Learning Forum

[AnthonyB08]

Hi all, 

I am trying to impose multiple boundary conditions on a single face, similar to the photo that is attatched to this post, but Ansys meshing software keeps returning the " mesh file exporter does not support overlapping geometry in named selections" error when I export my mesh. My question to the community is how do I impose multiple boundary conditions on a singular face WITHOUT going through (fluent with meshing) workshop. 

 

[Federico Alzamora Previtali]

Hello Anthony, 

I'm not sure what do yo mean by imposing multiple BCs on a single face but this error message occurs because a face or domain cannot be used for more than one "Named Selection" within a Fluent mesh, as Fluent is using the "Named Selections" to define the cell zones and boundary faces, respectively.
I would suggest giving the face a single Named Selection and assigning the BC that you want in Fluent.

[AnthonyB08]

Hi Frederico, 

See the image of my simulation, as you may see there are two unique boundary conditions on a single face. 

[Federico Alzamora Previtali]

I understand that, but numerically, what BC are you looking to set here? You can set multiphase BC on a single face in Fluent.

[AnthonyB08]

The top

Gas outlet- Mass flow outlet 

Liquid inlet- mass flow inlet 

Then at the bottom 

Liquid pressure outlet

Gas mass flow inlet

[Federico Alzamora Previtali]

Are your fluids coming in and out separately? If so, you would need to split their corresponding faces/cell zones. You cannot set overlapping BCs. 

[AnthonyB08]

How do you suppose these authors implemented the bottom boundary condition? In this snap shot, I see a gas inlet with a pressure outlet If Im not mistaken.. 

[Rob]

I think the key word there is "back flow". 

The top image shows distinct and separate surfaces for the gas outlet & liquid inlet, so that's fine. 

[AnthonyB08]

Backflow ensures the gas phase does not leave through that specific outlet, correct? I am still not understanding how to specify a mass condition for the gas phase without a boundary condition. I can set a back flow of 1 for the gas phase, but how do I describe the 38.5 kmol/m2/h ? 

[Rob]

Nope. Backflow defines what comes into a model if the flow conditions want to suck in rather than blow out of the meshed bit. I'm not sure why they're reporting flow in kmol/m2/h - that's a daft unit even for Americans! 

In Fluent we can set pressure and flow (mass/velocity) boundaries. Looking at the top image, what values do you know, so what options are there for each flow stream/boundary? Also consider whether a boundary is single or multiple phases when looking at it. 

[AnthonyB08]

 

The top should be a single-phase gas mass flow outlet, well say 2kg/s ( I can work on those units later), and a pressure outlet for the liquid phase, only, at the bottom. The liquid inlet is self-explanatory with well say 1kg/s. I am thinking I enable back flow for the gas phase at the liquid pressure outlet and a mass flow outlet at the top for the gas phase, but I see Ansys doesn’t offer a mass flow outlet for the two phase. How would I accomplish this task? 

 

[Rob]

It's available for mixture model, so you could suck gas out the top. Which model are you using? 

[AnthonyB08]

 

I’d like to use an Eulerian-Eulerian model to solve for the phases independently. I was thinking, maybe I could do a gas inlet but reverse the flow, doesn't like it will work but it was a thought. 

 

[AnthonyB08]

I am trying to mimic that snap shot of their simulation, in which they used an Eulerian-Eulerian model. 

[Rob]

Try a negative velocity. The mass outlet was removed a while ago; source terms can be made to work. 

[AnthonyB08]

If I do a negative velocity, should the back flow volume fraction at the bottom be equal to 1 for the gas phase ? 

[Rob]

Yes, but do some testing. The boundary behaviour has changed over the last several versions and I can't remember.