|
[Sponsors] |
[blockMesh] Error in BlockMesh: inconsistent number of faces |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 19, 2010, 04:48 |
Error in BlockMesh: inconsistent number of faces
|
#1 |
New Member
Join Date: Aug 2010
Posts: 4
Rep Power: 16 |
Hi there,
I'm trying to develop a trapezoidal-shaped channel in BlockMesh, consisting of 2 three-sided prism and in between a normal cuboid. In the attached PDF-file you can find a sketch of the geometry. Below the blockMesh is posted. My problem is that when I'm trying to define different number of cells in x and in y direction like for example: blocks ( hex (3 2 2 3 7 6 5 4) (1300 50 10) simpleGrading (1 1 1) hex (3 9 8 2 7 11 10 6) (1300 50 10) simpleGrading (1 1 1) hex (8 9 9 8 10 11 15 14) (1300 50 10) simpleGrading (1 1 1)) ); I get the following error: [...] Inconsistent number of faces between block pair 0 and 1 From function blockMesh::createMergeList() in file createMergeList.C at line 196. FOAM exiting If I define the mesh as follows: blocks ( hex (3 2 2 3 7 6 5 4) (100 100 10) simpleGrading (1 1 1) hex (3 9 8 2 7 11 10 6) (100 100 10) simpleGrading (1 1 1) hex (8 9 9 8 10 11 15 14) (100 100 10) simpleGrading (1 1 1)) ); everything works fine. Can anyone tell me how to solve this problem? I don't know what I have to change to get this working. I'm thankful for any advice. Regards, pc1 my BLOCKMESH: /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.5 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1.; vertices ( (0 0 0) // 0 (0 40 0) // 1 (0.48 40 0) // 2 (0.48 0 0) // 3 (0 0 0.16) // 4 (0 40 0.16) // 5 (0.48 40 0.16) // 6 (0.48 0 0.16) // 7 (1.72 40 0) // 8 (1.72 0 0) // 9 (1.72 40 0.16) // 10 (1.72 0 0.16) // 11 (2.2 40 0) // 12 (2.2 0 0) // 13 (2.2 40 0.16) // 14 (2.2 0 0.16) // 15 ); blocks ( hex (3 2 2 3 7 6 5 4) (1 1 1) simpleGrading (1 1 1) // p hex (3 9 8 2 7 11 10 6) (1 1 1) simpleGrading (1 1 1) //q hex (8 9 9 8 10 11 15 14) (1 1 1) simpleGrading (1 1 1) // r ); edges ( ); patches ( //left: Prism p wall xminp ( (4 5 2 3) ) patch yminp ( (3 7 4 3) ) patch ymaxp ( (2 5 6 2) ) patch zminp ( (3 2 2 3) ) patch zmaxp ( (4 7 6 5) ) // middle: cuboid q patch yminq ( (7 11 9 3) ) patch ymaxq ( (6 2 8 10) ) wall zminq ( (2 3 9 8) ) patch zmaxq ( (11 7 6 10) ) // right: Prism r wall xmaxr ( (15 9 8 14) ) patch yminr ( (15 11 9 15) ) patch ymaxr ( (14 8 10 14) ) patch zmaxr ( (15 14 10 11) ) patch zminr ( (8 9 9 8) ) ); mergePatchPairs ( ); // ************************************************** *********************** // |
|
August 19, 2010, 07:11 |
|
#2 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi pc1,
there are numbering problems in your blockMeshDict. Try this one: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.5 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1.; vertices ( (0 0 0) // 0 (0 40 0) // 1 (0.48 40 0) // 2 (0.48 0 0) // 3 (0 0 0.16) // 4 (0 40 0.16) // 5 (0.48 40 0.16) // 6 (0.48 0 0.16) // 7 (1.72 40 0) // 8 (1.72 0 0) // 9 (1.72 40 0.16) // 10 (1.72 0 0.16) // 11 (2.2 40 0) // 12 (2.2 0 0) // 13 (2.2 40 0.16) // 14 (2.2 0 0.16) // 15 ); blocks ( hex (4 3 2 5 4 7 6 5) (1300 50 10) simpleGrading (1 1 1) // p hex (3 9 8 2 7 11 10 6) (1300 50 10) simpleGrading (1 1 1) //q hex (9 15 14 8 11 15 14 10) (1300 50 10) simpleGrading (1 1 1) // r ); edges ( ); patches ( //left: Prism p wall xminp ( (4 3 2 5) ) patch yminp ( (4 3 7 4) ) patch ymaxp ( (2 6 5 2) ) //patch zminp //( //(3 2 2 3) //) patch zmaxp ( (4 7 6 5) ) // middle: cuboid q patch yminq ( (3 9 11 7) ) patch ymaxq ( (2 8 10 6) ) wall zminq ( (3 9 8 2) ) patch zmaxq ( (7 11 10 6) ) // right: Prism r wall xmaxr ( (9 15 14 8) ) patch yminr ( (9 15 15 11) ) patch ymaxr ( (14 10 8 14) ) patch zmaxr ( (11 15 14 10) ) //patch zminr //( //(8 9 9 8) //) ); mergePatchPairs ( ); // ************************************************** *********************** // Martin |
|
August 19, 2010, 10:19 |
Same error occured again
|
#3 |
New Member
Join Date: Aug 2010
Posts: 4
Rep Power: 16 |
Hello Martin,
