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

DPM with boundary inflation layer

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

Like Tree6Likes
  • 1 Post By RodriguezFatz
  • 2 Post By Far
  • 1 Post By Far
  • 1 Post By RodriguezFatz
  • 1 Post By RodriguezFatz

Reply
 
LinkBack Thread Tools Display Modes
Old   August 14, 2014, 09:53
Default DPM with boundary inflation layer
  #1
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Hello all,

I am using DPM and k-w SST turbulence model.

The k-w SST turbulence model requires a very fine mesh at the boundary (yplus value <2).

However if yplus value is very small, while doing particle tracking it not only takes a long time but also results incomplete tracking (8200 tracked & 6500 incomplete).

So it seems small yplus value =? successful particle tracking. Can anyone help?

Thanks,
Richard
richard ben is offline   Reply With Quote

Old   August 15, 2014, 01:43
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Hi Richard,

First of all k-w SST also runs with wall functions, so it doesn't require a resolved boundary layer.
Now, I am not 100% sure about that, but I think that DPM algorithm is based on the fact that particles move through single cells. Thus, cells must be large compared to the particle size. So I remember my simulation crashing when particles moved into zones with cell sizes that are smaller than themselves.
richard ben likes this.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 15, 2014, 21:05
Default
  #3
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
RodriguezFatz,

Thank you so much for your reply.

I guess you are right that the cell size has to be smaller than the particle size. I changed the mesh (inflation layer thickness), and the results is much better. Less particles are incomplete. Again I appreciate your help. Now but the problem is the yplus value is bigger than 10.

What do you mean by saying "k-w SST doesn't require a resolved boundary layer"? I don't need to create inflation layers? I found from the Fluent guide that the all k-w models use enhanced wall treatment. And this wall treatment, the yplus value of the first layer should be 1-10 and smaller than 2 is even better. Is this the same as/different from what you meant?

Thanks,
Richard
richard ben is offline   Reply With Quote

Old   August 16, 2014, 03:49
Default
  #4
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Latest near wall model implemented (in fluent and CFX) is hybrid-type model which does not require yplus to be 2. Y+ up to 10 would produce the same results as lower values.

http://num.math.uni-goettingen.de/ba...ings/knopp.pdf

Quote:
What do you mean by saying "k-w SST doesn't require a resolved boundary layer"?
It means that There are three versions (in fact implemented through one universal wall model) of wall model.
1. Low Re model (requires Y+ <2 for omega based models and SST is one of them)
2. Wall function model : Works with Y+ > 30
3. Model to treat the buffer zone

If your mesh has yplus greater than 30, Wall function model will be activated. If it is lower than 2, low Re model shall be activated. If it is varying from 2- 100 hybrid model shall be implemented.

Some comments :

1. There is no need to use Y+ 2 and 40 layers in boundary layer. Y+ 10 and 10-15 no of layers in boundary layer are enough to capture the effects of wall on main flow

2. SST with wall function model produced the most poor results than any other model. Instead use K-epsilon with scalable wall function

3. Very low values of Y+ mean stretched meshes or high aspect ratio cell. Which also slow down the convergence rate significantly.
richard ben and seu_007 like this.
Far is offline   Reply With Quote

Old   August 18, 2014, 11:08
Default
  #5
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Far,

Thanks for your information.

I changed my mesh as much as I can and the majority of the y+ value is between 10-13, but the mam is 16, min is 2.

Now my another question is how to determine the NO. of inflation layers? Is there any standard to decide (like the y+ at the outset inflation layer) ? You mentioned 10 -15 and I tried them, they gave me different results.

Thanks,
Richard
richard ben is offline   Reply With Quote

Old   August 18, 2014, 11:28
Default
  #6
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Use flat plate empirical formulae for boundary layers thickness for laminar and turbulent flows. Use that value in your meshing software and make sure in that region you have 10-15 layers.

You can also see in post processing by plotting the velocity vectors (or contour plots) to confirm that boundary thickness you had selected is enough or not.
richard ben likes this.
Far is offline   Reply With Quote

Old   August 18, 2014, 12:04
Default
  #7
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Far,

I appreciate a lot for your help. I will try that and get back to you here.

