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

Wall functions Ansys Fluent

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

Like Tree9Likes
  • 8 Post By Far
  • 1 Post By Crank-Shaft

Reply
 
LinkBack Thread Tools Display Modes
Old   November 30, 2012, 15:00
Default Wall functions Ansys Fluent
  #1
New Member
 
Nagrecha R
Join Date: Nov 2012
Posts: 3
Rep Power: 5
rm123 is on a distinguished road
Hi,
Can someone please tell me how to decide on which wall function should i use for k-epsilon equation? I know it is something related to y+ and y* but I will appreciate a bit of detail.

Many thanks.
rm123 is offline   Reply With Quote

Old   December 2, 2012, 01:16
Default
  #2
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,010
Blog Entries: 6
Rep Power: 40
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
There are two type of wall functions available for the high Reynolds number K-epsilon model:

1. Standard wall Functions (Will give problems if mesh is refined below Y+ 30)

2. Scalable wall function. Applicable for the meshes with even Y+ 1. But still it is wall function. The only purpose of scalable wall function is to avoid problems of successive refinements in standard wall function meshes. The algorithm ensures that your solver Y+ (Y* in Fluent) is always greater than 11.225. Y+= 11.225 is the intersection of linear and log law profile.
It has function which chooses the maximum of (11.225, Y*).

You already know that the Y* is different than the Y+ somehow. I don't remember when they are different and when they are same, having to do with buffer and log layer (Hint: turbulent and viscous stresses). Check the related material on the Y* and Y+. But any how in background fluent uses the Y*. So it will choose the 11.225 if Y* is less than 11.225 and uses Y* if it is greater than 11.225.

For low Reynolds number K-epsilon model there are two methods available (Select option enhanced wall treatment).

1. If Y+ is less than 1, it uses the pure two layer model and you solve the viscous sub layer. This formulation is good when you have separation or you want to resolve the near wall effects e.g. drag prediction, otherwise this will wast your resources and takes more solution time due to excessive stretching of mesh in the boundary layer.

2. If Y+ is variable along the wall (which is always present in practical industrial problems) then it use the enhanced wall treatment. It is the method to implement the enhanced wall function (hybrid wall function see this y+=1 vs Wall Function and Enhanced Wall Treatment ) for the two layer k-epsilon model) For this method you should ensure Y+<10 for best usage. Otherwise for the higher Y+ values this will gradually use the log layer i.e. wall function approach.
Far is offline   Reply With Quote

Old   December 4, 2012, 20:45
Default
  #3
New Member
 
Nagrecha R
Join Date: Nov 2012
Posts: 3
Rep Power: 5
rm123 is on a distinguished road
Hi Far,

Thanks a lot for your help.
Also I have one question is how to calculate total pressure drop between inlet and outlet in ANSYS?

Many thanks...
rm123 is offline   Reply With Quote

Old   December 4, 2012, 23:37
Default
  #4
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,010
Blog Entries: 6
Rep Power: 40
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
It is total pressure difference at inlet and outlet....
Far is offline   Reply With Quote

Old   December 13, 2012, 07:29
Default Particle velocity in solid-gas flow
  #5
New Member
 
Aisha
Join Date: Dec 2012
Location: Malaysia
Posts: 3
Rep Power: 5
3ashoosh is on a distinguished road
Send a message via Skype™ to 3ashoosh
Dear all,

I am running a 2D simulation for FCC riser in ANSYS Fluent 14 using Eulerian multiphase model for the solid-gas flow. I use the standard k-epsolon per phase turbulence model with the standard wall function. The geometry is so simple axisymmetric pipe. The inlet boundary conditions for both phases were coded in UDF .c file and interpreted in the fluent setting up.

When running the case, it converged after 100's of iterations but the outflow particle velocity profile is not parabolic (not fully developed). It decreases slowly from the centre then fall sharply near the wall. Some times has another peak (maxima) near the wall as if it is an annular core flow.
I used no slip conditions for both phases at the wall, also tried different specularity coefficients for the solid phase, but I got same results.

When plotting the wall Y+ value for the solid phase, it changed sharply from 25 to 300 at the inlet then remain between 150 and 160 for the rest of the metres along the wall. And for the gas phase it stays below 20.

