Hello,

I have a problem with y plus in my calculation. I would like to calculate a compressor with heat transfer. For the most part of the heat transfer is in the viscous sublayer so the y plus must be about 1. But the velocity is in the flow field of a compressor very large so the first cell of the boundary layer mesh is very thin (about 0,01-0,0001mm). To the thin cells very small tetra elements are connected evidently so the finish element number becomes too high ( 10-12million). If I increase the size of tetra element so this operation results too large difference between size of the tetra and prism elements what can cause some numerical errors. What can I do in this situation? Thanks in advance!

Roland

You need to add more prism layers, until the prism layers have an aspect ratio of approximately one. This way the final layer should be roughly the same size as the bordering tets.

Hello Johnny,

Yes, I understand it but there are critical parts which have very small gaps (0,1-0,2mm) for example between the outside wall of the housing and the end of the blades. Your idea is really good but I can't apply in these small gaps unfortunately...

Hi,

Why do you say for heat transfer y+ must be around 1? This is not correct. Heat transfer can be modelled with normal wall functions (ie y+>11) as well. Have you tried the standard wall function approach in your application?

Glenn Horrocks

Hi Glenn,

I calculated a 3D tube before my compressor simulation. In tube compressible air flows , the SST turbulence model and the automatic wall function were used. Re=40000, this is low Re number so the y plus must be 1. I studied the wall heat transfer coefficient (at the wall) in case of y plus 1 and y plus 5. If y plus=5 => wall heat transfer coeff. = 90 W/m2*K. If y plus=1 => w.h.t.c = 480 W/m2*K. I conclude from these results that I must divide the viscous sublayer thoroughly anyway. Although there is high Re number in the flow field of the centrifugal compressor, the heat transfer is in the viscous sublayer in this case too, therefore I think, that y plus must be 1. Please, help me, if my conception is not correct.

Thanks Roland

For k-omega models with wall-modeling, the recommended y+ range is 30<y+<300, where closer to 30 generally leads to the best results. Y+=5 might not be large enough to trigger the employment of wall functions, leading to a poorly resolved boundary layer.

Run the same pipe flow simulation for an even coarser boundary layer mesh and see if your solution improves.

But what means that the y+ range 30? 0-30? or 30-300? And what is the recommented y+ range for the Reynolds stress turb. models? I would like to calculate later with these because I rode that the R.S. turb model is the best solution for highly swirling flows and strong curved streamlines...

Sorry, i meant to type 30<y+<300. So using wall functions, you shouldn't have an y+ smaller than ~30. Close to 30 is recommended.

RSM models are indeed necessary when you are dealing with highly swirling flows (anisotropic turbulence in general), but they come with a package of associated problems (convergence, stability, incorrect separation prediction). The y+ criteria are the same (ie. depending on wall-treatment approach), but you need to take special care in creating a mesh as these models are very sensitive to element-quality.

ehm, some kind of bug alters my input 30 < "y+" < 300 displays as 30<300 when I type it without the quotes.

test 30<y+<300

Thank, I understand you. The mesh quality is not too high because the geometry is fairly complicated so I can create only tetra mesh. It is practical perhabs if I calculate with SST rather...

Glenn, by using the standard wall function , you are not close enough to the wal hence we don`t tend get capture wall heat transfer coefficient, So using Wall function under a case where one is looking to capture the temperature distribution at the wall , we can lead to big errors .

Sorry Pratik but you are completely wrong. You can model heat transfer accurately with a wall function approach. Have a look in the documentation.

Whether this approach is valid or not in the exact application depends on what you are trying to do. In general if the wall function approach is valid for the momentum equations then it will be valid for the heat transfer equation too.

Glenn Horrocks

Glan,

Consequently the viscous sublayer must be divided (in the case of the heat transfer too) only then, if the Re number is low? (in the case of laminar flow?)

Hi Roland,

Sorry I don't understand your comment. If I have misunderstood you in my answer below please restate the question.

Wall functions mean you don't need to model the viscous sublayer as it is empirically included in the wall function approach. This applies to both the momentum and energy equations (and also scalars too if they are present).

Wall functions do not work well at low Re so in this case it would not be a good approach and you should consider integration to the wall. There are a number of other applications when wall functions are not appropriate, they include turbulence transition modelling, large separations. Wall functions are based around simple flow over a flat plate so it is all about how close that is to your modelled situation.

If the flow is laminar then there is no turbulence and therefore no wall functions, y+ or anything like that. Your only approach is to integrate to the wall and do a mesh sensitivity study to check your mesh is OK.

Glenn Horrocks

Hi Glenn,

Then you mean to say that the heat transfer coefficient using wall function ( having Yplus value above 10 ) is same as when one use enhance wall treatment( Yplus < 5). I think the later case is more accurate for heat transfer problems

Kindly explain if you do not agree , thanks for your inputs

Hi,

General statements about one approach being better than the other are too simplistic. If the wall function approach is applicable then using wall functions for heat transfer (with y+>11) is likely to be accurate. If the wall function approach is not applicable then integrating to the wall is likely to be more accurate.

Glenn Horrocks

Hi Glenn,thanks for your inputs.

As far as the user is concerned, for undertanding the applicability and the accuracy of the wall function, which I think that this issue is too problem dependent. So using a good wall meshing strategy for resolving the boundary layer is always going to be accurate than wall function approach.Can you please sharing your experience on where you tried to resolve the boundary layer and still could not reach a good agreement / conclusions/ convergence .

As far as my exp is that more you try to resolve the boundary layer more unstable the solution gets and takes more time for convergence. This can be due to following two reasons

Reason 1

here can be either that the mesh is havin a very big expansion factor or high aspect ratio , in general a very bad mesh quality near the wall .

Reason 2

it is the inherent difficiulty of the Near wall approach to produce an accurate solution from that particular solver, ( what level of accuarcy are you looking for here )

Are you pointing towards my second reason ,that makes you use wall function approach and lead a simple life .

And as far as CFX solver or fluent is concerned, they have very good models for the near wall treatment, and works well with Komega model(SST).

I would like to know your feedback for the above

Best Regards