|
[Sponsors] |
Setting cyclicAMI and cyclic Boundary conditions (ICEM Mesh to OpenFoam) |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Join Date: Dec 2016
Posts: 6
Rep Power: 9 ![]() |
I want to simulate turbine rotating in a circular channel. Due to symmetry, the mesh only contain 1/3 of the domain(120 degree wedge). I want to use simpleFoam and MRF. I've made two cellzones jointed by cyclicAMI BCs. I also want to apply cyclic BCs to side faces of both inner and outter domain.
However, I also get errors either due to cyclicAMI or cyclic BCs. My way of setting BCs is: 1. I used fluent3DMeshToFoam (also tried fluentMeshToFoam) to convert Mesh from ICEM to OpenFoam format. 2. I manually change the boundary conditions in constant/polyMesh folder to set cyclic and cyclicAMI BCs in certain faces. This is okay for cyclicAMI BCs, but I got errors for faces of cyclic BCs like: FOAM FATAL ERROR: face 741 area does not match neighbour by 147.120008% -- possible face ordering problem. patch:SYSINL my area:0.0041659859 neighbour area:0.0273467715 matching tolerance:0.0001 Mesh face:11758713 fc ![]() Neighbour fc ![]() I've checked my Mesh carefully and the nodes on cyclic BCs faces are symmetric. 3. Due to suggestions from the forum, I used createPatch -overwrite to create cyclic BCs, which could help to reorder faces. But boundary file in constant/polyMesh keeps unchanged so I then manually changed the boundary file in constant/polyMesh. (I also tried use createPatch to create BOTH cyclicAMI and cyclic/use createPatch to create all BCs). By doing this, there e is no problem with cyclic BCs. However, errors for cyclicAMI showed, such as: AMI: Creating addressing and weights between 27000 source faces and 3103 target faces --> FOAM Warning : From function AMIMethod<SourcePatch, TargetPatch>::checkPatches() in file lnInclude/AMIMethod.C at line 57 Source and target patch bounding boxes are not similar source box span : (8.50000286 2.59809914 1.49999989) target box span : (2.25992262 1.03910747 0.727020719) source box : (-3.5 -1.29906085 0) (5.00000286 1.29903829 1.49999989) target box : (-2 0.259930804 0.750000076) (0.25992262 1.29903828 1.4770208) inflated target box : (-2.12957193 0.130358877 0.620428149) (0.389494547 1.42861021 1.60659272) --> FOAM FATAL ERROR: Unable to set source and target faces Could anyone provide a idea of how to set these boundary conditions? Thanks in advance |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Join Date: Dec 2016
Posts: 6
Rep Power: 9 ![]() |
I've solved this problem!
The steps are okay but we cannot change the order of boundaries in constant/polymesh/boundary file. Just change the type! |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Jul 2017
Posts: 6
Rep Power: 9 ![]() |
Hi bowen1024
I have the same problem like yours, I have created two cellzones too through ICEM. boundary like yours I choiced cyclicAMI BCs. I selected pisoFoam solver, but there were some errors showed at the below jpg image. Now, could i send my case file to you and help me find out the reason which why it doesnt run. and my email:917443727@qq.com. And I would appreciate you. otherwise, it must be the best of you send your boundary file to me. In the end, I wonder if only manually change the 'boundary' file which in the consant/polyMesh/ folder after the command of 'fluentMeshToFoam'. best wishes |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Join Date: Dec 2016
Posts: 6
Rep Power: 9 ![]() |
Hello William,
The proper order would be: 1. "fluent3DMeshToFoam" to convet fluent mesh to openfoam format. 2. add a createPatchDict file in the system folder (perhaps you have to find a template for it) and then use "createPatch -overwrite". In the createPatchDict file, you may only have to write patches for cyclic BCs. However, this step would not change anything in the "constant/boundary" file. 3. You may then have to manually change the boundary settings in "constant/boundary" file. When I converted the fluent mesh to openfoam, the default type of the BCs were "wall". I changed certain BCs to cyclic or cyclicAMI. The last line means that: for example, you have: sidefaceL { type wall; nFaces xxx; ..... } inlet { type patch; nFaces xxx; ..... } sidefaceR { type wall; nFaces xxx; ..... } you can only change the type e.g. from wall to cyclic Do NOT try to rearrange the order of the boundaries in the boundary file, for example: inlet { type patch; nFaces xxx; ..... } sidefaceL { type cyclic; nFaces xxx; ..... } sidefaceR { type cyclic; nFaces xxx; ..... } 4. Finally, use "checkMesh" to ensure all the settings are correct! Best wishes, Bowen |
|
![]() |
![]() |
![]() |
Tags |
cyclic boundaries, cyclicami; |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Setting up cyclic boundary condition | KateEisenhower | OpenFOAM Pre-Processing | 6 | January 11, 2017 17:17 |
Can not find my own boundary conditions when running a solver | Eric Brant | OpenFOAM Running, Solving & CFD | 2 | November 7, 2016 20:08 |
Possible bug with stitchMesh and cyclics in OpenFoam | Jack001 | OpenFOAM Pre-Processing | 0 | May 21, 2016 08:00 |
OpenFOAM cases with cyclicAMI in tecPlot 360 | Aidan | Tecplot | 0 | January 24, 2016 10:57 |
CyclicAMI Boundary Condition | CUBoulderPhDStudent | OpenFOAM Running, Solving & CFD | 0 | May 21, 2014 18:34 |