) arc 3 5 (0 22 11) arc 5 7 (0 16.5 20.52628) arc 7 9 (0 5.5 20.52628) arc 9 11 (0 0 11) arc 11 1 (0 5.5 1.47372) arc 13 15 (100 16.5 1.47372) arc 15 17 (100 22 11) arc 17 19 (100 16.5 20.52628) arc 19 21 (100 5.5 20.52628) arc 21 23 (100 0 11) arc 23 13 (100 5.5 1.47372) ); boundary ( outerface { type wall; faces ( (1 13 15 3) (3 15 17 5) (5 17 19 7) (7 19 21 9) (9 21 23 11) (11 23 13 1) ); } inlet { type wall; faces ( (25 1 3 25) (25 3 5 25) (25 5 7 25) (25 7 9 25) (25 9 11 25) (25 11 1 25) ); } outlet { type wall; faces ( (26 15 13 26) (26 17 15 26) (26 19 17 26) (26 21 19 26) (26 23 21 26) (26 13 23 26) ); } ); mergePatchPairs ( );``` and created a file topoSetDict to divide it to two regions flow, and tube like this: Code: ```actions ( // flow inside the tube { name flow; type cellSet; action new; source cylinderToCell; sourceInfo { p1 (0 11 11); // start point on cylinder axis// p2 (100 11 11); // end point on cylinder axis// radius 10.0; } } { name flow; type cellZoneSet; action new; source setToCellZone; sourceInfo { set flow; // name of cellSet } } //tube { name tube; type cellZoneSet; action clear; } { name tube; type cellSet; action add; source cellToCell; sourceInfo { set flow; } } { name tube; type cellSet; action invert; } { name tube; type cellZoneSet; action new; source setToCellZone; sourceInfo { set tube; } } );``` but when running blockMesh, topoSet, splitMeshRegion it divide it to one region (tube) and this is log file log.topoSet Code: ```Create time Create polyMesh for time = 0 Reading topoSetDict Time = 0 mesh not changed. Created set flow Applying source cylinderToCell Adding cells with centre within cylinder, with p1 = (0 11 11), p2 = (100 11 11) and radius = 10 Set flow now size 0 Created set flow Applying source setToCellZone Adding all cells from cellSet flow ... Set flow now size 0 Created set tube Clearing set Set tube now size 0 Read set tube with size 0 Applying source cellToCell Adding all elements of cellSet flow ... Set tube now size 0 Read set tube with size 0 Inverting set Set tube now size 6000 Created set tube Applying source setToCellZone Adding all cells from cellSet tube ... Set tube now size 6000 End``` and log.splitMeshRegions Code: ```Create time Create mesh for time = 0 Creating single patch per inter-region interface. Trying to match regions to existing cell zones. Number of regions:1 Writing region per cell file (for manual decomposition) to "/home/khattab/ahmed.2.0.1/tutorials/heatTransfer/chtMultiRegionFoam/Graetz10/constant/cellToRegion" Writing region per cell as volScalarField to "/home/khattab/ahmed.2.0.1/tutorials/heatTransfer/chtMultiRegionFoam/Graetz10/0/cellToRegion" Region Cells ------ ----- 0 6000 Region Zone Name ------ ---- ---- 0 1 tube Sizes of interfaces between regions: Interface Region Region Faces --------- ------ ------ ----- Reading volScalarField Y_char Reading volScalarField cellToRegion Reading volScalarField p Reading volScalarField T Reading volScalarField k Reading volScalarField epsilon Reading volScalarField P_rgh Reading volScalarField Y_pmma Reading volVectorField U Only one region. Doing nothing. End``` please help

 May 28, 2012, 04:18 #2 Senior Member     ahmed Join Date: Feb 2010 Posts: 163 Blog Entries: 1 Rep Power: 7 Dears, finally i have found the problem. in blockMeshDict i have converted units to centimeter so i have wrote 0.1m as 10. in toposet i used same value but it red it as meters so 10 became 10m. it red only tube region because it was invert of other region which had been red as empty. as assigned all cells for tube region. now every thing is do well. thanks for all who red this post. ahmed farahiam and range_rover like this.

