|
[Sponsors] |
Can't simulate heat transfer in an operating room |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 10, 2022, 11:28 |
Can't simulate heat transfer in an operating room
|
#1 |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
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
|
|
November 10, 2022, 14:48 |
|
#2 |
New Member
David
Join Date: Jul 2021
Posts: 14
Rep Power: 5 |
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. |
|
November 11, 2022, 04:06 |
|
#3 |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
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
|
|
November 11, 2022, 08:14 |
|
#4 |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
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?
|
|
November 16, 2022, 07:49 |
|
#5 |
New Member
Join Date: Sep 2021
Posts: 7
Rep Power: 5 |
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.
|
|
November 16, 2022, 09:29 |
|
#6 |
New Member
David
Join Date: Jul 2021
Posts: 14
Rep Power: 5 |
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". |
|
November 17, 2022, 04:20 |
|
#7 | |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
Quote:
|
||
November 17, 2022, 09:46 |
|
#8 |
New Member
David
Join Date: Jul 2021
Posts: 14
Rep Power: 5 |
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. |
|
November 18, 2022, 03:48 |
|
#9 | |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
Quote:
Last edited by AndreaVinci; November 18, 2022 at 08:11. |
||
November 18, 2022, 03:52 |
|
#10 |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
here's the geometry file, you'll find it inside the attached folder
Last edited by AndreaVinci; November 18, 2022 at 08:10. Reason: incorrect attachment |
|
November 18, 2022, 12:38 |
|
#11 |
New Member
David
Join Date: Jul 2021
Posts: 14
Rep Power: 5 |
I'll take a look when I get home. I may need to upgrade to latest SC release depending on what year you have.
|
|
November 21, 2022, 07:02 |
|
#12 |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
||
November 28, 2022, 15:25 |
|
#13 |
New Member
Yogesh
Join Date: Sep 2022
Posts: 12
Rep Power: 4 |
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? |
|
November 28, 2022, 19:24 |
|
#14 |
Senior Member
Alexander
Join Date: Apr 2013
Posts: 2,363
Rep Power: 34 |
the reason, author doesn't define interface between solid and fluid regions
__________________
best regards ****************************** press LIKE if this message was helpful |
|
November 29, 2022, 04:20 |
|
#15 | |
New Member
Andrea Vinci
Join Date: Nov 2022
Posts: 21
Rep Power: 3 |
Quote:
|
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Modelling the wall heat transfer | magicbretzel | CONVERGE | 5 | March 3, 2021 04:38 |
Simulate a coil in air (heat transfer) | suktan | Main CFD Forum | 0 | July 8, 2020 16:07 |
Question about heat transfer coefficient setting for CFX | Anna Tian | CFX | 1 | June 16, 2013 06:28 |
Convective / Conductive Heat Transfer in Hypersonic flows | enigma | Main CFD Forum | 2 | November 1, 2009 22:53 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 15:55 |