|
Porous Jump Boundary
Hi 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. |
hi,
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 |
hi bob12
thanks for you attention |
Porous jump BC
Hi,
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! |
Porous Jump Boundary
Hi
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 |
hi L.Hamid, thank you very much for the prompt advice!
|
Hi,
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. |
Hi 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. |
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. |
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 |
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. Sabrina |
Sorry I could not attach my file.
|
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 Hamid |
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. Sabrina |
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" Regards Hamid |
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 -
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. Sabrina |
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 Hamid |
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? Thnaks, Akim |
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. Thanks, Akim |
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.. zaynah. |
Dear zaynah Let me to explain two different boundary conditions: 1) Porous media 2) Porous jump If you want to use porous media boundary condition it means that you have a volume have been filled with porous material. For this modeling you should know these items: a viscous loss term and an inertial loss term. It means that in your modeling you have different volumes but one of these volumes is porous media. In gambit you should separate this volume from the other volumes. I mean that you should insert the different name for this specific volume. Notice, if this specific volume has some walls that they are joining to the other volume you should set them as an "interior" in the boundary condition. Then you export the model in fluent and set the values for a viscous loss term and an inertial loss term in define\boundary condition\your specific name for your specific volume with TYPE: Fluid. You should check the porous zone in this part. If you want to use the porous jump boundary condition, it means that you didn't want to model the porous volume. I mean it is not necessary for your project to know the pressure drop through this volume. In this case you know the thickness of the porous media and pressure jump and permeability of the face. Therefore in gambit, you set the "Interior" boundary condition for this face and in fluent you select the porous jump in define\boundary condition part. It should be noted that your face have to be located in the middle of model. I mean the outer boundary couldn't set as a porous jump boundary condition (Please see the Akim679 comment) By means of this process you wouldn't have any problem. Please inform me if you try this process or not. Good luck Hamid |
Dear Hamid thank you for such prompt reply.
I want to use a porous square in 2D to observe how the air enter the porous square and how it goes out.I mean i want to observe how my velocity changes after passing through the porous square. but i Do not know how to proceed.. as each time i put Porous_jump In gambit when export to fluent it refuse to acknowledge it..:( Thanks zaynah |
According to your explanation (I mean I want to observe how my velocity changes after passing through the porous square.), you couldn't achieve to the result (velocity behavior through porous square) by means of using porous jump boundary condition. You can extend your 2D model into 3D. Set the third dimension value to 1 m. then you have a volume (porous media). In fact you have a cube with 2D dimension values and the third dimension is 1 m.
Now, I have a question from you: does your inlet flow has distance from one side of the square? if not you should extrude left and right side of your cube for producing the inlet and outlet sections. I mean you couldn't set inlet and outlet boundary condition for the right and left side of the preliminary cube. You should extend the desired sides for setting the inlet and outlet boundary condition. (If you don't know the length of the extension, this value for inlet is 5 * hydraulic diameter of the inlet surface. I mean the distance between inlet surface and inlet side of the cube. The distance between outlet boundary and the outside of the cube is 10 or 8 * hydraulic diameter of the outlet surface.) Now, by means of this procedure you have 3 volumes. (Left, middle and right) As I said before, you should set the surfaces joining to the left and right volumes to "INTERIOR". In gambit, in zone section\Specifying continuum type, you should have one volume for porous and 2 other volume for your fluid. Try it please Good luck Hamid |
dear Hamid
Sorry for late reply i was in fact trying it. but in my Gambit in the specify continuum i have only fluid or solid That is why i was asking about the job of porous_jump in gambit. :( zaynah |
Hi Zaynah Yes, in the specify continuum in gambit we have just fluid or solid. You should set your specific volume (porous media) as a fluid and then go to fluent. (Please insert the specific name for your porous media such as "POROUS SECTION") Read your case and check model's mesh. Now after your desired setting for model and material in "define" option. Then in the Define\boundary condition, you see the window divided into two parts, "Zone and Type". Now you should find your specific volume in the Zone part (remember I set your porous volume as "POROUS SECTION"). Notice your volume property is "fluid" in Type part. Now click on "Set…"and put a check mark on "porous zone". Good luck |
Hi All,
How can I define a membrane be permeable to air only? I have defined the membrane as a Porous Jump. And I have a mixture of air and water and I want this membrane to be permeable to air only. But I'm not sure how to set this. Could anyone help me? Thanks, Leram |
Hi all,
Could you please tell me how can I calculate "face permeability" for porous jump BC when My model is a porous pipe submerged in water. I made the model in 2D, so pipe is just a line of 6 m. Any help will be really appreciated . |
openfoam
hi hamid:
dear hamid your experience and guidance are so useful ... i want to know that did you use porous media in openfoam ?because i should solve my problem in this solver with porousInterFoam and when i export my case to openfoam, this solver can not find the porous media.. would you mind please help me to make my boundary condition in right way? :confused: |
Quote:
Dear Hesam, I'm awfully sorry. I have not any experience about openfaom. sorry again :( regards Hamid |
Vart
Hi all
I have a proplem. In the VARTM process simulation in fluent. I use porous boundary condition. I prepared the same geometry with my media. - Prepared a rectangular surface body as add material (active body). - Prepared all the baffles as rectangular surface body as frozen. - Total-2 surface: 1-flow media, 2-fiber inlet is "pressure inlet", outlet is "pressure outlet". but results are not as analytical and experimental. (time filling). If someone were simulated and the results properly, please help me thank! dinhgiap |
Hello, Hamid
I want to simulate flow through a rectangular porous section with inlet on leftside and outlet on right side with other two as walls in FLUENT. I have tried it by taking 'porous zone' in 'fluid' dialog box and given 'porosity' and left other things default. in the BCs for the interior surface i have chosen 'interior'. I have successfully completed simulation. Is it solving 'continuity and momentum equations in porous media'? One more doubt is I found in user manual "porous jump" gives fast covergence for 2D models. How can I use porous jump. it is actually for an edge (in 2D), but I am having a surface here. how can I give this boundary condition? Thank you |
Quote:
Hi SS17 about your first question: Yes, it solves continuity and momentum equations in porous media. the second question: if you model your porous media as a volume and you want to see the viscus resistance and inertia resistance in the porous volume you should select the media as the porous zone and set required data. but if your goal is not studying detail behavior of fluid in the volume you can use porous jump BC. if you want to model your geometry in 2D, you should draw a rectangle. split the rectangle via a edge in two parts. Now select the edge as a pressure jump BC. you should insert the permiability, thickness and pressure jump coefficient for this edge. Good Luck |
[QUOTE=Leram;412342]Hi All,
How can I define a membrane be permeable to air only? I have defined the membrane as a Porous Jump. And I have a mixture of air and water and I want this membrane to be permeable to air only. But I'm not sure how to set this. Could anyone help me? Thanks, Leram[/QU Hi. my problem is like to your problem. so for your simulation and speak about work: asareh.p@gmail.com. thanks |
Hello Hamid
I want to simulate flow through a cylindrical porous section with inlet on top and outlet on the bottom side of the cylinder. air with benzene entered from the inlet and benzene will adsorb to porous section. how can i define this problem in fluent? I was wondering if you could help me define this problem? Much appriciated! Thanks, Amin |
Good evening Sabrina. I am also using porous jump but when should I calculate C2?
|
| All times are GMT -4. The time now is 19:38. |