[Roland R]

Hello All,

I need to simulate an oil filter. I calculate it with porous domain but there is a thing which is not ok for me;

I define 3 parameters;
1. volume porosity
2. press. loss.coeff.
3. Permeability

If I decrease the volume porosity then the velocity increases in the porous domain. It is OK. But the pressure drop doesn't change. I think, if the velocity increases then the pressure drop should increase too. But the pressure frop total same both of case of volume porosity values.

What is the problem??

Thanks
Roland

[evcelica]

Are you using superficial or true velocity porous medium? If superficial then you won't see a difference in pressure drop since it uses the superficial velocity. Use true velocity if you want the volume porosity to make a difference.
Also, look in the documentation, it describes all this much better than I.

[Roland R]

OK, thanks a lot!

[Thomas MADELEINE]

If I am right, with superficial porosity the parameter you use are uncoupled...
so the pressure drop only depend on the pressure loss coefficient
the velocity depends on the void factor normally

be also careful of your mesh since the characteristics are really mesh dependant you have to use the exact same mesh to compare two configurations.

[Roland R]

Originally Posted by Thomas MADELEINE

If I am right, with superficial porosity the parameter you use are uncoupled...
so the pressure drop only depend on the pressure loss coefficient
the velocity depends on the void factor normally

be also careful of your mesh since the characteristics are really mesh dependant you have to use the exact same mesh to compare two configurations.

Hello Thomas,

thank for your answer. The mesh is same exactly. I use only one geometry with one mesh. My problem is solved with true velocity but the tuning of the parameters is not too simple. I have a pressure drop measurement in the function of volume rate. I need to have a velocity - pressure drop curve, which seems to be simple: V dot = v*A. But the determination of 'A' is quite complacated because of the complex geometry. If the value A is not correct (consequently the velocity value too) as a result the pressure drop will be too high in porous domain....

[katty17]

Hi All,

To study the effect of volume porosity, I created a simple tube with the following boundary conditions and simulation settings:

Domain type: Porous (full porous model)
Inlet: Opening with specified velocity profile.
Outlet: Opening with constant pressure.

Loss model: Isotropic loss, velocity type=True velocity, Permeability= 1E-4,1E-8,1E-14(m^2), Resistance loss coeff. = 0(m^-1).

Volume porosity: 0.1,0.5,0.9.

Why changing the volume porosity do not affect the velocity profile in the solution?

[ghorrocks]

You would have to give more details for us to answer that question. Attach some images of your model, what velocity profile you are talking about and your output file.

[katty17]

Hi Glenn,


Thanks for the reply.


The link below is a brief description of my simulation setup:
http://s000.tinyupload.com/?file_id=...24418317362600


And this is the link to the simulation output:
http://s000.tinyupload.com/?file_id=...69977472392453


Please let me know if I should provide any further information.

[ghorrocks]

In future please attach the files directly to the post, and put images in your post. This FAQ may help: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

But the answer to your question is obvious - with just an inlet and an outlet the velocity has to go from the inlet to the outlet (it can't go anywhere else!), and all you do when you change the porosity settings is change the pressure loss along the duct. The velocity profile stays the same.

[katty17]

Thanks for your help.

I didn't know we can upload images to the forum directly.

Regarding my problem; Oh, you are right. The inlet is a part of the porous medium too. So what I am doing is actually setting the velocity inside the porous media and there will be no reduction in the cross sectional area of the flow passage.

Thanks!