CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

mass flow between two regions (faceZone)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 31, 2016, 11:37
Default mass flow between two regions (faceZone)
  #1
New Member
 
Cartuns11's Avatar
 
Join Date: May 2015
Location: Barcelona
Posts: 23
Rep Power: 3
Cartuns11 is on a distinguished road
Hello everybody,

I'm working on a complex model but firstly I've carried out a simple model due to the problems found in the big model.

Currently, I use two "very very simple" models. The first model consists of two cubes with the same fluid but each cube is a different region (cubes2.png). And the second is the same geometry but with one prism (prism.png), which will be used to compare the results obtained with 1 or 2 regions.(prismT.png)

The target is to get the same results on both models.

I want the interface between regions to have a mass flow exchange (exch.png). The boundary is "mappedWall" (left_to_right and Right) type and I don't know how to define de BC.....U, p_rgh and T.

I'm using 2.4.0 and the chtMultiregionSimpleFoam solver. The massFlow model is in this post.

I have some ideas, for example mappedFlowRate or mapped......and also the cyclicAMI but this doesn't work with multiregion....
Using the mapped philosophy, I've obtained info in the "/combustion/fireFoam/les/oppositeBurningPlanels" tutorial. However it doesn't work in my model.

could you help me?

Thanks
Attached Images
File Type: jpg prism.jpg (154.5 KB, 12 views)
File Type: jpg cubes2.jpg (23.7 KB, 15 views)
File Type: png prismT.png (25.6 KB, 16 views)
File Type: png exch.png (6.4 KB, 14 views)
Attached Files
File Type: zip massFlow.zip (27.5 KB, 4 views)
Cartuns11 is offline   Reply With Quote

Old   November 7, 2016, 10:02
Default Coupling of two regions
  #2
New Member
 
Max
Join Date: Sep 2016
Location: Delft, Brussels
Posts: 5
Rep Power: 2
WildeCat is on a distinguished road
Hi Cartuns,

I am working on quite a similar problem as you did one and a half year ago. I need to couple the mass transfer between two fluid regions with a boundary condition. I have been looking into mappedFlowRate and other mapped boundary conditions. However without too much success so far. Currently my thought is to rewrite the thermal boundary condition turbulentTemperatureCoupledBaffleMixed to achieve my my goal.
I would like to know whether you managed to solve the problem and could assist me.

For the coupling of the temperature, you can simply use the turbulentTemperatureCoupledBaffleMixed boundary condition in the following form

Code:
    <patchName>     
{
         type            compressible::turbulentTemperatureCoupledBaffleMixed;
         Tnbr            T; // neighbouring field
         kappa           lookup; // fluidThermo, solidThermo
         kappaName       kappa;
         thicknessLayers (0.1 0.2 0.3 0.4); // optional
         kappaLayers     (1 2 3 4); // optional
         value           uniform 300; // placeholder     
}
more information on:
http://cpp.openfoam.org/v4/a02795.html

I know I am very late, but maybe it helps someone else in the future.

Thanks in advance
Max
WildeCat is offline   Reply With Quote

Old   November 10, 2016, 05:04
Default One way coupling of all variables in multi region
  #3
New Member
 
Max
Join Date: Sep 2016
Location: Delft, Brussels
Posts: 5
Rep Power: 2
WildeCat is on a distinguished road
Hello everyone,

I would like to give an update for all people who are attempting to couple to fluid regions.

Two way temperature coupling can be achieved with the thermal boundary conditions. Many different exist. More information can be found on:

http://openfoam.org/release/2-3-0/thermal/

Apart from temperature, in some cases it is necessary to couple also other variables such as rho, U or p. In these cases, as far as I know, no two way coupling exists. If however you know that you only need to transfer information from one region to the other, so not coupling it, you can use mappedField. This boundary condition allows to map the conditions at one patch to another patch on different regions. The source guide may help you to understand this boundary condition better.

http://cpp.openfoam.org/v4/a01446.html

Since the source guide is for OF4.x, but I use OF2.3.x, where it is implemented somewhat differently, I will add here how to implement this boundary condition. Make sure the interface between the regions is a mappedWall.

Code:
    <interfacePatchName>
    {
        type                  mappedField;
        sampleMode      nearestPatchFace;
        sampleRegion    <neighbourRegion>;
        samplePatch      <interfacePatchNameOnOtherRegion>;
        fieldName          <vairable>; // scalar or vector
        setAverage        no;
        average             (0 0 0); // 0 for scalar
        value                 uniform (0 0 0); // placeholder, 0 for scalar
    }
I am currently working on writing two way coupling between different regions for U. Depending on my case I may be able to solve it differently, but should i find a suitable solution, I'll try to post it here.

Hope I could help
WildeCat is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 8 October 25, 2016 19:48
Total pressure and mass flow boundary condition at inlet bscphil OpenFOAM Pre-Processing 2 April 19, 2015 07:56
mass flow inlet and pressure outlet with target mass flow rate Zigainer FLUENT 10 January 5, 2013 22:51
Convergence problem with target mass flow rate ADL FLUENT 2 May 29, 2012 21:11
mass flow Wenbin Song FLUENT 0 September 27, 2005 13:00


All times are GMT -4. The time now is 02:48.