# TETRAEDRAL OR HEXAEDRAL MESH IN CFD

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

 April 25, 1999, 17:59 TETRAEDRAL OR HEXAEDRAL MESH IN CFD #1 Christophe David Guest   Posts: n/a Dear collegues, I am a new CFD engineer and I have one question : Can you tell me if the use of tetraedral mesh is not very dangerous. In fact, I heart a lot of people that they prefer to use a hexaedral mesh to be sure that the physic of the problem will be conserved. I am waiting your recommendations and your experience. Thanx in advance. Christophe.

 April 26, 1999, 04:41 Re: TETRAEDRAL OR HEXAEDRAL MESH IN CFD #2 Dave Minns Guest   Posts: n/a Hi, I think most people would like to use a hex mesh at all times but often the geometry may be too complex or just not suited to hex meshing. Also the time taken to generate a hex mesh can be far longer than a tet mesh. For example, I have worked on a mesh for the external flow around an INDY (I think they have changed the name, but cannot remember it) racing car including mirrors, gearbox and support arms. A tet grid takes a couple of days but I wouldn`t even attempt to start hex meshing it. I hope my views are of some help regards David http://www.topologies.co.uk

 April 26, 1999, 04:45 Re: TETRAEDRAL OR HEXAEDRAL MESH IN CFD #3 Heinz Wilkening Guest   Posts: n/a Ciao Christophe, why should hexaedral meshes conserve physics better than tetrahedral meshes. Physics itself is, as long as you do not look at cristalls, is neither one nor the other. But this does not answer your question. I have used both methods, and I think, that for certain problems (eg. rectangular geometry) hexaedral meshes are more accurate. You can resolve a shock without much effort if the gridlines fit the shock. Hexaedral meshes are also cheaper in memory and cpu-time per node, but using a tetrahedral mesh sometimes you can save a lot of nodepoints, because terahedral meshes are more flexible. For complex geometries grid generation might be easier with tetraheral meshes. With hexaheral meshes you have to use multi-block methods. If you then also add mesh adaptation to the problem, tetrahedral meshes do not produce hanging nodes. To overcome all this pro and contra some people suggest hybrid meshes. I am sorry not to give a more definite answer. Ciao Heinz

 April 26, 1999, 10:02 Re: TETRAEDRAL OR HEXAEDRAL MESH IN CFD #4 Alberto Tamm Guest   Posts: n/a Hello Christophe, I donīt have to much experience with CFD, but one of my first models I do it with hexahedral and tretahedral mesh. It was a hydrocyclone for separing a kind of oil (rho=0.84) from water for the mining industrie. Firts I modelled it with tre (about 2 mill cells, Origin 2000, 4 Pros, 2 GRam) and the solution didnīt converge. After that I do it with hex and the V tang profiles seems as the experimental measurments doing with LDV. Hex is rapid and mostly are the difusion erros lower than with tre. In my opinion for complex models (rotating, high swirl, etc) itīs better model the geometry with hex. At the beginnin you must invest much work and time, but later you will be reward. Now I model a pump with hex (712.000 cells) and for having a good mesh it is the only way to modell it, because with tre a good grid will be much greater . I need all the Ram for solving the problem so I must save resource because the modell is to big for my machine (a Pentium II with 512 MRam). An other example is a Submarine what I modelled with tre grid. The geometry was to complex for hex grid and I have study only the force. resuming I think: always try to model it with hex grid (you save resource and can use it for increase your modell or solve your problem much rapidly.) If the geometry is to complex and the model are "simlpe" (nothing is simple)(without movin parts, high swirl, multi-phase, etc) use tre grid. I hope my recomendation help you in your work. Alberto Tamm tamm@tfa.maschinenbau.tu-darmstadt.de

 April 26, 1999, 14:55 Re: TETRAEDRAL OR HEXAEDRAL MESH IN CFD #5 John C. Chien Guest   Posts: n/a (1). Based on my experience with a commercial code, it is hard to get reliable wall parameters ( skin friction, heat transfer ) by using tet-mesh. (2). This is because in 2-D or 3-D, a large number of triangular cells are required near the wall to avoid the cell skewness problem. In other words, the dimension of the cell in the parallel to wall direction(lateral) must be reduced to the cell size in the normal to wall direction to minimize the cell skewness. So, if you use a low Reynolds number model with Y+ =1 as the first cell size, then cell size in the parallel to wall directions must also be kept near this value ( to avoid high skewness cells). (3). In 3-D, this approach requires excessive number of cells near the surface of the wall. (4). The alternative is to use hex cells or prism cells,where the lateral dimension of the cell can be made much larger than the normal to wall dimension, without creating too much a problem. This makes the computation of 3-D problem practical. (5). So, the conclusion is : it is hard to use fine tet-mesh to cover the boundary-layer-like region of the flow, whether it is a wall boundary layer, a mixing layer, or a thin shock layer. (6). Hybrid mesh is the one which uses hex or prism cells near the wall, while the tet-mesh is used away from the wall. It is a good idea to experiment with different mesh types or arrangements for the problem being solved, especially if you are after the solutions in the boundary layers.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post mani CFX 4 March 7, 2007 04:41 hung FLUENT 7 April 18, 2005 09:38 Gennady Kireyko Main CFD Forum 0 May 6, 2001 11:13 John C. Chien Main CFD Forum 36 January 24, 2001 22:10 Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27

All times are GMT -4. The time now is 08:50.