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

LES of a confined impinging jet reactor..

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2009, 11:00
Default LES of a confined impinging jet reactor..
  #1
Member
 
vishwanath somashekar
Join Date: Apr 2009
Posts: 41
Rep Power: 8
vishwa is on a distinguished road
Hi Guys,
I am very very new to Openfoam. I have been using fluent to perform LES simulation for a some time now.

I have been trying to understand the tutorial files and it has not been that easy.

Here is what I did to get the case running.
  1. used fleunt3dtofoam and it worked well on the .cas file so long as i had not adapted the grid using fluent. is there a way to get it to work when the grid has been adapted?
  2. in fluent i used dynamic smagorinsky model. I couldn't find a template from the tutorials where this particular one has been used. so, i tried with oneEqeddy model in the pitzDaily folder. Even here I have a few problems
    1. how do you figure out what files are needed in the initial condition folder based on the model you choose. For the oneEqmodel, i saw the files B, k, p,U,nuSgs, nutilda..
    2. as to the type in those files like inletoutlet, turbulentinlet etc.where do i find a list of all available things that i could use and their description..I tried to look up the source code files and I am not too familiar with C++ .. In fluent, I say the inlet to be like plug flow and the outlet condition to be outflow. how do i specify that in the files?
    3. I finally managed to get it to run with a time step of 1e-6 seconds and it ran for like 10 steps wherein, the max courant number was like 0.19 and then from then onwards, the courant number kept increasing and in a matter a few more timesteps the courant number for 1e6 and the simulation stopped. Not sure why and what to check for.
    4. I then changed to model to dynSmagorinsky in the LES properties file and ran the case, at which point it gave a error about the filter.. I didn't know where to include that info for the solver. Fortunately, I had O1.5 installed as well. in the LES properties file there was inclusion for the filter. I included those lines in my LESproperties file and started the case and it is running now.. Not sure for how long it will run.
  3. Assuming that it will run without any issues, I need to get turbulent statistics like urms, vrms, wrms, tke etc..etc..on the midplane. How do I accomplish that?. I am not sure if this is relevant, but I am running this on a cluster.
As to the solve settings, I am just using the settings of pitzDaily with the LESmodel being dynSmagorinsky.

Sorry for the long posting..

Hope to hear from you guys soon and thanks a tonne in advance..

Vishwa
vishwa is offline   Reply With Quote

Old   September 28, 2009, 17:18
Default
  #2
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
Hi Vishwa,

I'll try to give you some answers so you can go on with your simulations:

1. I don't know what you mean by "adapting the grid" in Fluent, but I usually use fluentMeshToFoam from a .msh file and it works fine. After, be sure to change the types of boundaries in constant/polymesh/boundary.

2.1 Look at the constructor in the .C file of the model you want to use. When MUST_READ is specified, this variable is needed.

2.2 You can refer to the manual for boundary conditions types. I'm not really sure about plug flow, but it sounds like a fixedValue for U (uniform inlet). You can set your outlet as zeroGradient for U and fixedValue for p.

2.3 For your courant number, I suggest you add some correctors for your Piso loop (2 or 3).

2.4 ...

3. For calculating values at each timestep, you can build a functionObject (refer to OpenFOAM-1.5/src/postProcessing/). You can also monitor variables using probes.

Good luck with your simulations and don't give up on OpenFOAM, it's well worth the effort!

Regards,

Philippe
philippebv is offline   Reply With Quote

Old   December 4, 2010, 16:23
Default dynSmagorinsky specifications
  #3
Member
 
Join Date: Oct 2010
Location: Stuttgart
Posts: 35
Rep Power: 6
grandgo is on a distinguished road
hello!

i'm very new in OF.....

i've been looking for "must-read" entries in dynSmagorinsky.C file but i can't find any.....
i still do not know, what this model needs:

1) which files i have to supply
2) how i can choose a filter
3) where i can specify a heat transfer model
4) the near wall treatment....

??

every tutorial case in OF 1.7.1 is using the "oneEqEddy" model. so i have no pattern...

can someone help me? or tell me, where i can find help?

thanks

best regards

Last edited by grandgo; December 4, 2010 at 18:58.
grandgo is offline   Reply With Quote

Old   December 5, 2010, 18:21
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by grandgo View Post
1) which files i have to supply
Clone a tutorial. It does not matter if you have additional files. Smagorinsky models do not need B and k, for example.

Quote:
2) how i can choose a filter
In the LESProperties dictionary, with something like

Code:
dynSmagorinskyCoeffs
{
    filter simple;
}
Quote:
3) where i can specify a heat transfer model
The energy equation is solved only in compressible LES solvers.

Quote:
4) the near wall treatment....
What wall treatment are you looking for?

