here is my problem? I want to mesh a volume which have two parts. One is too big size compared with another. i know i should divide the volume into two parts. I meshed one with 20 (interval size ), another with 4. but when i export the whole mesh to fluent. Fluent give me a worning: "non-positive volume exist".

How to handle with the interface meshing when we mesh a volume wiht two parts that have big different size? or some other methods?

thanks a lot

use tgrid or tmerge to first merge or unite the two different grid meshes. Open tgrid and read the two mesh files and just save them to a new mesh file. Then open the new mesh file in fluent. In fluent you can merge or fuse the two interfaces into a common inteface or interior zone. You can do that in tgrid also.

thanks,anindaya. i try with your method,it is ok. but when i smooth/swap the mesh, fluent give warning : no face with given nodes and Error: swap_3_to_2: face w node not edge etc. how can i handle with it ? is there any rules i have to comply when i mesh a volume with two diffrent grid meshs?

I am not sure what the problem is. But if you created the two volumes separately and mesh them separately too and used tgrid then you would not have any problem. Just see when you create your two volumes, see that they have proper coordinates and locations.

Else you can let me know exactly how you created the meshes and what you did next. Also what type of mesh is it.. structured or unstructured?

thanks for your reply, anindya the volume i meshed is a draft tube which compose two parts: a cone, a elbow .they holds a common interface. the meshing process is listed as follows: 1. firstly mesh the interface1 with structured face mesh with interval size 10 then mesh the volume by hybrid grid with interval size 10. 2. define the inlet in cone with velocity inlet and interface 1 with interface(volume 1);export the mesh with name 1.msh 3.delete volume 1 and here exists only volume 2 in the gambit. 4.mesh the interface2 on the elbow with structured face grid with the same interval size 10 as interface 1 then mesh the elbow by hybrid grid with the interval size 20 5.define the outlet in elbow with and interface 2 with interface;export the mesh with name 2.msh 6. start tgrid and open these two mesh and save as 1+2.msh 7. open fluent and read 1+2.msh then there is a note note :Separating wall zone 3 into zones 3 and 1.

wall:0 -> wall:0 (3) and wall:001 (1) Warning: Number of nodes read (95043) does not match number referenced (92479).Resetting counter to match the number referenced. 8 i scale the mesh with 0.001 in x,y.,z. and check the grid . it is still ok 9.smooth and swap the mesh and check the grid again then problem comes up: "grid check fails"

would you help ?

I would suggest that you do this.

Create the two volumes separately, i.e., run gambit twice separately to create the two meshes, say a.msh and b.msh. Use whatever method you choose to make the meshes and then define the interfaces, say interface-a and interface-b.

Open tgrid and read the two mesh files. Here in the window for reading the files, left click on the mesh files a.msh and b.msh so that both the file are now under Mesh File(s). Then press ok . After that a window appears called "working". After that window disappears, now go to Write/Mesh. Then give the name of the combined mesh as say a-b.msh in Mesh File(s) and click on ok.

Then close tgrid and open Fluent. Read a-b.msh and do the grid check and scaling and smooth and swap. I believe there would not be any problems now. After that you can use the merge command under Grid to merge the two interfaces into an interior zone and then start defining your other problem parameters.

Let me know if that works.

anindya, thanks a lot. i have try with your method. it is ok.Thanks. some thing i have to methion is that i must use hybrid mesh with two parts. if not, although there are no promlem with smooth/swap and check , when i merge this two parts and then check , check fails. do you have more advices about this---merge two different meshes ( one is hybrid, another is structure mesh like map ) and then check anyway, the problem is cracked.

thanks you

anindya, how to merge the two interfaces into an interior zone? i can merge the two interfaces into a common interface,how can i make the interface be a interior ?

after merge the two interfaces to be a common face and define other boundary condition, i start iteration but it can not converge. but when i unite the two parts in Gambit and mesh the whole one then compute with fluent, it will converge.

I am not sure whether you have talked about nonconformal grids for fluent 6, but this is probably what you need. You have to read section 5.4.1 through 5.4.4 to apply it properly on your problem. Good luck.

i use fluent5.5. now if i unite two parts into one and then mesh it with hybrid/tgrid method in Gambit.then open fluent to compute, there is no prblem. it will converge.

but if i mesh one part with hybrid/tgrid and define the interface by interface1,(and velocity inlet) export it with name a.msh then mesh another part with hybrid/tgrid and define the interface by interface1,(and outflow) , then export it with name b.msh. i merge these two parts into one in Tgrid and write by the name ,A+B.msh. open fluent and compute, it will not converge. the continuity line keeps horizontal.

i use fluent5.5. now if i unite two parts into one and then mesh it with hybrid/tgrid method in Gambit.then open fluent to compute, there is no prblem. it will converge.

but if i mesh one part with hybrid/tgrid and define the interface by interface1,(and velocity inlet) export it with name a.msh then mesh another part with hybrid/tgrid and define the interface by interface1,(and outflow) , then export it with name b.msh. i merge these two parts into one in Tgrid and write by the name ,A+B.msh. open fluent and compute, it will not converge. the continuity line keeps horizontal.

how to crack it ?

regards

You need to do one of two things to A+B.msh, if you have not already done so: either fuse interface1 and interface1 in case you want a conformal mesh or you need to define a non-conformal grid interface by going to Define-->Grid Interface in case you want a non-conformal mesh. See Fluent user's guide 5.4.2.

I would use names like interface1 and interface2 instead of interface1 and interface1. Remember to do one of the two things in the previous paragraph before doing any iterations. Also follow the requirements and limitations of non-conformal meshes in 5.4.2 very closely. I hope this helps. Good luck.