|
[Sponsors] |
[blockMesh] blockMesh multiple merging on same hex |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 13, 2018, 17:14 |
blockMesh multiple merging on same hex
|
#1 |
New Member
Join Date: Oct 2018
Posts: 19
Rep Power: 7 |
Hi,
I'm working on mesh which should be merged from four different sub-parts and I'm using blockMesh to do it. I'm on step where I have four blocks (see numbers on the enclosed image). But when I try to merge four boundaries (four dotted lines) only first two merges work fine and on the third merge there is always error like this: Code:
Creating merge patch pairs Adding point and face zones Creating attachPolyTopoChanger --> FOAM FATAL ERROR: Face 164393 reduced to less than 3 points. Topological/cutting error A. Old face: 2(74389 74570) new face: 2(74389 74570) From function void Foam::slidingInterface::coupleInterface(Foam::polyTopoChange&) const in file slidingInterface/coupleSlidingInterface.C at line 1461. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::slidingInterface::coupleInterface(Foam::polyTopoChange&) const at ??:? #3 Foam::polyTopoChanger::topoChangeRequest() const at ??:? #4 Foam::polyTopoChanger::changeMesh(bool, bool, bool, bool) at ??:? #5 Foam::attachPolyTopoChanger::attach(bool) at ??:? #6 ? in "/usr/bin/blockMesh" #7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #8 ? in "/usr/bin/blockMesh" Aborted (core dumped) This happens always on the third merge even if I change the order. So I guess first two are changing something on the geometry and makes next two meshes impossible. I'm using mergePatchPairs because I want to have different mesh sizes on merge faces. Does anyone have any idea what should I do to succeed in merging these four patches? Thanks, Krzysztof |
|
December 20, 2018, 00:03 |
|
#2 |
Senior Member
Join Date: Aug 2013
Posts: 407
Rep Power: 15 |
Hi,
There is a long-winded way to solve your problem. 1. Create the 4 meshes separately 2. Merge meshes 1 & 2 using mergeMesh. Let us call this mesh12 3. While this is happening, you can concurrently merge meshes 3 & 4 using mergeMesh as well. Let us call this mesh34 4. Use stitchMesh on mesh12 using the right patch of mesh 1 & left patch of mesh 2 are the master & slave patches. 5. After step 4, use createPatch to combine the top surfaces of mesh12 so that you have a single top patch (call top12). Similarly you can do for the bottom surfaces (call it bottom12). 6. Repeat 4 & 5 with mesh34. Call the respective patches top34 & bottom34. 7. Merge meshes mesh12 and mesh34. Call it mesh1234 8. Stitch mesh1234 using top12 and bottom34 as your master & slave patches. End result you will have a single mesh. Alternatively, since mergePatchPairs will work at least once, you could generate two of them together and then do a similar thing as above. So when you create your meshes, instead of creating 4 separate meshes, you could generate say mesh 1 & 2 together (and specify the merging patches in blockMeshDict itself) & do the same for mesh 3 & 4. You then follow step 8 from above with the correct patch names. Hope this helps. Cheers, Antimony |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[blockMesh] --> FOAM FATAL ERROR: Trying to specify a boundary face | A.A. | OpenFOAM Meshing & Mesh Conversion | 41 | June 26, 2020 07:06 |
[Other] mergeMatchPairs with arcs | vainilreb | OpenFOAM Meshing & Mesh Conversion | 1 | August 5, 2013 08:11 |
[blockMesh] apparently the mesh doesn't want to be created in one direction | Maxime Thomas | OpenFOAM Meshing & Mesh Conversion | 1 | August 18, 2012 06:05 |
[blockMesh] Blockmesh error - 2D scramjet | ishaninair | OpenFOAM Meshing & Mesh Conversion | 7 | March 18, 2011 00:14 |
CheckMeshbs errors | ivanyao | OpenFOAM Running, Solving & CFD | 2 | March 11, 2009 02:34 |