thanks for your reply. I just tested to turn the numbers as you proposed and removed the "interior" walls. Unfortunately I still get the same Error: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Creating block mesh from "*********/mesh/constant/polyMesh/blockMeshDict" Creating blockCorners Creating curved edges Creating blocks Creating patches Creating block mesh topology Default patch type set to empty --> FOAM Warning : From function polyMesh::polyMesh(... construct from shapes...) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577 Found 2 undefined faces in mesh; adding to default patch. Check block mesh topology Basic statistics Number of internal faces : 2 Number of boundary faces : 14 Number of defined boundary faces : 14 Number of undefined boundary faces : 0 Checking patch -> block consistency Creating block offsets Creating merge list Inconsistent number of faces between block pair 0 and 1 From function blockMesh::createMergeList() in file createMergeList.C at line 196. FOAM exiting The first Warning appears because of the removed walls, which are not really walls but rather edges. In a test with a single three-sided prism I found out that I have to define them. The shifting of the numbers doesn't have any effect on the result. The biggest problem is the inconsistent number of faces between the blocks. Still have no idea how to solve it. Any proposals? Regards, pc1 |
|
August 19, 2010, 10:40 |
|
#4 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
Hi,
after adding Code:
empty dummies ( (4 5 5 4) (15 14 14 15) ) Code:
checkMesh -allTopology -allGeometry Does it run anyway? Martin |
|
August 19, 2010, 10:45 |
|
#5 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
And did you really tried my blockMeshDict? I don't have the inconsistent number of faces problem here...
|
|
August 19, 2010, 14:12 |
tried your BlockMeshDict and checkMesh, both failed
|
#6 |
New Member
Join Date: Aug 2010
Posts: 4
Rep Power: 16 |
Hi,
I did try your BlockMeshDict, but unfortunately BlockMesh aborted because of the inconsistent number of cells. Don't know why you don't have the same problem with the BlockMesh? My CheckMesh also failed. Is there an other possibility to define such a geometry in the BlockMeshDict? Or does anyone else have some advice for me? Tomorrow I'll continue searching for the reason of this error... pc1 |
|
August 19, 2010, 18:37 |
|
#7 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 22 |
What about this idea:
Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.5 | | \\ / A nd | Web: http://www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 1.; vertices ( (0 0 0) // 0 (0 40 0) // 1 (0.48 40 0) // 2 (0.48 0 0) // 3 (0 0 0.16) // 4 (0 40 0.16) // 5 (0.48 40 0.16) // 6 (0.48 0 0.16) // 7 (1.72 40 0) // 8 (1.72 0 0) // 9 (1.72 40 0.16) // 10 (1.72 0 0.16) // 11 (2.2 40 0) // 12 (2.2 0 0) // 13 (2.2 40 0.16) // 14 (2.2 0 0.16) // 15 (0.6 0 0.08) // 16 (0.6 40 0.08) // 17 (1.6 0 0.08) // 18 (1.6 40 0.08) // 19 ); blocks ( hex (5 6 7 4 2 17 16 3) block1 (11 1300 10) simpleGrading (1 1 1) // p hex (2 17 16 3 8 19 18 9) block2 (11 1300 50) simpleGrading (1 1 1) //q hex (17 6 7 16 19 10 11 18) block3 (10 1300 50) simpleGrading (1 1 1) // r hex (10 14 15 11 19 8 9 18) block4 (11 1300 10) simpleGrading (1 1 1) // s ); edges ( ); patches ( patch xFront ( (4 3 16 7) (3 9 18 16) (9 15 11 18) (16 18 11 7) ) patch xBack ( (5 2 17 6) (2 8 19 17) (17 19 10 6) (8 14 10 19) ) patch yLeft ( (3 2 5 4) ) patch yRight ( (8 9 15 14) ) patch zBottom ( (3 9 8 2) ) patch zTop ( (4 7 6 5) (7 11 10 6) (11 15 14 10) ) ); mergePatchPairs ( ); // ************************************************** *********************** // Martin |
|
August 20, 2010, 07:24 |
|
#8 |
New Member
Join Date: Aug 2010
Posts: 4
Rep Power: 16 |
Great!
That one works fine! Thank you for your help!!! Regards, pc1 |
|
Tags |
blockmesh, number of faces |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Layers not growing at all | zonda | OpenFOAM Meshing & Mesh Conversion | 12 | June 6, 2020 12:28 |
[snappyHexMesh] SHM is not extruding/adding Layers everywhere | matthiasd | OpenFOAM Meshing & Mesh Conversion | 2 | October 16, 2016 17:45 |
[mesh manipulation] Importing Multiple Meshes | thomasnwalshiii | OpenFOAM Meshing & Mesh Conversion | 18 | December 19, 2015 19:57 |
[snappyHexMesh] No layers in a small gap | bobburnquist | OpenFOAM Meshing & Mesh Conversion | 6 | August 26, 2015 10:38 |
AMI interDyMFoam for mixer | danny123 | OpenFOAM Running, Solving & CFD | 4 | June 19, 2013 05:49 |