# [ANSYS Meshing] Setting up first layer distance to meet Y+ value for CFD analysis

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

 December 3, 2012, 00:54 Setting up first layer distance to meet Y+ value for CFD analysis #1 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 9 Sponsored Links Hi all, I'm working on axial flow pump. Need to meet desired y+ value near the blade walls to capture the boundary layer effects precisely. I have used y+ calculator to find the 'y' distance from the wall. I ran a simulation and i found the y+ value is 40. I use ANSYS Meshing. I have used inflation to generate prism cells near the blade wall. How do i setup first wall distance from the blade if i use "Total thickness" inflation option. Am i supposed to use "First layer thickness" to establish such a small distance as first layer? Appreciate your help and suggestions.

 December 3, 2012, 02:22 #2 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,331 Blog Entries: 6 Rep Power: 45 Where you have got the Y+ = 40? What about the suction and pressure side Y+ values? The Y+ formula you are using is derived for the flat plate and zero pressure gradient. So you must expect the deviation from the values you get from this law. Keep in mind that Y+ calculator gives you a smart starting guess and not the final values . Moreover you have the varying values of Y+ along the wall surface. Can you show us the maximum, minimum and average Y+

 December 3, 2012, 02:49 #3 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 9 Hi Far, Thanks for your quick response. Though we have y+ estimation/calculation for a flat plate, they could still be used if i'm right with some deviation. I'm not sure about the inlet pressure conditions. So i run it with Total pressure being 0 Pa at the inlet and Mass flow rate being 0.22 kg/s at the outlet. Reference pressure is set to 1 atm. From physical testing, i found that the pump delivers 13.3 lpm at a pressure head/rise of 100 mBar. I wanted to simulate this case and validate our pump specifications. I would like to setup the problem using Single Reference Frame. Water at 80 C is the fluid. Impeller (solid volume) had been subtracted from fluid domain so that i can have single fluid domain. Using named selection, i have applied rotating wall conditions with a speed of 500 RPM to the impeller. I don't get 'Counter rotating wall' in CFX for some reasons. Guess i'm missing something. Once a case is validated, then i can run series of simulations to plot the performance curve of pump at different rotational speeds. Strange thing is that y+ value calculation from emprical relations actually vary from readily available calculators. I used skin friction formulae to calculate wall shear and then used friction velocity to calculate 'Y' distance with a predefined Y+ =2. Thanks in advance.

 December 3, 2012, 12:30 #4 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 I usually just run the mesh with the prism default settings. You will see that where you have areas of curvature, it should give you finer mesh which leads to thinner prism layers as the default tries to match the last prism volume with the adjacent tetra. This improves convergence, etc. Then I run the solution and check the y-plus after the fact. I also check to make sure that the boundary layer region stays within the inflation layer. If it looks like I need to adjust, I can always go back, make a change and try again. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 December 4, 2012, 01:20 #5 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 9 That's true Simon. But how can we make sure that our boundary layer lies within inflation ?

 December 4, 2012, 13:42 #6 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 I usually try it and it usually works... __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 December 4, 2012, 14:34 #7 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,331 Blog Entries: 6 Rep Power: 45 Calculate the total boundary layer thickness from the flat plate formulae. Make the inflation 10% more thick than the total boundary layer thickness from the flat plate formula. Keep in mind that the boundary layer is thin at the leading edge and will become thicker towards the trailing edge. Put atleast 10-15 points within boundary layer for proper resolution.

December 4, 2012, 15:11
#8
Retired from CFD Online

Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
Quote:
 the boundary layer is thin at the leading edge and will become thicker towards the trailing edge
Is why I usually just tell people to try it and see. The mesher will automatically give you prisms that transition nicely to the volume. I have seen too many new users trying to apply that flat plate Y+ to their models and in the process they mess up what would have been a perfectly good boundary layer. They end up controlling the initial height, ratio and number of layers, which forces the total height to be uniform along the surface. It also means that the transition between the last prism and first tetra is poor, which can lead to discontinuities, poor convergence, etc.

If they skip the Y+ calculation (which is rarely applicable to their real life model anyway) and just trust the mesher, they will have an easier time generating the mesh. They can get to the solver and run it. In post processing, if they see that the boundary layer has not fully formed by about 80% of the way out of the inflation layer, they can go back and mesh again with a larger number of layers. If it forms completely in the bottom 40%, it just means they wasted time generating too many layers and should probably settle for fewer on the next equivalent model.

Of course, trusting the mesher to set the prism heights assumes you set the size function correctly to begin with. For that you need some experience, trial and error, a look at how someone else set sizes for a similar example or a refinement study to be really sure.

I did agree that 10 to 15 layers is probably a good place to start.
__________________
-----------------------------------------

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

 December 4, 2012, 15:14 #9 Retired from CFD Online     Simon Pereira Join Date: Mar 2009 Location: Ann Arbor, MI Posts: 2,665 Blog Entries: 1 Rep Power: 39 Perhaps a good compromise would be to run the Y+ calculation, but still set the prisms up with default floating initial and total heights. Set 10 to 15 layers. Generate the mesh. Then check the mesh to see if it is close to the Y+ you were looking for. If the initial height of the mesh is close, head to the solver. If the initial height of the mesh is much too coarse, then your surface mesh was too coarse. Adjust the mesh parameters for the surface mesh and run prism again with the same settings. If the initial height of the mesh is too fine, then perhaps you will be wasting time in your solver. You can decide if it is worth going back and adjusting the mesh parameters for a coarser mesh. __________________ ----------------------------------------- Please help guide development at ANSYS by filling in these surveys Public ANSYS ICEM CFD Users Survey This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)... CFD Online Users Survey

 September 11, 2013, 08:00 #10 New Member   Join Date: Dec 2012 Posts: 13 Rep Power: 6 Hello, I am modelling a turbine and I am dealing with the Y+ issues you have discussed. However, you mentioned something about the height of the boundary layer being within the thickness of the inflation layers. How can I check for that? Through Fluent or through calculations that I do? On another note you said to leave things as default. Then when should I specify the thickness of the first inflation layer? What is the importance played by the first inflation layers? Many thanks

 November 21, 2014, 06:01 y+ URGENT!!!!!!!!!!!!!! #11 New Member   Shravan Join Date: Sep 2014 Posts: 4 Rep Power: 4 how to know the present y+ distance in our analysis?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post kasimirXV OpenFOAM Native Meshers: snappyHexMesh and Others 10 May 10, 2016 23:04 hamed.majeed CFX 14 February 4, 2015 08:07 EVBUCF OpenFOAM Native Meshers: snappyHexMesh and Others 14 August 20, 2012 04:31 perdita FLUENT 0 November 23, 2010 10:15 Mujahid S. Suhaeb Main CFD Forum 8 December 1, 1999 18:14