
[Sponsors] 
April 9, 2013, 14:46 
Boundary Layer Calculation Y+

#1 
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Hello CFD Users,
I was another Student who have problems with Boundary Layers.... I would like to simulate the turbulence between Trains in a wind tunnel. I have already calculated my wall distance with the Y+ calculator. My first Question is: I would like to simulate the problem with SST (Menters). It is right, I have to set the Y+ from 30 up to 300 and construct my boundary layer between this Y+ Numbers!? > First Layer 030, then with growth rate from 30300 (510 Layers)!? My second problem: I have a really big Model (10m20m) and need a Layer with Y=0,0002m first layer thickness with Y+=30. When I want a Layer up to Y+=300 I get Y=0,002m. ...and thats a really thin/small layer. (Im working with Hypermesh, AcuConsole and AcuSolve, velocity=55m/s) Hope anyone has experience with similar problems and can help me!!!! Sorry for my terrible english...., and thx for every answer 

April 10, 2013, 07:06 

#2 
New Member

Hi,
As far as i understand you need Y+ = 30 to 300 That does not mean that your First Layer Height should be 30 or 300... The first layer height should be able to provide you Y+= 30, that means that from the calculation http://www.cfdonline.com/Tools/yplus.php base on the velocity... density.. etc you get your Reynolds number and the first element height. So please tell us first what you get there after you fill up the data... then in HM you can add this First element height on the menu for CFD meshing and add a growth rate of 1.2 to 1.3 but please do not choose more than 1.5 as far for the second question, I have a really big Model (10m20m) and need a Layer with Y=0,0002m first layer thickness with Y+=30. When I want a Layer up to Y+=300 I get Y=0,002m. ...and thats a really thin/small layer. Yep, if your calculations are ok, then we need that first element height, can you share with me your data? Thanks Lazaros 

April 10, 2013, 13:51 

#3 
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Hi Lazaros,
thank you very much!! I understand, to calculate my first layer thickness. I looked on different homepages and the best thing I read about the SST and Y+ is: "The SpalartAllmaras 1equation turbulence model includes automatic switching between using a wall function approach wherever the mesh has y+ between 30 and 300, to fully resolving the boundary layer in the regions where the mesh has a y+ of 1. If the flow has separation or strong adverse pressure gradients, then you will need to model these regions with a y+ of 1 to accurately capture the boundary layer behaviour. Similar to the SpalartAllmaras model, the komega SST 2equation turbulence model is able to work with either Wall Functions or fully resolve the boundary layer, so the same y+ conditions apply. So we can have y+ of between 30 and 300, or a y+ of 1 if the flow has adverse pressure gradients or separation regions that need to be properly resolved. The use of scalable wall functions will automatically activate the local usage of the log law in regions where the y+ is sufficiently small to fully resolve the boundary layer, in conjunction with the standard wall function approach in any regions where the y+ is coarser." > http://www.computationalfluiddynamics.com.au/tipstricksturbulencewallfunctionsandyrequirements/ But I dont understand the follow topics: 1.) What is better Y+=30 or Y+=300 and what are the criterion to set a small or a big Y+????? The size of my model, the velocity, the Fluid.... 2.) The next topic is: How much Boundary Layers I need or how high was the complete BL?? Example: Y+ = 30 Y+=300 When I using Y+=30 I get a boundary layer = 0,00025m = 0,25mm When I using Y+=300 > 0,0025m = 2,5mm > my conclusion: When I create a boundary layer with 0,25mm FIRST LAYER THICKNESS And then 78 another Layers I get a complete thickness from ALL Layers up to 2,5mm (Y+=300). But the craziest thing of all is: In my last post I write about too small layers to compute these in Hyperworks. The Problem is, when I use the "1st cell height Calculator" in Hyperworks, I get the first layer thickness with 0,00045m = 0,45mm When I now press ACCEPT, Hyperworks assumes the Number in [m], but my model is in [mm]. I have already run AcuSolve with a 0,0005mm = 0,0000005m first cell thickness in the boundary layer. In the next two days I show you pics, what the velocity and the Y+ display in the Result. The Y+ is only in the first layer..... Sorry, but I cant upload the model, because its from a great corporation.... Greetings and I hope u understand..... 

