sHM and cyclicGgi
Hi Foamers,
when i want to run sHM, I get the following error message: Code:
Cannot handle coupled patch cyclicX of type cyclicGgi 1) Run blockMesh (creates the box) 2) run createPatch 3) run snappyHexMesh => crash i try to simulate the flow around a cylinder in a cuboid-box. the cylinder is placed near one side of the box to have an unsymmetric flow. so i use cyclicGgi to have a symmetric flow as i would have, if i had placed the cylinder right in the middle of the box. this is only a test case for me, because i would like to implement cyclicGgi in a case in which it is absolute necessary. have i done something wrong or it is not possible to use cyclicGgi and sHM in the same case? is cyclicGgi the rigth patch type or is cyclic better? what are the differences? as i am new in sHM and cyclic boundaries, any help is appreciated! My createPatchDict: Code:
matchTolerance 1E-3; Code:
4 |
Hello,
seems to me that SHM does not handle cyclic boundaries. You should change steps 2 and 3: 1) create the surrounding coarse mesh with blockMesh 2) apply SHM 3) apply createPatch to make the appropriate patches cyclic Hope that helps. Please keep us posted how it is working out. Regards Markus |
thanks for your reply, markus.
i´ve changed steps 2 and 3, and it works. but when i want to run simpleFoam, i get the following error-message: Code:
Reading field p Code:
dimensions [0 2 -2 0 0 0 0]; |
the mistake of the last post was only a mistake in writing the patch names.
but i haven´t get my case running... my steps are: 1)blockMesh 2)sHM 3)createPatch 4)copy the p,U,...-files into last directory 5)run simpleFoam => crash: Code:
Create time so the mistake must be related to createPatch/simpleFoam any help is much appreciated! |
Hello,
you should try running the solver in DEBUG-mode to obtain more information. Markus |
Hi Markus,
unfortunately i dont know how to run in debug.mode. i added the last line in simpleFoam-folder make/options: Code:
EXE_INC = \ then i´ve tried to run simpleFoam in my case-folder again to receive more information about the segmentation fault. but it crashs like before... can you give me a hint? thx |
Hi,
See http://openfoamwiki.net/index.php/Main_FAQ in 8.1 An application ends with a segmentation fault. What is wrong? ...To find out where this occurs make a separate copy of the OF-sources, recompile them with the swich WM_COMPILE_OPTION set to Debug (just uncomment the right lines in the bashrc/cshrc files). This makes OF run slower, but accesses to List<> etc are checked for ranges and the program aborts if you access outside of a range (plus you get a stack trace). This won't solve your problem, but it will help you find out where it occurs. See also General debugging tips. For recompiling OpenFOAM look at Howto_compile_OpenFOAM Markus |
3 Attachment(s)
Thx for the answer.
i changed lines 92, 94 and 96 in bashrc (folder: OpenFOAM/OpenFOAM-1.5-dev/etc): Code:
# Compilation options (architecture, precision, optimised, debug or profiling) Code:
# Compilation options (architecture, precision, optimised, debug or profiling) But the only output was that everything is up to date. In OpenFOAM-1.5-dev folder the same (see log). If i run simpleFoam in my case-directory, because nothing changed => segmentation fault. What am I doing wrong? Attached Allwmake log and bashrc/cshrc EDIT: Now I am compiling my debug-version of OF. I followed the instructions of http://www.cfd-online.com/Forums/ope...oam-1-6-a.html post #2. |
Hi Fabian,
you do not need to change the bashrc or cshrc (by the way you need only one of them - depending on the type of shell you have - so let us suppose your linux uses bash-shell like for example OpenSUSE does). What you do is: 1) Change the environment variable to debug export WM_COMPILE_OPTION=Debug (check it with echo $WM_COMPILE_OPTION) 2) source your bashrc again . ~/.bashrc this will run all the initialisation scripts for OF and set the right stuff for the Debug mode 3) rerun Allwmake as before but pay attention that the executables are written to /home/fabian/OpenFOAM/OpenFOAM-1.5-dev/applications/bin/linuxGccDPDebug/ usually it is written do *Opt 4) Run the solver again - to check which one you are using type which simpleFoam To reuse the Opt branch again do export WM_COMPILE_OPTION=Opt and source again. Hope that helps. Markus |
thank you very much. the debug mode works.
