|
[Sponsors] |
April 16, 2013, 08:38 |
Boundary conditions for Internal faces
|
#1 |
Member
Evangelos
Join Date: Sep 2011
Posts: 87
Rep Power: 15 |
Hello i want to set the boundary conditons for internal faces
i run simple how to set the internal faces for P ,U i just want the fluid flow through the face and no special boundary condition Last edited by Danath; April 16, 2013 at 09:04. |
|
May 3, 2013, 06:02 |
|
#2 |
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 314
Rep Power: 18 |
Dear Evangelos,
did you find an answer ? I have the same kind of problem. I want to set a boundary condition for a patch inside the flow domain. Let me know. Regards, Stephane. |
|
May 3, 2013, 12:51 |
|
#3 | |
Member
Evangelos
Join Date: Sep 2011
Posts: 87
Rep Power: 15 |
Quote:
but if you want to connect volumes and eliminate the internal faces try " merge faces " using Gambit |
||
May 4, 2013, 21:22 |
|
#4 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
Quote:
For example, there is a tutorial named "TJunctionFan", located in "incompressible/pimpleFoam/TJunctionFan", which creates a cyclic baffle. It then uses a special boundary condition of type "fan"... well, the specifics are in the file "system/createBafflesDict" and in "system/topoSetDict" you can see how the cell faces are selected for later converting to the cyclic baffles. @Evangelos: creating a faceSet or faceZoneSet might be enough, if you want to calculate the mass-flow going through the selected faces, or some kind of value monitor. These are selected using topoSet, as described in the aforementioned tutorial. Best regards, Bruno
__________________
|
||
January 13, 2014, 21:40 |
|
#5 |
Member
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 14 |
Hi ,
I have created a solid sheet patch inside a fluid domain in salome and imported to fluent. the internal patch has been defined in face zones. I want to define it as a wall and specify some field values for it. Can someone help me on this? |
|
January 26, 2014, 15:01 |
|
#6 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings Dinesh,
If you can provide a small example case, it would be easier to help you. Best regards, Bruno
__________________
|
|
January 26, 2014, 15:03 |
|
#7 |
Member
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 14 |
Hi Bruno,
Thanks for the help. I can work and see on it. |
|
January 26, 2014, 16:07 |
|
#8 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
By the way, doesn't this page explain what you are trying to do? http://openfoamwiki.net/index.php/Ho...internal_walls
|
|
January 26, 2014, 16:31 |
|
#9 |
Member
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 14 |
Hi Bruno,
I created a large box. Inside which i created a duct, as a solid domain. Then I used partition operation for two bodies. The boundaries are created in the face zone of the polymesh. I need to create a temperature boundary condition in the walls in the 0 directory. But I cant find the boundary condition for the walls. This is my problem. |
|
January 26, 2014, 16:51 |
|
#10 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Dinesh,
Mmm... OK, then if the instructions at http://openfoamwiki.net/index.php/Ho...internal_walls don't do what you need, then I need an example case so that I can test this myself. Best regards, Bruno
__________________
|
|
January 26, 2014, 17:05 |
|
#11 |
Member
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 14 |
Hi,
If you can send ur email id, I can send the case to you directly. |
|
January 29, 2014, 23:34 |
|
#12 |
New Member
Steven
Join Date: Jan 2014
Posts: 14
Rep Power: 12 |
Greetings everyone,
I have been running into a related issue with my simulation, although it may be an even simpler case. I've been following along the $FOAM_RUN/tutorials/incompressible/pimpleFoam/TJunctionFan tutorial to see if I can create a baffle in my domain. My general procedure so far has been to first define my topoSetDict to create a faceZone that will then be converted into an internal wall with createBaffles. The actions field inside my topoSetDict looks like: PHP Code:
Any help would be greatly appreciated! Regards, Steven |
|
January 31, 2014, 00:28 |
|
#13 |
New Member
Steven
Join Date: Jan 2014
Posts: 14
Rep Power: 12 |
Hello all,
I seem to have solved my problem. For those that are interested, I will explain what I did in order to create my infinitely thin wall. Please forgive me if my explanation isn't technically sound, it is merely how I understand it. What I needed was essentially a vertical partition in my wave flume to create a 180 degree bend, essentially what is shown in my primitive drawing below (imagine the dots aren't there): _________________________________________ |........ ___________________________________| |_________________| I needed it to behave as the external walls did with all the same initial and boundary conditions for k, epsilon, velocity, pressure, eddy viscosity, etc. In the first step I created a topoSetDict with the following entries inside: PHP Code:
