|
[Sponsors] |
[snappyHexMesh] Can't couple front & back faces in cyclic BC after snapping in SHM |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 25, 2013, 14:00 |
Can't couple front & back faces in cyclic BC after snapping in SHM
|
#1 |
New Member
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 14 |
Hi everyone!
I have a problem involving the createPatch utility and snappyHexMesh. I'm setting up a 3D simulation across a wing section, and I want to couple the front and back faces of the mesh with a "cyclic" boundary condition. In order to bring down the cell count, I have to do some work on the mesh after generating it in SHM. For this reason, I initially define the front and back faces of my mesh as "empty", and only convert them to "cyclic" later using the createPatch utility. My problem is that if I allow SHM to go through with the snapping stage, it reorders the face list in such a way that the faces on the front and back patches can no longer find their twin on the opposite patch. This makes it impossible to convert these faces from "empty" to "cyclic". I've tried the renumberMesh utility, but that didn't solve the problem. Do any of you know how to go about converting patches generated in snappyHexMesh to the cyclic type? regards, Håkon |
|
June 4, 2013, 06:25 |
|
#2 |
New Member
Thomas Lloyd
Join Date: May 2011
Posts: 7
Rep Power: 15 |
Dear Håkon
I recommend that you specify the cyclic patches as type "cyclic" in a blockMeshDict. Then when SHM runs, it will preserve these patches as cyclic and you should require not further mesh processing. This worked for me. See the openfoam website for details of how ti assign patch types in blockMesh. Regards, Tom |
|
November 28, 2013, 09:40 |
|
#3 | |
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Beijing, China
Posts: 849
Rep Power: 18 |
Quote:
Code:
convertToMeters 1; vertices ( (0 -0.1145 0.3) (0.3 -0.1145 0.3) (0.3 -0.1145 0) (0 -0.1145 0) (0 1 0.3) (0.3 1 0.3) (0.3 1 0) (0 1 0) ); blocks ( hex (0 3 7 4 1 2 6 5 ) (20 60 20) simpleGrading (1 1 1)//28 39 28 ); edges ( ); boundary ( cyc_half0 { type cyclic; neighbourPatch cyc_half1; transform rotational; rotationAxis (0 1 0); rotationCentre (0 0 0); faces ( (3 7 6 2 ) ); } cyc_half1 { type cyclic; neighbourPatch cyc_half0; transform rotational; rotationAxis (0 1 0); rotationCentre (0 0 0); faces ( (0 3 7 4 ) ); } ); mergePatchPairs ( ); Code:
-> FOAM FATAL ERROR: More than one patch accessing the same transform but not of the same sign. patch:cyc_half1 transform:0 sign:-1 current transforms:(-1 0 0) From function Foam::label Foam::globalIndexAndTransform::addToTransformIndex ( const label, const label, const bool ) const in file lnInclude/globalIndexAndTransformI.H at line 268. FOAM exiting |
||
December 4, 2013, 09:17 |
|
#4 |
Member
phil
Join Date: Oct 2013
Posts: 36
Rep Power: 13 |
Hi,
you can also define your patches as wall (default for sHM) etc. in snappy and after snappy running through you can modify your 0/* files and boundary file with the "changeDictionaryDict" command. For this you need a changeDictionaryDict file in your system folder. You can find example files either by yourself or have a look at this one located in: /tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater/system/ In case you run in parallel you have to modify the command. 1. First move to the processor* folder 2. Then enter "changeDictionaryDict -dict /path/to/the/dict/file" 3. Repeat step 1 and 2 for all processor folders. Greetings Last edited by gelbebanane; December 4, 2013 at 09:18. Reason: bye |
|
December 8, 2013, 17:50 |
|
#5 |
New Member
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 14 |
Hi all and thanks for the advice,
My question was regarding a masters project that I handed in in June, and I seem to have misplaced the case files, so I can't go back and check it. However, the work that I intended to do on the mesh included cutting out a subset of the mesh, including some of the front and back faces, and extruding it to a lower spanwise resolution before putting it back in. It was therefore not possible to define the front and back boundaries as cyclic from the get-go, as that would mess up the subset and extrusion processes. I also tried what you suggest, banana, but this process of cutting and extrusion changed the cell count of the mesh, which threw off the face numbering. Now, this shouldn't have been a problem when generating a cyclic boundary, as any face on one of the planes should have been able to find its twin on the other, based on its position and area. For some reason, though, this automatic face matching didn't work, and I just decided to drop the problem after a while, as it wasn't essential. @sharon: I think the problem may be that the rotationAxis on one of your cyclic patches is defined the wrong way. Try changing one or the other to (0 -1 0). However, i also think you might be using syntax from an old version of OF, as you don't have to define the coupling of your cyclic boundaries that explicitly anymore. Check out the tutorials with cyclic boundaries. I think some of them are defined in a simpler way. best regards, Håkon |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Foam::error::PrintStack | almir | OpenFOAM Running, Solving & CFD | 92 | May 21, 2024 08:56 |
[snappyHexMesh] Layers not growing at all | zonda | OpenFOAM Meshing & Mesh Conversion | 12 | June 6, 2020 12:28 |
[snappyHexMesh] SHM Layer Addition Phase | dickcruz | OpenFOAM Meshing & Mesh Conversion | 4 | November 1, 2018 08:05 |
Compressor Simulation using rhoPimpleDyMFoam | Jetfire | OpenFOAM Running, Solving & CFD | 107 | December 9, 2014 14:38 |
DecomposePar unequal number of shared faces | maka | OpenFOAM Pre-Processing | 6 | August 12, 2010 10:01 |