so, i´ve got the following error message: Code:
Create time Code:
// Check index i is within valid range (0 ... size-1). |
Hi,
can you post your current boundary file? I use shm with cyclics by just creating the whole mesh without ggi and changing the patch type in a last step in that file by hand (don't know whether createPatch would be an alternative) Best regards, -Thomas |
Hi Thomas,
constant/polyMesh/boundary: Code:
6 1/polyMesh/boundary: Code:
FoamFile That would be great! |
Hi FabOr,
if the second file was your actual one, following things are strange: - there is only one cyclicGgi entry; there should be two (for example "cyclicY") - not all subentries are filled in; you have to define the correct shadow patch (if the above was correct, the shadow patch entry in "cyclicX" should be "cyclicY") - your mesh has to have the corresponding face zones which you also have to define for example via faceSet - take care of the rotation angle; fill in the correct value for your case. I'll have a look whether I can find a very simple test case to demonstrate the setup. Meanwhile, you could search the net (I remember that I derived my setup from a presentation of a member of the turbomachinery SIG, but I don't remember the name...) Regards, -Thomas |
1 Attachment(s)
Hi,
thanks for your answer Thomas. Let me explain you what i want to do: I´ve got a stl-file which is implemented by snappyHexMesh in a simple Box(like in attached picture). Because of unsymmetry of the stl file(but its periodic) i want to have the influence of the opposite sites in the simulation=> minX/maxX and minY/maxY. The aim of the implementation of cyclicGgi is that i dont simulate only the stl-geomatry part, but lots of them by only computing one. i hope you understand me:) So i dont need a rotation axis or angle. but i am not sure anymore if cyclicGgi is the right patch-type. i hope you can tell me if i am right. regards |
Hi FabOr,
The link I mentioned above is http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/case_study_2010_OP.pdf where you can find informations on setting up a ggi boundary for either cyclic or translational cases. I think ggi (not cyclicGgi!) will work for your case. You could start by taking the mesh of a tutorial case (like channel395), change it to your needs and then introduce the ggi instead of the standard cyclic bc to get an idea of the correct setup. Be aware that ggi only works in 1.5-dev. Best regards, -Thomas |
Hi,
i´ve got a working case with strange results. My steps: 1) blockMesh 2) sHM 3) faceSet for minX,maxX, minY and maxY (changes needed in faceSetDict) 4) setsToZones -noFlipMap 5) change the boundary-file 6) simpleFoam I´ve getting also an uncovered faces warning message: Code:
Create time Due to the upload limit, i will send you the case-files and a paraview-picture of the strange results per email... Any help is much appreciated! |
Quote:
What is the difference between the latest version of OF (I think 1.7.1 which I have) and the 1.5-dev version? So you're saying that GGI won't work in 1.7.1? Regards, Ralph |
Hi Ralph,
I´ve read in other threads that Ggi is only implemented in the developer-version, short -dev. So it is not supported in the "normal" versions. http://www.cfd-online.com/Forums/ope...confusion.html Regards |
1 Attachment(s)
Hi all,
as i reported i get strange results using cyclicGgi and ggi. Attached is a plot over line on the x-Axis. Because of using ggi-patch, i thought that on both sides the velocity should be equal!? When running simpleFoam i get a message that there are uncovered faces on master and slave patch. Can that cause the error? If yes, how can uncovered faces be avoided? best regards |
1 Attachment(s)
Hi FabOr,
I've set up a simple channel flow case with cyclics which technically works (which does not mean it has any physical meaning...). Maybe this gives you some hints for your own setup... Good luck, -Thomas |
All times are GMT -4. The time now is 01:48. |