Learning Forum

[Donghyun Yim]

Hi,

 

When I initialize the solution on fluent solve, the following message appears.

 

Warning: zone of type interior found between different solids!

Material of cell zone 14 is sus, while material of cell zone 13 is polymide.

This will adversely affect the solution.

It is recommended that you fix this issue via the TUI command

 

/mesh/modify-zones/slit-interior-between-diff-solids

 

Unless I enter the above command it diverges, but when I enter that command it converges.

 

I got the final solution, but I am curious of why that warning appeared.

 

Thanks,

Donghyun

[Keyur Kanade]

'interior' is nothing but the interior cells. for any boundary usually we have 'wall' type. so it it is 'interior' then solver will treat as 'interior' rather than 'wall'. 

if this helps you, please mark this post as 'is solution' to help others on forum.

 

 

 

[Donghyun Yim]

So that warning message implies the absence of wall between different interiors (or solids), and that command splits them.

If so, do I need to modify mesh before solve in order to prevent that warning?

Thanks,

Donghyun

[Keyur Kanade]

no need to modify mesh. 

select face between two solids in meshing and give named selection. 

if you already have different named selection for this then please select this named selection in fluent and change its type to wall.

https://www.youtube.com/watch?v=-6Z2v8geroQ

 

[Donghyun Yim]

If the type of face between two faces is set to be wall, no thermal energy exchange or uds exchange occurs across the wall. (as I understood)

So its type needs to be 'interface', not 'wall', doesn't it?

 

Thank for your kind reply,

Donghyun

 

[Keyur Kanade]

you can set it as interface depending your configuration. 

[Ayushman Srivastava]

warning: zone of type interior found between different fluids!

Material of cell zone 8 is helium, while material of cell zone 9 is air.

This will adversely affect the solution.

[Rob]

Yes, that's a problem. 

[Ayushman Srivastava]

Please tell me how to resolve this problem.. i am facing the problem of floating point exception. Residual curves git diverged ... Please help me resolve this problem 

[Rob]

You have helium & air in connected fluid zones. That's not permitted without using some additional models. So, why have you got helium & air in connected fluid zones? 

[Ayushman Srivastava]

I have a shock tube. driver section of the shock tube is filled with helium at 0.9 MPa and the driven section is filled with air at atmospheric pressure. the diaphragm is there which separates the driver and driven section with each other. diaphragm ruptures and helium and air mixes with each other. shock wave then generates. How to remove that warning message and how to stop residual curves from diverging?

[Rob]

You'll need a species model, the tube is then a mixture of helium & air. To initialise the system you patch air & helium into the respective regions. Have a look at the species models tutorials in Help. 

[Ayushman Srivastava]

I patched the driver , driven sections in the cell zone condition. I was compelled to choose a mixture_template (helium+air) for the driver and driven section to avoid any warning or error. Simulation was running smoothly. Is it right way to run the simulation? As i wanted only helium in the driver section and air in the driven section, I dont know whether it is right to select the mixture_template.

But when i selected helium in the driver section and air in the driven section after turning ON the species transport model, a warning and error appeared. residuals were diverging.

 

[Rob]

Divergence is a different issue, and mostly likely linked to the mesh or solver settings. 

As you have two materials mixing you must use the species model. The cell zone contains the "mixture-template" and when you initialise you then need to patch species to suit. 

[Ayushman Srivastava]

my question is "After initializing, how to patch the driver with helium and the driven section with air after turning ON species transport model?"

[Rob]

After you initialise, you should see a button with "Patch" on it.