CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Porous Jump Boundary (

L. Hamid January 10, 2011 01:38

Porous Jump Boundary

I did a simulation of flow with porous wall. According to the user guide of fluent in the porous jump window, we need to the thickness of the medium. but in my model I did not know the thickness of the wall.

would you please help me.

bob12 January 11, 2011 05:52

the thickness of wall that you put into the boundary condiction is the same of the real problem. i think that it's a data of your problem.
i hope that it's helpfull
best regards

L. Hamid January 11, 2011 07:12

hi bob12

thanks for you attention

newcomer January 19, 2011 00:26

Porous jump BC

I am also figuring out porous jump model for FLUENT 2D and am a little bit confused of the assigning of boundary condition. As I understand from the guide, a porous jump BC is represented by a line in 2D application. I am wondering how should I set the BC when my porous medium is drawn as a block? In that case, should I assign the BC in 1 side or both 2 sides ?

Your help is really very much appreciated!

L. Hamid January 19, 2011 01:38

Porous Jump Boundary

suppose that you have a vertical porous block in 2D simulation that flow enters from left to right side, you should draw the left line of the block and set the BC for this line as a porous jump boundary condition. Then in the porous jump window you set the thickness of the block (distance between the left edge to right edge (the right edge has not been drawn) as a porous jump thickness.
If your simulation is in 3D, you should set the block as a volume and choose the porous zone in the fluid panel for the boundary condition.
i hope that it's helpfull

newcomer January 19, 2011 05:11

hi L.Hamid, thank you very much for the prompt advice!

Sabrinache December 5, 2011 21:50


I am also using porous jump condition for my 2D model. My system follows turbulence model. My media thickness varies with velocity and therefore my face permeability and C2 also varies. So, do I need to input these values all time for different velocity.

And also I am trying to find pressure drop using segregated model. So, in ANSYS 13, on Solution control option, do I need to active both "Flow and Turbulence" option?

Please help me about these.

L. Hamid December 10, 2011 09:27

Sorry for the delay. You mentioned that your media thickness varies with velocity. You mean that you have a structure with different thickness? If yes, you should divide you structure in different parts that in each parts the thickness is constant. Then you can insert the specific permeability and C2 to each part. It should be noted that the by this changes each two neighbor part has a face connected to each other. You should apply the 'interior' boundary condition to this faces.
Second question: ANSYS solves both (Flow and Turbulence) of these equations. If you select each of them ANSYS just shows to you the residuals of this equations. it is better to active both of these options. Therefore you can monitor the changes.

Sabrinache December 13, 2011 01:22

Hello Hamid,

Thank you very much for your reply. Actually I want to calculate pressure drop accross my structure. From the experimental data, I have calculated face permeability and C2 values. I know my inlet face velocity and pressure but I don't know my outlet information. Can you suggest me what kind of inlet and outlet BC I should use in ANSYS? Should I use "velocity-inlet" or "pressure-inlet" at inlet and "outflow" or "pressure far-field" or "outlet-vent" at outlet?

Thanks in advance.

L. Hamid December 13, 2011 03:21

Hi Sabrinache,

1- You can use 'velocity inlet' BC for inlet and 'outflow' or 'pressure outlet' BC for outlet. If you use 'velocity inlet' BC for inlet you should monitor the inlet pressure during the iteration. When your pressure at inlet reached to your desired pressure, your analysis is correct. Be careful, you should reach to your desired pressure at inlet with small tolerance.

2- But if you use 'pressure inlet' BC for inlet and 'outflow' or 'pressure outlet' BC for outlet, the conveyance process takes more time than the first selection I mentioned above. I should mention again, you should monitor the velocity at inlet and when you reach to your desired velocity (with small tolerance) your analysis in correct.

P.S. monitor is in the solve\monitor

good luck

Sabrinache January 18, 2012 13:23

Hi L.Hamid,

First of all, thanks a lot for reply and sorry for late response. Actually, I am trying the way you have suggested me. But I am still having some problem. Let me explain you my system 1st -

It is a rectangular structure which has a W-shaped reactor inside it. I am using 2D geometry for this. My inlet has 30 m/s face velocity and inlet pressure is 1 atm. I want to calculate pressure drop across the reactor. My reactor section is porous. From my experimental data, I have calculated C2 and face permeability. I have used porous jump BC for face of "W", interior for surface-interior zone, velocity-inlet for inlet, outflow for outlet and wall for wall-surface.

I have attached my geometry section for you. If you have any suggestion, please please please let me know.

P.S. my experimental pressure drop across reactor is 40 in water.