I don't know what to do to get the parabolic profile at the out let?
I appreciate any kind of help,

Regards,
3ashoosh
3ashoosh is offline   Reply With Quote

Old   December 27, 2012, 03:58
Default
  #6
New Member
 
Mohammed
Join Date: Oct 2012
Posts: 27
Rep Power: 5
mohw2002 is on a distinguished road
Quote:
Originally Posted by Far View Post
There are two type of wall functions available for the high Reynolds number K-epsilon model:

1. Standard wall Functions (Will give problems if mesh is refined below Y+ 30)

2. Scalable wall function. Applicable for the meshes with even Y+ 1. But still it is wall function. The only purpose of scalable wall function is to avoid problems of successive refinements in standard wall function meshes. The algorithm ensures that your solver Y+ (Y* in Fluent) is always greater than 11.225. Y+= 11.225 is the intersection of linear and log law profile.
It has function which chooses the maximum of (11.225, Y*).

You already know that the Y* is different than the Y+ somehow. I don't remember when they are different and when they are same, having to do with buffer and log layer (Hint: turbulent and viscous stresses). Check the related material on the Y* and Y+. But any how in background fluent uses the Y*. So it will choose the 11.225 if Y* is less than 11.225 and uses Y* if it is greater than 11.225.

For low Reynolds number K-epsilon model there are two methods available (Select option enhanced wall treatment).

1. If Y+ is less than 1, it uses the pure two layer model and you solve the viscous sub layer. This formulation is good when you have separation or you want to resolve the near wall effects e.g. drag prediction, otherwise this will wast your resources and takes more solution time due to excessive stretching of mesh in the boundary layer.

2. If Y+ is variable along the wall (which is always present in practical industrial problems) then it use the enhanced wall treatment. It is the method to implement the enhanced wall function (hybrid wall function see this y+=1 vs Wall Function and Enhanced Wall Treatment ) for the two layer k-epsilon model) For this method you should ensure Y+<10 for best usage. Otherwise for the higher Y+ values this will gradually use the log layer i.e. wall function approach.
Hello, I am using CFX and I want to get the values of y+, k+ and epsilon+ in the pipe for two cases one with perforations and without perforations.
Thanks in advance
mohw2002 is offline   Reply With Quote

Old   December 27, 2012, 10:26
Smile
  #7
New Member
 
Aisha
Join Date: Dec 2012
Location: Malaysia
Posts: 3
Rep Power: 5
3ashoosh is on a distinguished road
Send a message via Skype™ to 3ashoosh
Quote:
Originally Posted by Far View Post
There are two type of wall functions available for the high Reynolds number K-epsilon model:

1. Standard wall Functions (Will give problems if mesh is refined below Y+ 30)

2. Scalable wall function. Applicable for the meshes with even Y+ 1. But still it is wall function. The only purpose of scalable wall function is to avoid problems of successive refinements in standard wall function meshes. The algorithm ensures that your solver Y+ (Y* in Fluent) is always greater than 11.225. Y+= 11.225 is the intersection of linear and log law profile.
It has function which chooses the maximum of (11.225, Y*).

You already know that the Y* is different than the Y+ somehow. I don't remember when they are different and when they are same, having to do with buffer and log layer (Hint: turbulent and viscous stresses). Check the related material on the Y* and Y+. But any how in background fluent uses the Y*. So it will choose the 11.225 if Y* is less than 11.225 and uses Y* if it is greater than 11.225.

For low Reynolds number K-epsilon model there are two methods available (Select option enhanced wall treatment).

1. If Y+ is less than 1, it uses the pure two layer model and you solve the viscous sub layer. This formulation is good when you have separation or you want to resolve the near wall effects e.g. drag prediction, otherwise this will wast your resources and takes more solution time due to excessive stretching of mesh in the boundary layer.

2. If Y+ is variable along the wall (which is always present in practical industrial problems) then it use the enhanced wall treatment. It is the method to implement the enhanced wall function (hybrid wall function see this y+=1 vs Wall Function and Enhanced Wall Treatment ) for the two layer k-epsilon model) For this method you should ensure Y+<10 for best usage. Otherwise for the higher Y+ values this will gradually use the log layer i.e. wall function approach.
Hi,
Is this also true for multi phase. I mean how can I adapt the Y+ values? When I click the adapt button then Yplus/Ystar adaptation window then on clicking compute for phase 1 (air) gave max of 43.33. Then when I put the min allowed 30 and max allowed 300 and click adapt it gave me an error, fata signal (ACCESS_VIOLATION)
Can you or any one help me? Thanks
3ashoosh is offline   Reply With Quote

Old   January 13, 2013, 01:31
Thumbs up
  #8
Senior Member
 
Crank-Shaft's Avatar
 
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 145
Rep Power: 5
Crank-Shaft is on a distinguished road
Quote:
Originally Posted by Far View Post
There are two type of wall functions available for the high Reynolds number K-epsilon model:

1. Standard wall Functions (Will give problems if mesh is refined below Y+ 30)

2. Scalable wall function. Applicable for the meshes with even Y+ 1. But still it is wall function. The only purpose of scalable wall function is to avoid problems of successive refinements in standard wall function meshes. The algorithm ensures that your solver Y+ (Y* in Fluent) is always greater than 11.225. Y+= 11.225 is the intersection of linear and log law profile.
It has function which chooses the maximum of (11.225, Y*).

