Hi! I have a problem with meshing two pipes which are connected, but one of them are non-real volume and the second one is real. Real pipe I would like to mesh using the block-strukture mesh for example "Quad/submap or map" interval size 1.3 or less on faces and on the second pipe "Tri/pave". Unfortunatly if I mesh down real pipe I can not mesh the up non-real pipe using the Tet/hybrid. The upper pipe is non-real because inside I put some inserts. These two pipes have one face in place where they are connected. Maybe someone could help me. Best regards Paulina

Hi Paulina

I want that you now that the prediction of velocity profiles in tetrahedral mesh is very poor in my opinion, there is a relatively high numerical difussion for the prediction of pipe flow in 3D. I strongly suggest that you use a hexahedral mesh for both volumes.

It is my guess that you are working in a 3-D, if you are working in 2D I could not tell you what could be the prediction using tetrahedral grid.

Best regards

Alex Munoz

Hi Alex, Thank you for your response. Yes, I work in a 3D and I know about numerical diffusion in modelling in pipe.Numerical diffusion is main reason why I want to change the type of the mesh inside the first pipe. In second pipe I couldn't change mesh from nonstructure to structure,because I put into the pipe 6 SMX inserts. These inserts are very complicate and with them it is impossible to mesh using structure grid. So, now I try to find the way how connect to volume one real and the other one non-real and in how way mesh them using structure and non-structure grids. Maybe have you got some idea? Thanks for your advice. Best regards. Paulina

Hi Paulina

I know it is posible to have to types of mesh, I have seen in Fluent tutorial something similar to what you want to do under the name of hybrid mesh.

If the complexity of the geometry force you to use unstructural mesh, why you want to made a hybrid mesh? As long as the velocity profile reaches the unstructural mesh the numerical difusion takes place!!

Best regards

Alex

Hi Alex,

I have use the type of mesh TGrids (this is unstructural grid) for my inserts. I have not got any other solution, because that static mixer is very diffult geometry. Using the unstructural grid is only one way which I know.

I tried to mesh the mixer using the structural grids, but without success. Inside these inserts I didn't observe numerical diffusion. It takes place before inserts. It takes place especially at the inlet to empty pipe which it is put before the inserts. My geometry consists from empty pipe with a length 55 [mm], six SMX inserts with a length 165 [mm] and second empty pipe before inserts 137.5 [mm].

Nowadays I cann't see any other solution as mesh first pipe using the structural mesh and the inserts and the second pipe - unstrutural mesh.

I will be very greatfull if you could send me an information where you read about that topic in Fluent tutorial.

Best regards

Paulina

simply mesh your "empty pipe" volume first using Cooper scheme. After that, mesh "the pipe with inserts" using TGrid scheme. This way Gambit will automatically create a layer of prism cells/caps between these two zones.

anna

Hi Paulina

Anna give you a way, However, you should be careful to provide such a wise cells sizes so that you don't run in a high skewnwess in the transtion between the to meshes.

About the hybrid mesh, please I can tell the key words, it is up to you if you search in Fluent support web side, of course you or you company must to be register to have access to this files.

regards

Alex Munoz

Hi Anna,

Thanks for your help. I have done as you told. It works but I can mesh my geometry only with interval size 1.3 and 1.5, which give me a coarses grids. I need much more fine grids. When I want to mesh using the interval size for example 1.0 or less, Gambit didn't mesh the geometry.

Anyway last night I solved the problem with meshing nonreal and real volumes.

Once again, thanks for your advice.

Best regards

Paulina

Hi Alex,

Thanks for your an advice and an information. According to Fluent support web side I will talk with my professor.

Thanks for help.

Best regards

Paulina

use interval count instead of interval size for edge meshing first. That way you can control edge meshing, and visualize the density of nodes on the edges (coarse or fine). After edge meshing, go to face/surface meshing, and mesh them. Then go to volume mesh where you assign the size of the cell you want.(not interval size). In case of your first pipe which you will mesh using Cooper scheme, edge nodes have to be even number for base faces which you will maesh in the next step using quad/pave scheme. Side faces will be meshed in map/submap and don't have to have even number of edge nodes. After meshing faces, and checking their quality, mesh the volume using Cooper, and assign size of the cell you want.

anna

[goyalnn]

I have created a hospital room geometry whcihis divided into three volumes. Is it possible to mesh non-real volumes without converting into real ones?

[roukaia]

i need to simulate an IC engine (lister petter) so i tried to reproduce the same geometry as the tutoriel in-cylinder mesh
now i have no idea about how to construct the mesh (structured and non structured mesh in one face) in the valve
i need the valve layering zones to in structered (quad) because o the layering
have you got any idea how to do it in gambit