April 11, 2013, 03:30 

#4 
New Member

Hi Ruben,
Well, about Hmesh, the number that provides you have to study a little bit cause it seems that the calculation in Hm has some issues. As far for the number that apply the gui on the box, you have to uderstand that HM is not having Units, the engineer have to think everytime the unit system that he is using, ( meters, Pascal etc) and to apply the number. The Y+ calculator in HM have to have units, so it provides you a First Element Height in meters since the numbers of density etc are on meters. SO in case that you have "mm" you have to change of that to mm. About your questions But I dont understand the follow topics: 1.) What is better Y+=30 or Y+=300 and what are the criterion to set a small or a big Y+????? It is better to use Y+=30 The size of my model, the velocity, the Fluid.... 2.) The next topic is: How much Boundary Layers I need or how high was the complete BL?? You have to use a number of layers that will provide you a very good transition to tetra core, so the final layer element have to be not smaller than 50% of the next tetra element i would say not less than 60 % About that > my conclusion: When I create a boundary layer with 0,25mm FIRST LAYER THICKNESS And then 78 another Layers I get a complete thickness from ALL Layers up to 2,5mm (Y+=300). The total number of layers as i say is to define a smooth transition to the tetra core, if the total height of the layers is 2.5 mm that does not mean that your Y+ in 300.... only the first element height is important for the y+ Did you create the 0.00005 mm Firt element Height in HM or in Acusolve? Thx 

April 11, 2013, 12:43 

#5 
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Hey Lazaros,
thx for reply again. Now I understand....., not all, but the bigger part of the topic! I have found this formula too: . Its the Formula to calculate, where you have 99% from your mean velocity U, in normal direction from your wall. But its for a flat plate, today I download the book from Schlichting to get more information about this. Yes, I made a super fine Layer with HM (0.00005mm, growth rate 1,2 and 3 Layers). It works and I made a run with AcuSolve. It works with the SSTModel, but dont converge. The komega Model has with the same Mesh problems. I have suddenly areas where i get a lot of kinetic energy!? Then the energy appears and jump in a other Area of the fluid. Now I go drink a beer because I have birthday today! THX and I give feedback again! Last edited by Appleologe; April 11, 2013 at 16:21. 

April 11, 2013, 12:56 

#6 
Member
Elena Cortin
Join Date: Mar 2009
Location: Paris
Posts: 65
Rep Power: 10 
Hi
I have that issue with Y+ can you help me? 

April 11, 2013, 13:12 

#7 
New Member

Hi Ruben,
Happy Birthday ! ! I am sure that if you drink a couple of Beers the run with converge.. )) Please do not hesitate to contact me for any issue ( Regardign acusolve as well) Regards Lazaros 

April 11, 2013, 13:15 

#8 
New Member


April 17, 2013, 14:03 

#9  
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Quote:
Ok, now I have made a run with a Y+=30 value. First BL=0.2mm complete BL=2,75mm (growth rate 1.15 and 8 Layers) In the postprocessor, the results from Y+ was 20003000 in the area I need accurate resolutions. And it converge not. Then I remesh the model with a first BL=0.02mm and completely BL=0,275mm. At the moment the calculation is running the last 2 days, and it converge. At the moment I have residuals near then 0,0001 (eddy viscosity and pressure) and the residuals from velocity was already smaller then 1*10^5. I hope thats the right way.... At the moment i run with the Spalart Allmars model. When this run was finished I swap to the SSTMenters Model. INFORMATION: I write bullshit in the last threads, I made the first run with an Layer: > 0,005mm < Sooooorry @Lazaros: what are you doin with AcuSolve?! you work with it in your business or you are a student, or make things at home?! Last edited by Appleologe; April 17, 2013 at 14:24. 

April 18, 2013, 02:49 

#10 
New Member

Hi Ruben,
For a velocity of 55 meters per second the Y+ should be less than 2.1e4 , BUT, if you have sharp edges that will increase the velocity on the area that you have to have Y+ =30 then you have to count the Y+ in that area. So be careful with the local velocity as well But you already saw that... The residuals seems fine, i think that your results are ok. I would like to ask you somethings, how many elements do you have? What kind of workstation ? I think that 2 days run is too much , please inform me about that Also, please take a look the transition from the BL to tetra core, the ratio between tetra and BL ( last element height ) should not be more than 2. PS i am working for Altair..... 