You already know that the Y* is different than the Y+ somehow. I don't remember when they are different and when they are same, having to do with buffer and log layer (Hint: turbulent and viscous stresses). Check the related material on the Y* and Y+. But any how in background fluent uses the Y*. So it will choose the 11.225 if Y* is less than 11.225 and uses Y* if it is greater than 11.225.

For low Reynolds number K-epsilon model there are two methods available (Select option enhanced wall treatment).

1. If Y+ is less than 1, it uses the pure two layer model and you solve the viscous sub layer. This formulation is good when you have separation or you want to resolve the near wall effects e.g. drag prediction, otherwise this will wast your resources and takes more solution time due to excessive stretching of mesh in the boundary layer.

2. If Y+ is variable along the wall (which is always present in practical industrial problems) then it use the enhanced wall treatment. It is the method to implement the enhanced wall function (hybrid wall function see this y+=1 vs Wall Function and Enhanced Wall Treatment ) for the two layer k-epsilon model) For this method you should ensure Y+<10 for best usage. Otherwise for the higher Y+ values this will gradually use the log layer i.e. wall function approach.
Fantastic explanation Far. This is so much clearer to me now and although I haven't used the k-epsilon turbulence model lately, learning about the various features in a simplified and intuitive manner is definitely appealing.

Thanks for sharing your knowledge.
Far likes this.
__________________
--
Mechanical Engineering
Sydney, Australia


Crank-Shaft is offline   Reply With Quote

Old   February 28, 2013, 04:20
Default Translatio CFX-pre
  #9
New Member
 
Mohammed
Join Date: Oct 2012
Posts: 27
Rep Power: 5
mohw2002 is on a distinguished road
Hi everyone
I am looking for the answer about the translation by CFX-pre. My geometry is quarter pipe (inlet-velocity is boundary condition for axial inlet) with perforation at upper surface (mass flow rate for radial boundary conditions) and outlet-pressure for outlet pipe at 120" long. Please I want to extent this pipe to 2 copies i.e. to be 3 domains (one total domain) the total long is 360".
Now for the new domain one axial inlet (inlet-velocity at the beginning of the pipe) and at the end of the total domain is (outlet-pressure). My question what I will put the boundary conditions for the interfaces between 1 and 2, 2 and 3?

Thanks
mohw2002 is offline   Reply With Quote

Old   March 8, 2014, 09:01
Default multiphase wall functions
  #10
Senior Member
 
rkhr
Join Date: May 2011
Posts: 229
Rep Power: 7
Kanarya is on a distinguished road
hi,
is there any modifications in wall functions in fluent for two fluid models?
thanks in advance!
Kanarya is offline   Reply With Quote

Old   March 19, 2014, 05:43
Default
  #11
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,010
Blog Entries: 6
Rep Power: 40
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
i have no info about the two phase flow
Far is offline   Reply With Quote

Old   February 11, 2016, 15:01
Default Wall function for very rough surfaces
  #12
New Member
 
Siamak Gharahjeh
Join Date: Aug 2012
Posts: 27
Rep Power: 5
siamakghh2000 is on a distinguished road
Hello all,

Does anyone know if there is a certain type of wall function out there used for very rough surfaces?

Yours, respectfully,
Siamak Gharahjeh
siamakghh2000 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
Two-Sided Wall in FLUENT mlippy38 FLUENT 17 March 18, 2014 04:37
error in opening fluent in ansys workbench tmeysam92 ANSYS 3 March 12, 2013 07:10
Enhanced wall treatment and Enhanced wall functions Alina FLUENT 2 January 3, 2012 19:48
Wall function formulation in CFX and Fluent gravis ANSYS 0 May 4, 2010 11:03
Wall functions tutlhino OpenFOAM Pre-Processing 0 July 2, 2007 05:04


All times are GMT -4. The time now is 00:40.