|
[Sponsors] |
February 9, 2011, 00:39 |
block mesh wedge
|
#1 | |
Member
William
Join Date: Feb 2011
Location: Minnesota USA
Posts: 33
Rep Power: 15 |
Hey,
I'm having a hard time getting the wedge to look right. Can somebody tell me what I am doing wrong. Quote:
|
||
February 12, 2011, 07:25 |
|
#2 |
New Member
Radko Bankras
Join Date: Jul 2010
Location: Almere, The Netherlands
Posts: 5
Rep Power: 16 |
billynoe,
Your wedge looks better if you don't split up your blocks, so: Code:
hex (3 31 45 3 0 30 44 0) (1 1 1) simpleGrading (1 1 1) hex (2 18 32 2 1 19 33 1) (1 1 1) simpleGrading (1 1 1) hex (21 25 39 35 20 22 36 34) (1 1 1) simpleGrading (1 1 1) hex (27 41 35 21 29 43 39 25) (1 1 1) simpleGrading (1 1 1) hex (38 42 40 37 24 28 26 23) (1 1 1) simpleGrading (1 1 1) I guess the AER patch defines internal walls in the wedge of your cylinder. In that case I would define only the blocks which form the volume of your wedge together. This way it is easier to increase the grading in X and Y direction, and you can keep your wedge 1 cell thick. Kind regards, Radko Last edited by Radko; February 12, 2011 at 07:25. Reason: style |
|
February 14, 2011, 12:08 |
|
#3 |
Member
William
Join Date: Feb 2011
Location: Minnesota USA
Posts: 33
Rep Power: 15 |
Yes that definitely fixed the shape I changed the faces to (1 1 1) on the AER block and input output and (15 1 5) on the wedge. I am getting errors in checkMesh from the internal walls. I think I will need to use snappyHex to join the blocks is this correct?
|
|
February 15, 2011, 17:40 |
|
#4 |
New Member
Radko Bankras
Join Date: Jul 2010
Location: Almere, The Netherlands
Posts: 5
Rep Power: 16 |
Hi,
Any other mesher would be easier to use for your design. I suggest to have a look at Salome for drawing, meshing, and exporting to Foam via ideasUnvToFoam. This will allow you to perform the logical actions of subtracting two solids, like I guess you are trying to achieve. As an example of how the structure should be defined in blockMesh (for all I know), I have modified your file and added some extra points. Note that your AER structure has not been put in yet. It will take a few more hours to do so. Make sure the patches are defined in clock-wise direction when looking from inside the mesh. Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 0.146; vertices ( (0 241.3 0) //0 (0 0 0) //1 (0 -12.7 0) //2 (0 -1524 0) //3 (279.4 -12.7 0) //4 (279.4 0 0) //5 (292.1 38.1 0) //6 (292.1 -313.6926357352644 0) //7 (304.8 38.1 0) //8 (304.8 13.51505771044411 0) //9 (304.8 0 0) //10 (304.8 -304.8 0) //11 (863.6 216.9016246183983 0) //12 (863.6 -521.7016246183977 0) //13 (867.943655820235 204.9675283344171 0) //14 (867.943655820235 -509.767528334418 0) //15 (7620 241.3 0) //16 (7620 -1524 0) //17 (279.1341 -12.7 12.1873) //18 (279.1341 0 12.1873) //19 (291.822 38.1 12.7412) //20 (291.822 -313.6926357352644 12.7412) //21 (304.5099 38.1 13.2952) //22 (304.5099 13.51505771044411 13.952) //23 (304.5099 0 13.29522) //24 (304.5099 -304.8 13.2952) //25 (862.7780 216.9016246183983 37.6697) //26 (862.7780 -521.7016246183977 37.6697) //27 (867.1176 204.9675283344171 37.8592) //28 (867.1176 -509.767528334418 37.8592) //29 (7612.7474 241.3 332.3797) //30 (7612.7474 -1524 332.3797) //31 (279.1341 -12.7 -12.1873) //32 (279.1341 0 -12.1873) //33 (291.822 38.1 -12.7412) //34 (291.822 -313.6926357352644 -12.7412) //35 (304.5099 38.1 -13.2952) //36 (304.5099 13.51505771044411 -13.2952) //37 (304.5099 0 -13.2952) //38 (304.5099 -304.8 -13.2952) //39 (862.7780 216.9016246183983 -37.6697) //40 (862.7780 -521.7016246183977 -37.6697) //41 (867.1176 204.9675283344171 -37.8592) //42 (867.1176 -509.767528334418 -37.8592) //43 (7612.7474 241.3 -332.3797) //44 (7612.7474 -1524 -332.3797) //45 (279.1341 241.3 12.1873) //46 new (279.1341 241.3 -12.1873) //47 new (279.1341 -1524 12.1873) //48 new (279.1341 -1524 -12.1873) //49 new (7612.7474 0 332.3797) //50 new (7612.7474 0 -332.3797) //51 new (7612.7474 -12.7 332.3797) //52 new (7612.7474 -12.7 -332.3797) //53 new ); blocks ( hex (3 48 49 3 2 18 32 2) (20 1 20) simpleGrading (1 1 1) //0 hex (1 19 33 1 0 46 47 0) (20 1 10) simpleGrading (1 1 1) //1 hex (48 31 45 49 18 52 53 32) (100 1 20) simpleGrading (1 1 1) //2 hex (18 52 53 32 19 50 51 33) (100 1 5) simpleGrading (1 1 1) //3 hex (19 50 51 33 46 30 44 47) (100 1 10) simpleGrading (1 1 1) //4 ); patches ( wall Top ( (0 46 47 0) (46 30 44 47) ) wall bottom ( (3 49 48 3) (48 49 45 31) ) wall back ( (31 45 53 52) (52 53 51 50) (50 51 44 30) ) patch inlet ( (2 18 32 2) ) patch outlet ( (1 33 19 1) ) wall nub ( (18 19 33 32) ) wedge side1 ( (3 2 18 48) (1 0 46 19) (48 18 52 31) (18 19 50 52) (19 46 30 50) ) wedge side2 ( (3 2 32 49) (1 0 47 33) (49 32 53 45) (32 33 51 53) (33 47 44 51) ) empty zoinks ( (3 2 2 3) (1 0 0 1) ) ); mergePatchPairs ( ); Last edited by Radko; February 15, 2011 at 17:43. Reason: no comments |
|
February 15, 2011, 18:01 |
|
#5 |
Member
William
Join Date: Feb 2011
Location: Minnesota USA
Posts: 33
Rep Power: 15 |
Thanks for the help Radko.
I have been using gmsh for converting and meshing iges files which is ok, but I have been having problems with makeAxialMesh specifically collapseEdges. I also tried just reassigning the generic patches created in gmshToFoam into wedge type which did not work. Do you know of another way to make wedge geometry? Beyond that I tried a 3D test case icoFoam using the gmshToFoam mesh assigning the sides of the wedge as "walls" as well as the other patches. Except output as constant velocity 1.3 m/s and input as 0 pressure just to see what would happen and the solution wouldn't converge after about 10 steps. Maybe I should set it as a negative pressure on input? I am basically trying to model a vertical mixer I know the velocity in the volute due to an impeller, which I am simplifying. Eventually I will need to model this as interfoam as the top surface is exposed to air. So this looks like it is going to be a long time before I get any data that is worth anything. I will try out the revised geometry tomorrow and I'll let you know how it goes. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
3D Hybrid Mesh Errors | DarrenC | ANSYS Meshing & Geometry | 11 | August 5, 2013 07:42 |
blockMesh: block with 6 vertexes | dani | OpenFOAM | 3 | June 25, 2009 14:13 |
Bug in blockMesh | feymark | OpenFOAM Bugs | 8 | March 24, 2009 23:11 |
basic of mesh refinement | arya | CFX | 4 | June 19, 2007 13:21 |
Icemcfd 11: Loss of mesh from surface mesh option? | Joe | CFX | 2 | March 26, 2007 19:10 |