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 5, 2010, 18:36
Default
  #5
Member
 
Join Date: Oct 2010
Location: Stuttgart
Posts: 35
Rep Power: 6
grandgo is on a distinguished road
hi alberto!

first, thanks for your replying.

1) you said, i can copy a tutorial case. but how do i know, which files a certain model needs? for example, the "oneEqEddy" model needs the "B" and "k" files, apparently. "dynSmagorinsky" doesn't need these files and they don't bother. but maybe it needs other files like "C" or "D"... so how do i get to know, WHICH files are needed IF needed?

4) i meant a near wall model. but after reading the user guide, i think this is specified in the 0/nut file....

best regards
grandgo is offline   Reply With Quote

Old   December 5, 2010, 23:37
Default
  #6
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi,

Quote:
Originally Posted by grandgo View Post
1) you said, i can copy a tutorial case. but how do i know, which files a certain model needs? for example, the "oneEqEddy" model needs the "B" and "k" files, apparently. "dynSmagorinsky" doesn't need these files and they don't bother. but maybe it needs other files like "C" or "D"... so how do i get to know, WHICH files are needed IF needed?
You either read the code to see, or OpenFOAM will complain if an input file is missing.

Quote:
4) i meant a near wall model. but after reading the user guide, i think this is specified in the 0/nut file....
A "near wall model" for what? In 0/nut you can specify the wall-functions for nuSGS, and if you want a fully resolved LES at walls, do not specify the wall-function, but set zeroGradient.

P.S. Are you using the dynamic Smagorinsky model? If so, search for another thread I posted today on this topic. You might find my piece of code useful.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 6, 2010, 08:06
Default
  #7
Member
 
Join Date: Oct 2010
Location: Stuttgart
Posts: 35
Rep Power: 6
grandgo is on a distinguished road
hi alberto,

i wanted to use the dynSmagorinsky model.
but there are two problems, i think:

1) i need a turbulence model that corresponds to the paper of germano et al (1991). and i read before, that dynSmagorinsky model doesnt match germano fully.

2) i need to use a heat transfer model. but you told me, that i have to use a compressible solver to do so. i could take the rhoPisoFoam solver, but there is no dynSmagorinsky model for compressible solvers (OF user guide 1.7.1).

do you have a solution?

i'm going to read your other posts now

thanks,
best regards
grandgo is offline   Reply With Quote

Old   December 6, 2010, 11:53
Default
  #8
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by grandgo View Post
hi alberto,

i wanted to use the dynSmagorinsky model.
but there are two problems, i think:

1) i need a turbulence model that corresponds to the paper of germano et al (1991). and i read before, that dynSmagorinsky model doesnt match germano fully.
Correct. The dynSmagorinsky model is implemented averaging coefficients on the whole domain, which is correct in the case of homogeneous turbulence.

You can pull an implementation that uses local values of the coefficients from my git repository:

git clone git://github.com/AlbertoPa/dynLocalAverageSmagorinsky.git

Test it before using it however.

Quote:
2) i need to use a heat transfer model. but you told me, that i have to use a compressible solver to do so. i could take the rhoPisoFoam solver, but there is no dynSmagorinsky model for compressible solvers (OF user guide 1.7.1).
The solution depends on your need. Do you need heat transfer in an incompressible code, or do you need a compressible code? :-)

If you need an incompressible code, simply add the energy equation to pisoFoam. If you need a compressible code, you will have to implement the compressible version of the dynamic model (not the one from Germano's paper, which does not provide closures for the energy equation).

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 7, 2010, 19:11
Default
  #9
Member
 
Join Date: Oct 2010
Location: Stuttgart
Posts: 35
Rep Power: 6
grandgo is on a distinguished road
hi alberto,

thanks for your support und patience...

can you explain me, how i can insert the energy equation:

{
solve
(
fvm::ddt(rho, h) (--> remove, right?)
+ fvm::div(phi, h)
- fvm::laplacian(turbulence->alphaEff(), h)
==
DpDt
);

thermo.correct();
}


in the pisoFoam.C file? copy and paste this and thats it??
i'm even worse in C++ than in OpenFoam....sorry

best regards
grandgo
grandgo 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
DNS for Impinging Jet on a Flat Plate Chandra Shekhar Main CFD Forum 3 January 18, 2010 06:03
impinging jet natesan Main CFD Forum 3 March 17, 2005 06:42
impinging jet natesan CD-adapco 1 February 25, 2005 04:16
impinging jet data Andreas Abdon Main CFD Forum 4 January 19, 2000 08:40
IMPINGING JET ........... HELP!!!!!!!! Amir Omoumi Main CFD Forum 10 August 30, 1999 22:11


All times are GMT -4. The time now is 10:38.