
[Sponsors] 
July 11, 2000, 04:21 
Mesh for 3 dim Geometry

#1 
Guest
Posts: n/a

I have generated a 3dim geometry and I have meshed this volume with Tet/Hyb Elements (Type T Grid) with spacing 0.001 (Intervall Size). I have seen that the mesh is not fine enough so I triede to mesh it with an intervall size of 0.0005. During the initialization of the Tetrahedral meshing, in the Transcript zone the following sentence is written: Initialization failed; perturb boundary nodes and try again.
Then: Err[3900] TG_Mesh_Domain failed with error code 1  Err [4608] Tetraheral meshing has failed for volume volume 1. This is usually caused by problems in the face meshes. Check the skewness off your face meshes and make sure the face meshes are not to large in areas of small gaps. Can someone explain to me what I can change to generate a finer mesh? Thanks for your help 

July 11, 2000, 10:05 
Re: Mesh for 3 dim Geometry

#2 
Guest
Posts: n/a

(1). The only successful method is to subdivide the geometry into smaller blocks. Several hundreds if necessary. (2). You shouldn't have the problem if you are dealing with simple cubes. So, check out the fine mesh for a cube first. If you still fail , then that's the best you can do with the code. (3). With several geometry and mesh codes I have used recently, whether it is structured or unstructured, they all have the same problem. I think, it is related to the algorithm used in the mesh generation, geometry representation, and accuracy of math used. (4). In some cases, I had to try 30 to 100 times in order to get a good mesh, using one code. Well, that's life. (5). So, if you can pass the simple cube test, then try to model the geometry using more patches or blocks.


July 11, 2000, 11:26 
Re: Mesh for 3 dim Geometry

#3 
Guest
Posts: n/a

agree, try subdivide to more blocks and remesh each.
Another lazy way I have tried is to mesh the big block bottomup, as the old versions of FIDAP used to do. First mesh the edges, with good graident for smaller geometries (small edge/face). Then the Face, find the ones you think is important. When mesh the volume in Gambit, be sure to turn off the delete old mesh/subentity option. By playing with edge intervals it will solve the mesh for those relatively small/detailed geometries compare to the big volume. Most of the time, it is just because the complication of the geometry which the algorithm is not that intelligent to handle yet and you need to give it some more information or limit its freedom... 

July 11, 2000, 11:39 
Re: Mesh for 3 dim Geometry

#4 
Guest
Posts: n/a

(1). Very good. I agree with you. (2). I think, geometry and meshing is still a wide open field which needs more "smart" or "intelligent" algorithms.


July 11, 2000, 11:56 
Thank you John but...

#5 
Guest
Posts: n/a

... I think it is not possible to subdivide my geometrie into smaller blocks. The problem with my geometry is, that the upper (wall) side of my volume touchs in one several points the lower (wall) side. So if I generate a mesh, the volumemeshing generates the points for the edges and begin with the facemeshing and then the two meshes (upper wall and lower wall) cross each other. I think this is the problem, so a volume mesh cannot be generated for this geometry. I haven't got the problem, when I change the distance to a (physicaly) tolerable value, so that there is a small gap between the upper and lower wall. Tell me if you would agree with.
Thank you for your help Phil 

July 11, 2000, 11:57 
Thank you for your help

#6 
Guest
Posts: n/a



July 11, 2000, 12:26 
Re: Thank you John but...

#7 
Guest
Posts: n/a

(1). I think I know what you are trying to say. That is, the geometry must be modelled first. (2). This is something I have been trying to say in many occasions. Taking the geometry directly from the CAD is not the best approach. (3). You can either leave a gap or seal the gap, depending upon the importance of the design. And if you need the gap, create a separate block and put a fine mesh there.


July 11, 2000, 20:45 
Re: Mesh for 3 dim Geometry

#8 
Guest
Posts: n/a

I quick way to get a finer grid is to do refinement/adaption inside Fluent on every cell in the coarse grid  this should work but you might loose some geometryaccuracy (adaption follows exisiting course mesh boundary and not the real geometry).


July 12, 2000, 00:11 
Re: Mesh for 3 dim Geometry

#9 
Guest
Posts: n/a

(1). Yes, mesh refinement in the solver is very useful, when the solution away from the wall is complicated. Using the adaptive mesh refinement, one can "bring out" the fine detail of the solution in the flow field. (2). But the mesh near the wall (curved walls) must be fine enough right from the begining. This is because the wall surface is actually replaced by the mesh. And the wall is replaced by the piecewise linear shape. In the solver, the mesh refinement can only occur on the linear segment. Thus, the original mesh not only define the flow field solution accuracy but also fixed the surface shape.(diamond shape surface) (3). For flow over a smooth blade or airfoil, it is very important to start with fine mesh on the blade surface right from the begining. I once created a corase mesh for transonic flow over a blade. In the Rampant solver, I refined the mesh stepbystep. The end result was, I was able to pick up the trailing edge shock. But I also realized that waves are also generating from the diamond shape surface which was created by the use of the corase mesh at the begining. (4). So, preplanning before creating a mesh (which can have a permanent effect on the geometry and the solution) is essential. This is also very important for the cavity flow problem with cooling, seal, and leakage flow. The spacing in certain part of the flow field is very small. The flow field must be predicted accurately in order to get accurate mass flow rate. In these cases, it is convenient to divide the flow field based on the geometry into a series of blocks. In this way, one can easily distribute the mesh in the right regions. (5). The difficulty is because the solution, the mesh and the mesh are now all coupled together. We need to know the solution, in order to plan the mesh distribution. And the mesh distribution is in most cases affected by the geometry requirement. (6). So, Ideally, the mesh is the last thing to determine. (after the solution and the geometry) Unfortunately, we need the geometry and the mesh first in order to get a solution. To create a proper mesh, it is not uncommon to have 100 edge curves,where the nodal point distribution is controlled onebyone by hand. (7). So far, there is no simple solution to handle the complex geometry flow problem and the asociated mesh generation.


July 12, 2000, 04:39 
Thank you John...

#10 
Guest
Posts: n/a

... you are a source of knowledge I searched for!!
Thanks Phil 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to set periodic boundary conditions  Ganesh  FLUENT  15  November 18, 2020 06:09 
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation  tommymoose  ANSYS Meshing & Geometry  48  April 15, 2013 04:24 
[snappyHexMesh] Mesh a geometry without stl file  eysteinn  OpenFOAM Meshing & Mesh Conversion  0  May 5, 2011 10:15 
fluent add additional zones for the mesh file  SSL  FLUENT  2  January 26, 2008 11:55 
unstructured vs. structured grids  Frank Muldoon  Main CFD Forum  1  January 5, 1999 10:09 