April 18, 2013, 03:55 

#11  
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Quote:
My wind tunnel have a size: length=21500mm width= 6000mm heigth= 8000mm The Model Size is: length=21500mm width=2.8/2=1.4m=1400mm heigth=4600mm At the Moment I have on the surface of the Model Cells ~1020mm Then the small Layer ~0.3mm and on the Layer I create a TetMesh with Interpolate. At the moment I have 3 Modells: 1.) 1,7 Mio Cells > Start now with same Boundary Conditions 2.) 3,6 Mio Cells > This is the model with small residuals 3.) 4,9 Mio Cells > Last Run i will start over the Weekend my Cell heigth in the last Layer is 0,05mm and my Cells next to the BL in the 3,6 Mio model are ~1020mm. Thats really bad..... Its not 2 is more than 100!!! The only thing I can test is to give a smaller "transition ratio" in CFD tetramesh!!!! Computer: Lenovo S20 Workstation CPU: 2,66 GHz XEON W3520 RAM: 16GB GPU: Quadro Fx 4800 Last edited by Appleologe; April 18, 2013 at 05:43. 

April 18, 2013, 06:09 

#12 
New Member

Ruben,
that is fine, you can do that. here is some advices 1) create more Boundary Layers , 2create first 10 layers with Growth rate of 1.2 2) Then create "face" and on these faces of the first BL group just create another on BL with 10 layers with Growth rate of 1.5 Take a look these numbers No of Layer Growth Rate Thickness of Last layer total thickness 1 1,2 0,02 14,55337309 2 1,2 0,024 3 1,2 0,0288 4 1,2 0,03456 5 1,2 0,041472 6 1,2 0,0497664 7 1,2 0,05971968 8 1,2 0,071663616 9 1,2 0,085996339 10 1,2 0,103195607 11 1,5 0,123834728 12 1,5 0,185752093 13 1,5 0,278628139 14 1,5 0,417942209 15 1,5 0,626913313 16 1,5 0,940369969 17 1,5 1,410554954 18 1,5 2,115832431 19 1,5 3,173748646 20 1,5 4,760622969 Then you will have last element height of 5 mm almost and total BL thickness of 14 mm Then create a refinment box over your area that you need to study ( train, car etc) and apply as tetra size of 40 mm You will have a model of 20 million elements Your workstation is ok to handle that in HM and Acusolve you will need 4 hours to solve that model Laz 

April 18, 2013, 07:11 

#13  
New Member
Ruben Geiger
Join Date: Apr 2013
Posts: 8
Rep Power: 6 
Quote:
I made the cells on the Surface a little bit smaller then I need a smaller layer. EDIT: Today I calculate a the File with 1600000 Elements, in 5 hours = 75 iterations. 20 Mio....., that`s more then to much. I test on the Weekend a File with ~4 Mio Elements, but I think thats already to slow. We have in the company a datacenter with more power, when i get good results and the my computer is to slow i can switch and calculate on this. Workstation 1 day ~23 hour in datacenter. but before I need good results..... I made the ground of the tunnel as Wall without turbulence model, are you agree with this?! And what converge tolerance can I use, to calculate this problem in 4 hours?! What are you working for Altair?! I hope they build a reference manual for AcuConsole and AcuSolve, because they have no theorey informations about the program, like Fluent. thx Last edited by Appleologe; April 18, 2013 at 11:00. 

August 10, 2015, 04:53 
height of boundary layer

#14 
New Member
Join Date: Jun 2015
Posts: 20
Rep Power: 4 
hi
i have a ducted propeller model with 0.3m diameter. i work with cfx and icem for meshing. i set my first Boundary Layer height at 0.0005m with ratio 1.2 and 5 layer. but i don't know that how calculate Yplus and estimate boundary layer height. help me please 

August 17, 2015, 02:36 

#15 
Member
Colinda
Join Date: May 2012
Posts: 73
Rep Power: 7 
Dear Sohrabmajd,
You can use linearised Blasius equation to compute Yplus. The link as given earlier in this topic is useful as well: http://www.cfdonline.com/Tools/yplus.php Also in the post of April 11 2013 of this same topic you find an estimation of the boundary layer height. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Radiation interface  hinca  CFX  15  January 26, 2014 18:11 
A question on "Specifying Boundary Layer Deformation Smoothing"  didiean  FLUENT  2  January 16, 2012 22:39 
RPM in Wind Turbine  Pankaj  CFX  9  November 23, 2009 05:05 
New topic on same subject  Flow around race car  Tudor Miron  CFX  15  April 2, 2004 06:18 
Boundary Layer thickness calculation in External f  Narsimloo  Siemens  0  January 2, 2001 01:41 