|
[Sponsors] |
August 14, 2014, 10:53 |
DPM with boundary inflation layer
|
#1 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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 |
|
August 15, 2014, 02:43 |
|
#2 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
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.
__________________
The skeleton ran out of shampoo in the shower. |
|
August 15, 2014, 22:05 |
|
#3 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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 |
|
August 16, 2014, 04:49 |
|
#4 | |
Super Moderator
|
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:
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. |
||
August 18, 2014, 12:08 |
|
#5 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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 |
|
August 18, 2014, 12:28 |
|
#6 |
Super Moderator
|
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. |
|
August 18, 2014, 13:04 |
|
#7 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
Far,
I appreciate a lot for your help. I will try that and get back to you here. Thanks, Richard |
|
August 19, 2014, 09:58 |
|
#9 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
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?
__________________
The skeleton ran out of shampoo in the shower. |
|
August 19, 2014, 10:44 |
|
#10 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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 |
|
August 19, 2014, 10:48 |
|
#11 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
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?
__________________
The skeleton ran out of shampoo in the shower. |
|
August 19, 2014, 11:13 |
|
#12 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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 |
|
August 19, 2014, 11:22 |
|
#13 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
||
August 19, 2014, 11:27 |
|
#14 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
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. |
|
August 19, 2014, 11:32 |
|
#15 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
Yeah I checked it. BTW can you see my mesh pic? I have no idea whether I uploaded it in the correct way.
|
|
August 19, 2014, 11:35 |
|
#16 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
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. |
|
August 19, 2014, 11:46 |
|
#17 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
Yes I did my mesh in ANSYS Workbench. I will try to mesh it again.
Thanks |
|
October 14, 2014, 12:54 |
|
#18 |
New Member
Join Date: Jan 2014
Posts: 11
Rep Power: 12 |
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 |
|
October 16, 2014, 22:29 |
|
#19 |
Member
ben
Join Date: Apr 2013
Posts: 36
Rep Power: 12 |
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.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 08:38 |
Divide Prismatic Boundary Layer Mesh causes overlapping faces | SilentRunner42 | enGrid | 4 | May 4, 2015 04:37 |
Error finding variable "THERMX" | sunilpatil | CFX | 8 | April 26, 2013 08:00 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 16:55 |
errors | Fahad | Main CFD Forum | 0 | March 23, 2004 14:20 |