I ran topoSet after my mesh was created and was able to view the newly created "set" and "zone" in paraview (not yet a patch). To convert it to a wall I ran createBaffles with the following createBafflesDict entries: PHP Code:
If anyone who understands this better I would love to know if my procedure is standard, or if there is an easier way etc! Hope it helps someone, Steven |
|
February 2, 2014, 10:30 |
|
#14 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
@Dinesh: Quote:
I ask this because otherwise your email will only get lost in the several other emails I get, which is why I like to keep OpenFOAM+forum related questions only on the forum itself, including private messages. @Steven: Thanks for sharing the solution you've reached. And sorry, but I don't have time to go over the solution you've found . Best regards, Bruno
__________________
|
||
April 11, 2019, 12:27 |
|
#15 | |
Member
Gareth
Join Date: Jun 2010
Posts: 56
Rep Power: 16 |
Good Day All
Sorry for reviving an old post but i think my question fits in here. I have created internal faces similar to the original post
The inlet and outlet patches are pressure based and i am using bouyantSimpleFoam as the solver since i have a heating element in my mesh. Below is my U file Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { #includeEtc "caseDicts/setConstraintTypes" "Box_walls|Box_pcb|Box_heater|Box_ppm" { type noSlip; } Box_inlet { type pressureInletOutletVelocity; value uniform (0 0 0); inletValue uniform (0 0 0); } Box_outlet { type pressureInletOutletVelocity; value uniform (0 0 0); inletValue uniform (0 0 0); } "baffel1_master|baffel1_slave" { type flowRateInletVelocity; massFlowRate constant 0.000925; rhoInlet 1; // estimate for initial rho } } Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 101325; boundaryField { #includeEtc "caseDicts/setConstraintTypes" "Box_walls|Box_pcb|Box_heater|Box_ppm" { type fixedFluxPressure; value uniform 101325; } Box_inlet { type fixedFluxPressure; value uniform 101325; } Box_outlet { type fixedFluxPressure; value uniform 101325; } "baffel1_master|baffel1_slave" { type fixedFluxPressure; value uniform 101325; } } Quote:
I have a zip of the case file but its too large to attach I have attached a screenshot of the mesh. the solid white patch would the baffels. The inlet and outlet are on the right side. These are clips of the stl used to make the mesh. Any advice welcome Last edited by bullmut; April 11, 2019 at 12:36. Reason: attaching case file |
||
April 21, 2019, 08:47 |
|
#16 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick answers:
__________________
|
|
June 26, 2019, 16:31 |
|
#17 |
New Member
Paras
Join Date: Jun 2019
Posts: 3
Rep Power: 7 |
@alientxtmsgs
I did exactly what you did and it worked. Now if I want to create inner walls which are not vertical or horizontal but inclined (60 degree) what should I choose? I cannot use box to face so what else can I use? |
|
June 26, 2019, 16:37 |
|
#18 | |
New Member
Paras
Join Date: Jun 2019
Posts: 3
Rep Power: 7 |
Quote:
|
||
June 20, 2023, 14:41 |
|
#19 |
New Member
water
Join Date: Mar 2022
Posts: 2
Rep Power: 0 |
hi everyone, i am having the same problem, but its a boundary that is an artefact of using fluentMeshToFoam so i'm stuck with it.
the yellow wall is the wall i dont need for my simulation. i've set that boundary to internal and defined the initial conditions as type internal. this works just fine when i check my conditions (by typing paraFoam before running the sim) but upon running the sim, i get an error saying it cannot form a matrix for this wall. for the simpleFoam solver, i can use an internal condition as well (simpleFoam -listScalarBCs -listVectorBCs) any ideas on how to fix it? i have tried this and it doesnt work, openfoam does not expect wall_A and expects a ) or } https://openfoamwiki.net/index.php/H...internal_walls thanks! |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] Add Mesh Layers doesnt work on the whole surface | Kryo | OpenFOAM Meshing & Mesh Conversion | 13 | February 17, 2022 08:34 |
mesh file for flow over a circular cylinder | Ardalan | Main CFD Forum | 7 | December 15, 2020 14:06 |
ribbed channel / simpleFoam / boundary conditions | beeo | OpenFOAM Pre-Processing | 20 | July 17, 2013 09:39 |
Please help with flow around car modelling! | Tudor Miron | CFX | 17 | March 19, 2004 20:23 |