Changing from Wall to Interior
 

Hi all,

I currently have a wall in my simulation in Ansys 15.0 that I would like to change to interior. Upon searching online, it seems that the choice of options from this dropdown menu would enable me to make this change: https://www.sharcnet.ca/Software/Flu...g/node1354.htm
However, under the boundary conditions section of my Solution Setup, I have many more options (interface, pressure outlet, velocity inlet, etc) but no interior. How can i make this change?
Thank you very much to any help, I'm quite new to Fluent!

In order to use interior your surface must be inside the domain, for example if your current wall is the edge of the domain it will not let you select interior. Interior, fan, porous jump, etc that show up in your link arent exactly "boundary" conditions. The BC's you listed, outlets and inlets, lead me to believe your wall is a surface at the edge of your domain.

Thank you very much! How would I go about creating something that is inside of my domain, as everything I'm doing isn't working. To elaborate on what I'm trying to do: I am simulating the vortex rings emitted from a capsule in 2D. There is a cylinder with a cap, both of which are rectangles. The cap needs to begin as a wall. However, after some time steps, it must be changed to interior (as if it has disappeared) to allow the vortex rings to form. I know this has been done before, but it was done using GAMBIT which is not an option for me. Do you know how to make this change? Whenever I try creating a geometry of rectangles and created 2 bodies, it doesn't allow me to do this.

You will just need to have mesh inside the cap region then you will be able to change the cap surface to interior. Right now the cap surface is separating a fluid region (mesh) from nothing (no mesh). That means it can never be an interior surface because the solver wont know what to do when it passes through that surface, theres no mesh there! All you need to do is create mesh on the other side of the cap surface too then you will be able to change that wall into an interior.

In order to create an interior boundary in Fluent I advice the following steps. Identify an adequate parameter to mark the cell faces that you want to specify as interior boundary. After the cell faces are marked, go to separate faces from mesh. This will need to the creation of a new boundary. If the faces of the created boundary have fluid cells on both sides you should be able to specify the boundary as wall, and then change back to interior.

Thank you all so much for the replies! I can indeed now change from wall to interior. However, when I scale my geometry correctly, I get the following error: "The mesh file exporter does not support geometry appearing in both the source and target in contact regions". This does not happen if I simply scale up by a factor of 5. Does anyone have an idea as to why this would happen?

Could you share the method to do this?

Hi didiean

This is how I fixed this - if you go to meshing, there is a branch of the tree on the left labeled "Contact Regions". Expand this, and delete all the contact regions there. I guess that when I scaled by a factor of 5, the regions were far enough away from each other to not be considered a contact region. Everything worked for me after I did this, hope it helps!

Well, the model should be scaled before the interface definition.

We have two bodies and we want to conduct airflow through this two bodies (from inlet to outlet). Also, we want to consider their common or mutual face as either interior or wall boundary condition (for closing and opening the airflow). Thus, we have to obtain the common face as interior in Fluent. However, when we import the mesh file to the fluent the mentioned face is seen as wall and as a result it is not changeable to interior. I am wondering to know how I can solve this problem?

I am busy with this problem for a long time, I am appreciated if you could help
http://tinypic.com/r/eriiib/9
http://tinypic.com/r/egwb54/9
http://tinypic.com/r/eriiib/9

wall and shadow interchanging problem
 

Hi

I am solving a reacting flow problem with reaction happening on the wall of the infinite parallel plate system, I have created a non-symmetric conformal mesh for the system of infinite plates with 2 surface bodies (namely solid wall and bulk fluid). Now the problem is after meshing, when mesh is exported into FLUENT window, on the solid-fluid interface reaction wall boundary gets interchanged with the shadow. I mean, if the meshing and geometry creation are right, we should get reaction boundary condition on the fluid side and coupled wall boundary condition on the shadow which faces the solid wall. But this is not so in my case. It comes exactly in the converse way.

Can anyone suggest me a solution other than non-conformal meshing

Thanks in advance

You always get a wall and shadow wall pair. Which side is the wall and which side is the shadow can be difficult to control and depends on the mesher. But whether it is a wall or shadow wall is not important, and you can just as easily rename them however you like. Just make sure you know which belongs to which, i.e. does the wall belong to the fluid side or does it actually belong to the solid side. The mesh doesn't actually know which is fluid, which is solid.

Do you use the boolean of Mesh software to separate the zones?
 

Do you use the boolean of Mesh software to separate the zones?

Maybe some bodies are set as solid
 

I wonder it's what you are looking for, but just in case I leave a reply.

In my case, I had walls and their shadows those I didn't want because they should be interfaces between fluidic bodies.

That problem fixed by setting fluid as a type of body in the 'Design modeler' of Ansys workbench.

I cannot open your link, can you upload a image directly?
 

I cannot open your link, can you upload a image directly?