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

"LRR Turbulent Model" Problems

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

Like Tree1Likes
  • 1 Post By maysmech

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2011, 13:01
Question "LRR Turbulent Model" Problems
  #1
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
maysmech is on a distinguished road
Dear experts,
By changing KEpsilon to LRR in constants/RASProprties OpenFOAM works fine apparently but the problem is in this model: k and epsilon which is set for inlet has a sharp decrease toward internal domain for example in my case which is a backward facing step it reach from k=7.5 to 0.0001, also same for epsilon.
I think it is a reason which it is not possible to reach true answer.
Settings are same as pitzDaily tutorial. i used pisoFoam.
What is the problem?
Any suggestion will be appreciated.
Regards.
maysmech is offline   Reply With Quote

Old   March 12, 2011, 04:43
Default
  #2
Senior Member
 
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 10
idrama is on a distinguished road
Hard to day: Did u set the inlet conditions for R correctly, meaning everywhere zero apart from the main diagonal and on the k=... I haven't the conditions formula on me, but you can loop up in Versteeg.
idrama is offline   Reply With Quote

Old   March 12, 2011, 04:49
Default
  #3
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
maysmech is on a distinguished road
inlet R is set zero for all 9 elements.
maysmech is offline   Reply With Quote

Old   March 12, 2011, 05:46
Default
  #4
Senior Member
 
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 10
idrama is on a distinguished road
You must set the BC for R correctly:

Compute k=3/2*(U_ref*Ti)^2

For U_ref take the velocity at the inlet, look in "U", set Ti = 0.05 (for other cases you muss adjusted it). If you have concrete value for k than set for R at the inlet:

type fixedValue;
value uniform (k/2 0 0 k/2 0 k);

as you can see the k-values are divided by 2; one is untouched, this one points in flow direction (here z-axis). Since you integrate a epsilon equation with these, you must set the BC suitable. Somewhere in the user guide or programmer's guide is an entry, you gotta go for it.
idrama is offline   Reply With Quote

Old   March 12, 2011, 07:55
Default
  #5
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
maysmech is on a distinguished road
Quote:
Originally Posted by idrama View Post
You must set the BC for R correctly:

Compute k=3/2*(U_ref*Ti)^2

For U_ref take the velocity at the inlet, look in "U", set Ti = 0.05 (for other cases you muss adjusted it). If you have concrete value for k than set for R at the inlet:

type fixedValue;
value uniform (k/2 0 0 k/2 0 k);

as you can see the k-values are divided by 2; one is untouched, this one points in flow direction (here z-axis). Since you integrate a epsilon equation with these, you must set the BC suitable. Somewhere in the user guide or programmer's guide is an entry, you gotta go for it.
Dear Claus,
Thanks for your suggestion.

i have calculated k and epsilon. k=7.5 and epsilon=500.
But by seeing incompressible/simpleFoam/pitzdaily tutorial decide to use (0 0 0 0 0 0) for inlet R.
By changing inlet R to what you told answers are seemed to be better.
Two questions:
1- How can R be calculated to what value you told? i mean if x direction be streamwise or if it be 3D and ...
2- Is T=(a b c d e f) means:
a d e
d b f
e f c
or it has another format for symmetric tensors. i searched in user guide and programmers guide but nothing found about it.
maysmech is offline   Reply With Quote

Old   March 12, 2011, 11:36
Default
  #6
Senior Member
 
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 10
idrama is on a distinguished road
(1) Basically, when you consider a canonical reference frame where the inlet is pointing into the x-direction than you must set:

R=(k 0 0 k/2 0 k/2),

i.e. in flow direction k and into the others k/2. The reason why k appears here is due to the relationship trace(R)=2*k (look Versteeg).

R is a symmetric tensor; to reduce memory consumption the symmetry property is exploited, i.e. 6 entries instead of 9, so (2) is right!

R is called the Reynolds Stress Tensor and appearce by reynolds averaging procedure.

My suggestion: Try to get Versteeg. Many times posted here and by simply entering it in google; you find in google books, definitely.

Cheers and good luck
idrama is offline   Reply With Quote

Old   March 12, 2011, 12:31
Default
  #7
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 9
maysmech is on a distinguished road
I have Versteeg. thanks for your suggestion.
if trace of reynolds stress tensor should be 2k and if your told R could be true, format of 6 elements tensor instead of 9 elements couldn't be what i told.
it should be:

T=(a b c d e f) means:
a b c
b d e
c e f

Isn't it?
songwukong likes this.
maysmech is offline   Reply With Quote

Old   March 12, 2011, 13:58
Smile
  #8
Senior Member
 
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 10
idrama is on a distinguished road
You got it, foamer!
idrama 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
Stability problem due to turbulent dispersion force in a subcooled boiling model Edy OpenFOAM 7 August 10, 2011 12:00
Laminar vs Turbulent Navier-Stokes truman Main CFD Forum 6 March 7, 2011 14:44
Turbulent Kinetic Energy Olga FLUENT 2 October 11, 2002 15:05
Problem of Turbulent Viscosity Ratio Limited David Yang FLUENT 3 June 3, 2002 06:13
Turbulent viscosity Christian Holm Main CFD Forum 4 June 23, 2001 22:04


All times are GMT -4. The time now is 19:55.