Thanks is advance. Eagerly waiting for your reply.


Sabrinache January 18, 2012 13:47

Sorry I could not attach my file.

L. Hamid January 22, 2012 12:10

Hi Sabrina

Sorry for late response. I couldn't see your model, but according to your explanation, the setting of the B.C is correct.

By this setting, you expect to reach the 40 in water pressure drop in your analysis. You should monitor the pressure drop across the W-shaped reactor. I mean, you should create an edge (because your modeling is 2D) on the right side and left side of the W-shaped reactor to monitor the pressure drop. The distance of these edges from the W-shaped reactor is about the thickness of the W-shaped reactor.

When your analysis converged or has stabilized, you should check the pressure drop.

Good luck

Sabrinache January 24, 2012 13:42

L. Hamid,

Thank you very very much for your co-operation. I am following your suggestion. But I am still having problem. I have found out that if I use "outflow" as "outlet" BC, I am not able to have 1 atm pressure at my "inlet". The value is far below than desired. Can you suggest me any other BC at outlet? I know something going wrong in my BC. I have no information at outlet. So, which BC will be appropriate for me and how will I get?

Thanks in advance.


L. Hamid January 25, 2012 04:30

Dear Sabrina

You should not worry about the value of the inlet pressure. In fact, at the end of the analysis you should reach to the correct pressure drop between inlet and outlet. If you set 'a' value for the inlet pressure, after the analysis the software calculates the 'a-dP' for the value of outlet pressure. You should set the 1 atm at operating pressure. I mean in FLUENT in the Define\Operating Conditions, in this window you should set 1 atm for operating pressure. By means of this procedure you can solve your problem.

Notice: If you set the outflow for outlet B.C, you should extend your outlet section. The length of extended outlet section is 5*(outlet hydraulic diameter).

P.S. if your problem didn't solved, you can use pressure outlet for "outlet"


Sabrinache January 27, 2012 01:00

Dear Hamid,

Thanks a lot for your reply. I found out where my problem was. I started my problem stepwise -

1. I prepared my geometry as a rectangular section with baffles (5 as a shape of W) inside. I showed me exact result which I wanted.

2. Then I prepared the same geometry with my media. Let me explain you how I did it -
  • Prepared a rectangular surface body as add material (active body).
  • Prepared all the baffles as rectangular surface body as frozen.
  • Prepared the porous media between the baffles as a W shape just like baffles.
  • Subtracted the baffles from active body.
  • Total 5 body - Surface body for active material (solid), and 4 surface body for porous media (frozen) as fluid.
During meshing, I just refined some edges and used "Create Name selection" for "Inlet", "Outlet" and "Wall"

After that I imported my data to FLUENT, now I am facing a problem. I was expecting FLUENT will find out all connection between porous media and fluid as an interior. But it creates fluid-porous media connection as a "Wall" and there is no interior option for this B.C.

How can it treat the connection as interior? BTW I have 2 cell zone - for surface body, I have used required fluid and for porous media, I have used "porous zone".

If you find out any thing wrong above the following steps, please please let me know. And I am really thankful to you for your assistance.


L. Hamid January 28, 2012 03:00

Dear Sabrina

If you expect FLUENT find out all the connections between porous media and fluid as in interior you should select these 4 surface bodies for porous media separately as a fluid region in Gambit in zone section and insert a different name to each 4 surfaces. by means of this process fluent could separate each zones with interior surface.

Good Luck

Akim679 March 15, 2012 15:48

Porous wall
hi guys,

I am trying to model a wall in a 3D channel as a "porous wall" is there a way to do that in GAMBIT and FLUENT?


Akim679 March 18, 2012 15:06

Porous Jump
I am actually having problems with specifying the boundary condition of a bottom wall of a 3D rectangular channel as a "porous jump" . In GAMBIT I select Boundary type as "Porous Jump" however, when I import my mesh in FLUENT I receive an error stating that: "Cannot change porous to porous-jump because
there is only one adjacent cell thread". I am not sure what that means, can anyone please help me with this case. Any suggestion is appreciated.


zaynah04 September 9, 2012 14:29

hi Hamid

I have same problem and i did as u advice Ie put each zone as porous_jump separately but unfortunately in Fluent it change it all to wall..:(

it sent the error message..:"Warning: Inappropriate zone type (jump) for one-sided face zone 3.
Changing to wall."

then" Error: Cannot change po to porous-jump because
there is only one adjacent cell thread."
Any help would be appreciated..


All times are GMT -4. The time now is 21:49.