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

fully developed channel with cyclic using simplefoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 6, 2014, 13:46
Default fully developed channel with cyclic using simplefoam
  #1
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 6
ArathoN is on a distinguished road
hi foamers,

I'm trying to simulate a channel with rectangular section so that i can take the outlet values of velocity and turbulent energy and feed it directly as input of my main simulation (the backward facing step case). My initial data are:
- U(developed flow) max =8.7
- I around 7 % (i calculated it from the experimental data of makiola for the backward facing step)
- Re= 15000 (then i'll do the same for the 64000 Re)
- y plus is less than 1 all over the domain for both the walls
- using the simplefoam solver with KEpsilon model


First i tried using a normal mesh but here i faced a little problem what value of the velocity should i consider, knowing the maximum velocity at the outlet. And i didn't find any publication where they studied the relation of the fully developed velocity flow and the inlet flow. I founded only a ppt of an Indian professor where he states that U(developed flow) = 1.5 U(inlet) but it isn't correct. Do any of you know any useful reports about this?

Second i used the cyclic condition, and because the mesh was done with gambit i've created the patch thanks to the createPatchDict library. The problem is that the epsilon variable doesn't converge. And i don't know what to do, please help me.

P.S. I found that i can use the data from a different case into another one by using one of these function:
- directmapped
- cyclic
- TimeVaryingMappedFixedValue
but i didn't understand exactly what they do (and i read a lot of threads here), from what i grasped the "cyclic" will link to patch creating a infinite loop so in the case of the channel it's like simulating an infinite channel; the "TimeVaryingMappedFixedValue" will do an interpolation in space and in time (what does this mean? if i give the value of a variable in 2 different times will it do an interpolation of the same variable over the two times given?.
I found close to nothing for the directmapped function, also the tutorial case where it was used now use the "TimeVaryingMappedFixedValue" condition.
If someone can link me some good and useful threads or directly explain it to me, i would be really really grateful.

PPS: i attached my "\0" and "\system" directories so please look at it and tell me what i'm doing wrong.
Attached Files
File Type: zip Cyclic.zip (13.3 KB, 10 views)
ArathoN is offline   Reply With Quote

Old   February 8, 2014, 10:46
Default
  #2
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 6
ArathoN is on a distinguished road
mmm I've almost give up on asking here but i hope someone would do it (this is my seven thread and until now no one even shed a light on any of my doubts).
ArathoN is offline   Reply With Quote

Old   February 21, 2014, 07:25
Default
  #3
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 6
ArathoN is on a distinguished road
At the end i understood all the 3 type of boundary condition, now i have a problem how can i compute the bulk velocity knowing the center-line velocity in the channel. I'm simulating a fully developed flow with the same conditions at in the first post.

Please help me... I searched everywhere but found nothing, the Reynolds number is based oh the channel height and it's the same for mu next case the backward facing step (ratio 1:1),

The only relation i founded is
Ubulk= Re(Ub) nu /Hchannel
But my Reynolds depends from the centerline and i can't figure out how i would i define the Re with repect to the bulk velocity, i read every paper i founded on the net but nothing..
ArathoN is offline   Reply With Quote

Old   February 21, 2014, 07:59
Default
  #4
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 12
Bernhard is on a distinguished road
You are asking a lot of questions here.

First, how did you plan to map the velocity of your channel case to the backward step case? The "mapped" patches might be your best approach, as it maps the velocity off a downstream slice to your inlet. However, I think it is mostly use for LES simulations, but I don't see a problem for using it in a RANS-simulation.

Second, there is probably not a simple relation between bulk and maximum velocity, but the factor 1.5 you found is for laminar flow, while for turbulent flow it will reduces with Reynolds number. Nothing stops you from doing a few simulations at different inlet velocity to see what happens.

Third, you are using the standard k-epsilon model on a y+<1-mesh. The standard k-epsilon model is only to be used in it's basic shape with wall-functions. If you have the refinement near the wall, you should add low-Re terms that act close to the wall. Maybe this is the reason your epsilon-equation is not converging?
Bernhard is offline   Reply With Quote

Old   February 21, 2014, 10:53
Default
  #5
Senior Member
 
ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 6
ArathoN is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
You are asking a lot of questions here.

