[FLUENT] How to calculate the drag in non-wall surface?
 

Hi everybody,

I am simulating the flow over and through a porous sphere, and would like calculate the drag on the porous surface (outer surface of the sphere).

However, Fluent allows to calculate the drag with wall-boundary condition only. Could you please recommend any way to calculate the drag on interior-surface? Or at least the way to determine the face area vectors of each elements on the porous surface só that I can use the momentum balance to get the drag?

I really need helps because I am quite new in FLUENT. Thank you all in advance.

Have you solved your problem? If yes, please help me in this regard. I'm facing the same problem while working on a 2D porous geometry.

Dear Jamshed,

I have found 2 ways to solve this problems. And unfortunately, they have different results of drag coefficient. You can check with your case.

1/ After completing the simulation, I change the boundary condition of porous surface (my case is in 3D) from interior to wall, so that I can force Fluent give me the drag coefficient. I am not sure this way is right but the positive thing is that we can have the face area vectors with wall boundary condition (so that we can approximate the momentum balance equation)

2/ I use the momentum balance over the porous object. Fluent provides information of velocity and pressure and we can get the face area vectors according to 1.

Hope that it can help you. Please let me know if it works for you. Thanks a lot :)

Hi bmaicuong
I am facing the same problem on calculating the force around a porous plate. Do you have more suggestions now?
Thank you very much for any of your reply.

Hi Zhang,

I used the momentum balance over the porous object to determine the force acting on it. You can see a more detailed strategy in my paper: https://doi.org/10.1016/j.oceaneng.2020.107140.

Check it and see if you can apply this for your case. Let me know if you need help.

I will read it carefully. You helped me a lot!

Hi bmaicuong
I have to say, I failed. I tried to model Patursson's case, which you can find in https://doi.org/10.1016/j.oceaneng.2009.10.001. But I got totally wrong drag coefficients. I am wondering how you managed to utilise the method mentioned in your paper? Through a User Defined Function or anything else?

Dear Zhang,

I did not get the idea. Why do you know your results are wrong? Did you compare them with experimental data?

In our method, we calculate the drag force based on momentum balance; we just exported the data of pressure, velocity and face area vectors to handle Eqn (11). No need to use UDF.

Best,
Cuong Bui

Hello Bui. So you mean you exported the result to some post processing software like CFD-Post? I think I can have a try. Thanks for your help.

Hi Zhang,

After finishing the simulations, you can export all data you need following this: File -> Export -> Solution data; Choose the File Type as ASCII then select the surfaces and quantities you need.

Let's give it a try and let me if it works. Good luck!

Best,
Cuong Bui

Hi Bui, I am sorry to bother you again but, could you please tell me how you get the area vector? The boundary of porous media is set "interior" by default. The exported "X Face Area" and "Y Face Area" data is all zero on the porous media boundary.

Hi Zhang,

Change it to 'wall' (after finishing simulations and collecting other data of velocity and pressure) so that you can get the information of the face area.

Hi Bui
I have to say, you really helped me a lot. I have got a satisfied result just now!
By the way, if anyone who could see this thread, I want to give you a tip that sometimes setting the correct porosity and clicking on "physical velocity" on the "cell zone conditions" task page will make your result different!
And, 2D simulation sometimes can not give you satisfied results.
Best
Chi Zhang