 May 28, 2012, 05:56 #3 Senior Member   cfdkid Join Date: Mar 2009 Posts: 133 Rep Power: 8 Hi, What does topoSet do ? __________________ ________________________________________ Regards, CFDkid It never gets easier You just get Better

May 28, 2012, 11:44
#4
Senior Member

ahmed
Join Date: Feb 2010
Posts: 163
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by kid Hi, What does topoSet do ?
Dear Kid,

topoSet is used to split your mesh into many regions so you can give properties to the entire region not only for patches. i used for the first time for heat transfer problem in chtMultiRegioFoam solver with multiRegionHeater case. you can try the case and will get a good experience of it.

if any question don't hesitate to post for me.

good luck

 May 28, 2012, 16:08 #5 New Member   Andrew Kettner Join Date: May 2012 Posts: 4 Rep Power: 5 New to OpenFoam and I am attempting post process the results from the the chtMultiRegionFoam tutorials. I cannot seem to get paraview to read any of the files. If I attempt to look at the with a gedit the file does not load correctly and I get nonsense. This has not been a problem for other tutorials. I am running open foam on a virtually install Ubuntu 12.04. Suggestions please Thanks

May 29, 2012, 05:50
#6
Senior Member

ahmed
Join Date: Feb 2010
Posts: 163
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by kettnera New to OpenFoam and I am attempting post process the results from the the chtMultiRegionFoam tutorials. I cannot seem to get paraview to read any of the files. If I attempt to look at the with a gedit the file does not load correctly and I get nonsense. This has not been a problem for other tutorials. I am running open foam on a virtually install Ubuntu 12.04. Suggestions please Thanks
Hi Kettnera,
i experienced same problem before, after processing chtMultiRegionFoam solver, as usual type paraFoam and paraview will open then from toolbar choose file then open, it will open window for you shows the directory of your case choose the five files with .openfoam extension (bottomair topair heater rightssolid leftsolid), click apply. now you can see results.

the problem with gedit is that results are written in binary so you can't see it correctly. if you want go to controlDict file in system directory then change ninary to Ascii code then you will see results correctly.

good luck

 May 29, 2012, 16:28 #7 New Member   Andrew Kettner Join Date: May 2012 Posts: 4 Rep Power: 5 Thx Ahmed That did it.

 June 4, 2012, 00:31 #8 Senior Member     ahmed Join Date: Feb 2010 Posts: 163 Blog Entries: 1 Rep Power: 7 you are welcome.

 June 7, 2012, 07:19 #9 New Member   Rehan amin Join Date: May 2012 Posts: 3 Rep Power: 5 Hello sir, 1)can you please tell me the significance of 'invert' action? also 2) what does 'type cellset' & 'type cellzoneset' mean?

June 7, 2012, 12:21
#10
Senior Member

ahmed
Join Date: Feb 2010
Posts: 163
Blog Entries: 1
Rep Power: 7
Quote:
 Originally Posted by rehan Hello sir, 1)can you please tell me the significance of 'invert' action? also 2) what does 'type cellset' & 'type cellzoneset' mean?
Hi Rehan,

1- invert is used to specify region which is the rest of the domain instead of specify it as every region you can just say that it is the invert of all regions in the domain.

 March 24, 2013, 16:18 #11 New Member   Meinan Chen Join Date: Mar 2013 Posts: 5 Rep Power: 4 Hi ~~ I wonder do you still work on chtMultiRegionFoam? cuz I see that the time you replied is really long time ago, I am totally new to OPenFoam, and now I am trying to split the region into solid and fluid. I generated my mesh in ICEM, and converted it in Openfoam, and now I am trying to split the region, I try to define the region in MakeCellSets file, I wonder am I doing right? Should I split the region in MakeCellSets or topoSet? I feel so confused, really hope that you can reply me! THanks!!!

 October 29, 2015, 09:26 #12 Member   Mahdi S Join Date: Jul 2012 Posts: 34 Rep Power: 5 Hi all I am building a test case with 2 main regions (1 solid and 1 fluid attached together). I built it simply by using topoSet. My question is if I wanna create a wallFilmRegion between these two regions, how can I address the source info for that? I mean what it the correct source info for this patch? If you look at the case "tutorail/lagrangian/reactingParcelFilmFoam/rivuletpanel", the wallFilmRegion is created using a source from blockMeshDict. { name wallFilm; type faceSet; action new; source patchToFace; sourceInfo { name filmWalls; } } { name wallFilm; type faceZoneSet; action new; source setToFaceZone; sourceInfo { faceSet wallFilmFaces; } } But in my case the connecting patch between solid region and fluid region is not defined in advance and should be created within the topoSet itself! (First by topoSet I define 2 regions and now I wanna address the patch in between as source for wallFilmRegion.) any idea for that!?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43 JFDC FLUENT 1 July 11, 2011 05:59 Se-Hee CFX 2 June 10, 2007 06:29 ParodDav CFX 5 April 29, 2007 19:13 Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52

All times are GMT -4. The time now is 21:44.