[AndreaVinci]

Hello everybody. I'm trying to run a cfd simulation of an operating room with ansys fluent. My problem is that I can't effectively simulate the temperature field of the room. I'm pretty sure that I'm making some mistakes during the geometry editing process. My model is made by the walls of the room inside which there are some solids (cylinders) that represent the doctors and the lamps. Each of these solid elements has some thermal properties that I put in the fluent setup (temperature, heat transfer coefficient etc). So there is air entering the room via the inlet area (on the top) and it leaves the room via the outlet areas. What I'm interested in is determining the air fluxes, the pressure field and the temperature field. I'm having problems only with the temperature field. What am I missing? Is there any tutorial online (that uses a similar model) that I can follow to understand how to fix this? P.S. I'll leave an image of the geometry attached to this thread. Thanks in advance

[rudyy]

Can you describe what the temperature profile looks like or why you believe it is inaccurate? (Or post some pics of temperature contours).

Did you "share" the geometry interfaces in Design Modeler and confirm the proper thermal BCs? (Ex: probably coupled BC for the objects in the environment, depending on how you are modeling the humans).

Would like to help but need more info.

[AndreaVinci]

Hi thanks for your response. The temperature profile is inaccurate because I just get constant temperatures on each of the bodies of the model, there's no heat exchange basically. Only thing I did in design modeler is combining all the parts in one single part, I created the geometry in spaceclaim

[AndreaVinci]

Ok I think I'm getting closer to the right solution. In fluent I have a shadow wall for each wall of my model. As far as I know shadow walls are necessary for simulating heat transfer between solid and fluid. Now my question is: how do I have to model these shadow walls? Do I have to put heat transfer coefficients, temperatures ecc just like I do with the regular walls?

[North Star]

You are in the right way. You need to model CHT to get temperatures inside your solids. For that, you don't need to do anything specific with your walls if you see them as coupled walls. Fluent will create a wall and a shadow if it sees an interface between a fluid and a solid. One of these walls is on the fluid side and the other is on the solid side, but physically it is a single wall. What you need to make sure of is that you have matching cells on both sides (you can do this by using the share topology option in design modeler, and visually inspect the cells to see if they match.) After this you need to use the correct turbulence model and the correct mesh (y+) to model CHT correctly. I might be missing something here but this should be the general idea.

[rudyy]

Like NorthStar said, you need to "share geometry". Honestly I still have trouble calculating y+, I'd love to learn more about this.


To share geometry in SpaceClaim, go to:

Top Ribbon -> Workbench -> Share -> Share all (green checkmark)

Make sure you do this after your geometry is complete (fluids extracted, etc). Any geometry you add after this step will not have shared boundaries.

Then, in Fluent, the boundaries should be set to "Coupled" by default. If you want to set a temperature BC on one side, set it to the shadow as well. (Recommended you create named groups in SC for any relevant BCs). For other BCs this may not be true. If you are making your humans as a volumetric heat source, for example, I believe you leave the BC as "Coupled".

[AndreaVinci]

Originally Posted by rudyy

Like NorthStar said, you need to "share geometry". Honestly I still have trouble calculating y+, I'd love to learn more about this.


To share geometry in SpaceClaim, go to:

Top Ribbon -> Workbench -> Share -> Share all (green checkmark)

Make sure you do this after your geometry is complete (fluids extracted, etc). Any geometry you add after this step will not have shared boundaries.

Then, in Fluent, the boundaries should be set to "Coupled" by default. If you want to set a temperature BC on one side, set it to the shadow as well. (Recommended you create named groups in SC for any relevant BCs). For other BCs this may not be true. If you are making your humans as a volumetric heat source, for example, I believe you leave the BC as "Coupled".

Hi thanks for your time. Your message makes a lot of sense but I dont know exactly what you mean with ''fluids extracted''. How do I do that?

[rudyy]

For an internal flow: after you model your solids (ex: pipe with inlet and outlet, internal geometry, etc) go to "Prepare" -> "Volume Extract". This way you can "fill" your model with fluid prior to meshing.

For external flow: you can model a fluid enclosure instead using the "enclosure" button.

Do this step before sharing geometry.

Feel free to share any files if you want me to take a look.

[AndreaVinci]

Originally Posted by rudyy

For an internal flow: after you model your solids (ex: pipe with inlet and outlet, internal geometry, etc) go to "Prepare" -> "Volume Extract". This way you can "fill" your model with fluid prior to meshing.

For external flow: you can model a fluid enclosure instead using the "enclosure" button.

Do this step before sharing geometry.

Feel free to share any files if you want me to take a look.

Ok I'll share the geometry file. The air input is that rectangle on the top and the outputs are the rectangles on the sides of the room. You'll also find the internal solids of the geometry (which are the bodies that have to cause heat exchange) and the named selections

[AndreaVinci]

here's the geometry file, you'll find it inside the attached folder

[rudyy]

I'll take a look when I get home. I may need to upgrade to latest SC release depending on what year you have.

[AndreaVinci]

Originally Posted by rudyy

I'll take a look when I get home. I may need to upgrade to latest SC release depending on what year you have.

Yes you need to upgrade if you dont have the latest version. I got the 2022 version

[yogesh03y]

There could be two reasons for getting constant temperature in your solution:


1. You did not enable Energy equation.


2. You are solving a steady-state simulation with boundary conditions that will eventually lead to a constant temperature in the domain.



What are your boundary conditions?

[AlexanderZ]

the reason, author doesn't define interface between solid and fluid regions

[AndreaVinci]

Originally Posted by yogesh03y

There could be two reasons for getting constant temperature in your solution:


1. You did not enable Energy equation.


2. You are solving a steady-state simulation with boundary conditions that will eventually lead to a constant temperature in the domain.



What are your boundary conditions?

Hi, I was able to find a solution. Thanks