Hi, I am having trouble decomposing the geometry of a 3D pipe T-junction so that I can use the cooper tool to mesh the object in Gambit. The T-junction has a side arm which is smaller than the mainline. A run down of how to go about this decomposition will help me out a lot. Thanks in advance.

If you really want a good mesh in the junction region, I strongly advise you to use nonconformal interfaces and to mesh the side arm separately. After meshing optimally the two components export them to separate msh files and merge them simply by reading them into Tgrid. Then save the resulted grid and read it into Fluent and create the interface. Before creating the interface, use this comand:

/define/grid-interfaces>use-virtual-polygon-approach

This algoritm is better suited for curved surfaces (which is your case).

Best whishes, Razvan

Hi Razvan, That does seem the best way to go about it. However, I dont have access to TGrid. All I have at my disposal are Gambit and Fluent 6.2. Could you tell me how you would merge the two volumes in Gambit. I have tried but my methods dont seem to work.

Also, I would like to create a finer mesh at the junction of the two volumes. Do you have a good method for this?

Thankyou very much.

Ok. Then go to: Fluent.inc\utility\tmerge2.1\ntx86\tm3d2120.exe. This is the same executable Tgrid is using when you read multiple meshes.

1.Copy the meshes in the same directory as the .exe;

2.Double-click the program, and if the meshes have been created with the geometry already in the right place, then you do not need to scale,translate or rotate it. So simply type the names of the files with .msh extension and give a final name to the merged file (actually this is not quite that simple, but you will manage it).

Hope this helps you. Razvan.

Thank you Razvan. That has helped me a lot. There is just one more problem I am having though.

I have the two meshes: sidearm.msh & mainline.msh

I have been able to mesh the sidearm with cooper type ok.

For the mainline, I have the volume formed by faces which include the interface (which will be merged with the side arm interface). I cant mesh this volume with cooper scheme, even though it is really just a cylinder volume.

Would you know of a way of meshing this volume with cooper mesh, while having this interface meshed also? This is the last thing I have to do and then the problem is solved.

Thankyou very much for your help so far.

John, the solution is even easier than you think. You don't have to "cut" a correspondent face for the side arm onto the mainline's geometry! That's the idea about these interfaces!

You mesh the main line with Cooper scheme just like you don't even know you have a side-arm (I'm not kidding!)

Then, define the half of cylinder on side-arm's side as "INTERFACE", just as the coupling face of the side-arm.

When you will define in Fluent the interface between the two meshes, the program itself will transform the non-overlapping part of the half-cylinder into "WALL", so your problems are finished!

That should do it.

Best whishes, Razvan

Thankyou Razvan, you have been a great help.

When I define the grid interface in Fluent, it creates the wall (non-overlapping part) and the overlapping part remains as an interface.

When I solve the model, the fluid seems to slow rapidly at this interface. I need this interface to disapear since there should be no hinderence to fluid flow at the t-junction.

Is there something i havn't done correctly?

Do I need to change the interface boundary condition?

[ghost82]

Hi I know this is quite an old topic, but I had this problem too.
The interface seems to be the easiest and fastest way for the T junction problem; I had also discontinuity problem in the contour plot at the interface boundary, but from the user guide:

Note that you cannot create zone surfaces for the intersection boundaries (i.e., the interior/periodic/external zones created from the intersection of the interface zones). You may instead create zone surfaces for the interface zones. Data displayed on these surfaces will be "one-sided''. That is, nodes on the interface zones will "see'' only the cells on one side of the mesh interface, and slight discontinuities may appear when you plot contour lines across the interface. Note also that, for non-planar interface shapes in 3D, you may see small gaps in your plots of filled contours. These discontinuities and gaps are only graphical in nature. The solution does not have these discontinuities or gaps. To eliminate these discontinuities for postprocessing purposes only, you can use the define/mesh-interfaces/enforce-continuity-after-bc? text command, which will ensure that continuity will take precedence over the boundary condition.

[saharesobh]

Hi. I have one question. Actually I am working with Ansys Fluent 13. and I meshed my model via Ansys Fluent . But I am going to change the boundary condition. I cannot go back to mesh set up. because the mesh filed was sent to me by my advisor. but you know, when I go to set up part in Ansys Fluent, file, mesh, gambit,,,,
I mean in set up I have gambit. but I don't know how to open my case file or mesh file in gambit in Ansys Fluent 13. Would you please give me some advise. Just to mention I don't have gambit in my laptop. I have just Ansys FLuent 13.

[saharesobh]

Hi. I have one question. Actually I am working with Ansys Fluent 13. and I meshed my model via Ansys Fluent . But I am going to change the boundary condition. I cannot go back to mesh set up. because the mesh filed was sent to me by my advisor. but you know, when I go to set up part in Ansys Fluent, file, mesh, gambit,,,,
I mean in set up I have gambit. but I don't know how to open my case file or mesh file in gambit in Ansys Fluent 13. Would you please give me some advise. Just to mention I don't have gambit in my laptop. I have just Ansys FLuent 13.