First, how did you plan to map the velocity of your channel case to the backward step case? The "mapped" patches might be your best approach, as it maps the velocity off a downstream slice to your inlet. However, I think it is mostly use for LES simulations, but I don't see a problem for using it in a RANS-simulation.

Second, there is probably not a simple relation between bulk and maximum velocity, but the factor 1.5 you found is for laminar flow, while for turbulent flow it will reduces with Reynolds number. Nothing stops you from doing a few simulations at different inlet velocity to see what happens.

Third, you are using the standard k-epsilon model on a y+<1-mesh. The standard k-epsilon model is only to be used in it's basic shape with wall-functions. If you have the refinement near the wall, you should add low-Re terms that act close to the wall. Maybe this is the reason your epsilon-equation is not converging?
First, Thank you for the reply you are the first to ever answer any of my question .

For the mapping from the channel to the backward facing step i'm using the utility available as 3rd party "setDiscreteFields" (or simply the nonuniform vector list type in the boundaries). The data i feed then i took it by sampling at the desired plane and i took two different approach, in one i opted for the cutting plane (surface) and I've set interpolate as false so that i have the cell values not the node ones, and for the second I used sets sampling at midpoint after specifying the normal vector and the starting point.

I found out about the deficiency of the kEpsilon model with low-Re meshes, and i started using the kOmegaSST with nutUSpaldingWallFunction for the nut at walls as stated in many other threads giving better results, now the U-profile is turbulent and not anymore exactly parabolic (as in a laminar fully developed channel). I tried also the Launder-Sharma simulation with good results. In both cases i initialized the fields with the kEpsilon data for faster convergence.

For the fully developed flow, I mapped the inlet with the outlet like this:

- U-boundary condition

Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type                  mapped;
        value                 uniform (9.07 0 0);
        interpolationScheme   cell;
        setAverage            false;
        average               (9.07 0 0);  
    }

    outlet
    {
        type            zeroGradient;
    }

    upperWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    lowerWall
    {        type            fixedValue;
        value           uniform (0 0 0);
    }

    frontAndBack
    {
        type            empty;
    }
}
-blockMesh

Code:
inlet
    {
        type mappedPatch;
        offset          ( 0.4 0 0 );
        sampleRegion    region0;
        sampleMode      nearestCell;
        samplePatch     none;
        faces
        (
            (0 5 11 6)
            (5 4 10 11)
        );
    }
    outlet
    {
        type patch;
        faces
        (

            (1 2 8 7)
            (2 3 9 8)          
        );
I wanted that the velocity at the center-line would be 9.07m/s, but from what i understood OF considers it as the bulk velocity, so it will raise to maintain the same mass flux. I wanted to do something more elegant than trying different velocity to obtain the desired center-line velocity from which i based the Reynolds number of the backward facing step.

Now the problem is that if i put the data of the channel outlet to the main case (backward facing step) i have some weird results. First of all the cumulative error is too high in my opinion (at about 0.005), knowing that i'm simulating a steady problem and if i try to trace the streamlines in parafoam there is no the recirculating region (I uploaded the images from parafoam), I don't know if it is some bad setting in the "stream tracer" or not. Even the plot of the wall shear stress is weird near the step and after days i can't understand how to solve it.

The zip with tha data of the case plus the last results are linked in my dropbox folder:
https://www.dropbox.com/s/bnr2z52nij...MappedData.zip


I know that i'm asking too much but i hope you can help me, I'm really desperate right now.
Attached Images
File Type: jpg BFS90_kOmegaSST_withDevelopedFlow.jpg (15.2 KB, 38 views)
File Type: jpg Streamlines_BFS90_kOmegaSST_withDevelopedFlow.jpg (47.1 KB, 34 views)
File Type: png tau-x.png (6.7 KB, 34 views)

Last edited by ArathoN; February 21, 2014 at 11:02. Reason: typos
ArathoN 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
ribbed channel / simpleFoam / boundary conditions beeo OpenFOAM Pre-Processing 20 July 17, 2013 08:39
interFoam vs. simpleFoam channel flow comparison DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21
How to get fully developed turbulent flow in a channel TQIM STAR-CCM+ 2 November 25, 2012 23:37
fully developed turbulent channel flow pankaj saha Main CFD Forum 0 August 24, 2007 18:15
LES fully developed channel flow Gem FLUENT 4 May 12, 2005 05:30


All times are GMT -4. The time now is 21:25.