Thanks,
Richard
richard ben is offline   Reply With Quote

Old   August 18, 2014, 12:13
Default
  #8
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
There are guys who are much better like Philipp, flotus and many more...
Far is offline   Reply With Quote

Old   August 19, 2014, 08:58
Default
  #9
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Richard, you were asking about the inflation layers. I didn't really get what you tried. Did you have 10 layers in one mesh and then 15 in a second mesh and your result changed? What result?
richard ben likes this.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 19, 2014, 09:44
Default
  #10
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Philipp,

Yes I have one mesh with 10 inflation layers and 15 with the other. I solved the flow solution first, then used DPM to do particle tracking, output the mass flow rate at the outlets so as to calculate the particle concentration. The particle concentration (result) changed in different mesh.

I am still trying what Sijal suggested - check the velocity vector so far. But haven't had any clue. Cause it is 3D model. But I will keep trying. I will be more than happy if you have any advice on this.

Thanks
Richard
richard ben is offline   Reply With Quote

Old   August 19, 2014, 09:48
Default
  #11
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
Hi,

1) It changed - how much?
2) I remember one setting in the DPM settings that says something like "normalize particle to face area". Do you know what I mean? Did you check that box?
richard ben likes this.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 19, 2014, 10:13
Default
  #12
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Thanks again.

1) I have two models. I tried to generate mesh with 5, 7, 10 and 15 inflation layers. The result for one of the models changes from 0.205 to 0.119, however the experimental data is 0.127.

2) I didn't get what you meant. I found "Scale Flow Rate by Face Area" in the DPM injection setting. But I think that's not the same. BTW, what's the "Normalize Particle to Face Area" for?

Thanks
Richard
richard ben is offline   Reply With Quote

Old   August 19, 2014, 10:22
Default
  #13
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
https://imageshack.com/i/exQe2oswp

This is my mesh with 15 inflation layers. I found it weird.
richard ben is offline   Reply With Quote

Old   August 19, 2014, 10:27
Default
  #14
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
2) Scale Flow Rate... Yeah, that's what I mean... I am pretty sure this makes sense to have checked.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 19, 2014, 10:32
Default
  #15
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Yeah I checked it. BTW can you see my mesh pic? I have no idea whether I uploaded it in the correct way.
richard ben is offline   Reply With Quote

Old   August 19, 2014, 10:35
Default
  #16
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19
RodriguezFatz will become famous soon enough
This mesh looks pretty coarse... Don't you have ICEM to make a good mesh?
It's done with that ANSYS mesher right? Why would they put triangles in the boundary? I am sure you can get better meshes even with that tool... Try to get a good mesh with help in the ANSYS meshing section of the forum.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 19, 2014, 10:46
Default
  #17
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
Yes I did my mesh in ANSYS Workbench. I will try to mesh it again.

Thanks
richard ben is offline   Reply With Quote

Old   October 14, 2014, 11:54
Default
  #18
New Member
 
Join Date: Jan 2014
Posts: 11
Rep Power: 4
ruturaj171 is on a distinguished road
I am trying mist cooling plate fin heat sink. I am getting convergence if residual is 0.001 with standard wall function k-epsilon. But if i reduce residual to 0.0001 then I am not getting convergence. Also if stop simulation in between for residual 0.0001 and see the results that also seems wrong to me. Can anybody help me?
Thanks
ruturaj171 is offline   Reply With Quote

Old   October 16, 2014, 21:29
Default
  #19
Member
 
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 5
richard ben is on a distinguished road
You can try decrease the under-relaxation factor. And see whether it get convergence. But there are many other ways like checking the mesh etc.
richard ben 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
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Divide Prismatic Boundary Layer Mesh causes overlapping faces SilentRunner42 enGrid 4 May 4, 2015 03:37
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
errors Fahad Main CFD Forum 0 March 23, 2004 14:20


All times are GMT -4. The time now is 15:04.