CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Mesh for 3 dim Geometry

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 11, 2000, 04:21
Default Mesh for 3 dim Geometry
  #1
Phil
Guest
 
Posts: n/a
I have generated a 3-dim 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
  Reply With Quote

Old   July 11, 2000, 10:05
Default Re: Mesh for 3 dim Geometry
  #2
John C. Chien
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 un-structured, 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.
  Reply With Quote

Old   July 11, 2000, 11:26
Default Re: Mesh for 3 dim Geometry
  #3
Kai Kang
Guest
 
Posts: n/a
agree, try subdivide to more blocks and re-mesh each.

Another lazy way I have tried is to mesh the big block bottom-up, 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/sub-entity 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...

  Reply With Quote

Old   July 11, 2000, 11:39
Default Re: Mesh for 3 dim Geometry
  #4
John C. Chien
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.
  Reply With Quote

Old   July 11, 2000, 11:56
Default Thank you John but...
  #5
Phil
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 volume-meshing generates the points for the edges and begin with the face-meshing 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
  Reply With Quote

Old   July 11, 2000, 11:57
Default Thank you for your help
  #6
Phil
Guest
 
Posts: n/a
  Reply With Quote

Old   July 11, 2000, 12:26
Default Re: Thank you John but...
  #7
John C. Chien
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.
  Reply With Quote

Old   July 11, 2000, 20:45
Default Re: Mesh for 3 dim Geometry
  #8
Jonas Larsson
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 geometry-accuracy (adaption follows exisiting course mesh boundary and not the real geometry).
  Reply With Quote

Old   July 12, 2000, 00:11
Default Re: Mesh for 3 dim Geometry
  #9
John C. Chien
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 piece-wise 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 step-by-step. 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, pre-planning 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 one-by-one by hand. (7). So far, there is no simple solution to handle the complex geometry flow problem and the asociated mesh generation.
  Reply With Quote

Old   July 12, 2000, 04:39
Default Thank you John...
  #10
Phil
Guest
 
Posts: n/a
... you are a source of knowledge I searched for!!

Thanks Phil
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Mesh a geometry without stl file eysteinn OpenFOAM Native Meshers: snappyHexMesh and Others 0 May 5, 2011 10:15
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 17:06.