# fully developed channel with cyclic using simplefoam

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
February 6, 2014, 13:46
fully developed channel with cyclic using simplefoam
#1
Senior Member

ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
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
 Cyclic.zip (13.3 KB, 12 views)

 February 8, 2014, 10:46 #2 Senior Member   ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 7 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).

 February 21, 2014, 07:25 #3 Senior Member   ArathoN Join Date: Jul 2011 Posts: 137 Rep Power: 7 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..

 February 21, 2014, 07:59 #4 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 12 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?

February 21, 2014, 10:53
#5
Senior Member

ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 7
Quote:
 Originally Posted by Bernhard 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
 BFS90_kOmegaSST_withDevelopedFlow.jpg (15.2 KB, 42 views) Streamlines_BFS90_kOmegaSST_withDevelopedFlow.jpg (47.1 KB, 36 views) tau-x.png (6.7 KB, 37 views)

Last edited by ArathoN; February 21, 2014 at 11:02. Reason: typos

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post beeo OpenFOAM Pre-Processing 20 July 17, 2013 08:39 DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21 TQIM STAR-CCM+ 2 November 25, 2012 23:37 pankaj saha Main CFD Forum 0 August 24, 2007 18:15 Gem FLUENT 4 May 12, 2005 05:30

All times are GMT -4. The time now is 17:29.

 Contact Us - CFD Online - Top