CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ANSYS Meshing] Setting up first layer distance to meet Y+ value for CFD analysis (

enr_venkat December 3, 2012 00:54

Setting up first layer distance to meet Y+ value for CFD analysis
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.

Far December 3, 2012 02:22

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+

enr_venkat December 3, 2012 02:49

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.

PSYMN December 3, 2012 12:30

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.

enr_venkat December 4, 2012 01:20

That's true Simon. But how can we make sure that our boundary layer lies within inflation ?

PSYMN December 4, 2012 13:42

I usually try it and it usually works...

Far December 4, 2012 14:34

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.

PSYMN December 4, 2012 15:11


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.

PSYMN December 4, 2012 15:14

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.

Elio September 11, 2013 08:00

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

shravansudden November 21, 2014 06:01

y+ URGENT!!!!!!!!!!!!!!
how to know the present y+ distance in our analysis?

All times are GMT -4. The time now is 01:33.