Dear all,

Using Fluent 5.3, I am doing a simulation of ventilation in a 2D room(Width x Height=9m x 3m). The turbulence model is standard k-e with conventional wall function. In the Fluent User Manual(P9-59), it is said that " A Yplus value close to lower bound (Yplus~30) is most desirable". But when I want to check the Yplus value by creating a ISO surface of first grid plane(a line in my case, say Y=0.08m) and then use X-Y plot(X--room width, Y--Yplus), I always get zero value on all the grid points, while on the Yplus contour display, by right click on the near wall layer(first grid layer), I can see from the FLUENT console window that my first mesh girds are mainly between 30~60(the Yplus value at some grid points are less than 30 but I cannot get all of them between 30~60). Can anyone tell me where have I done wrong? If the Yplus values at some points are out of the lower or upper bound, is it OK? Thank you very much in advance.

SP

If your Y+ values are around 30 to 60 then I would say that your ok. I don't know why you can't plot the Y+ values on an XY plot though.

You can refine the mesh if the values of Y+ are a lot greater than 60 if you think its a really big deal. It's quite easy in fluent to do so. i.e. from the main menu choose:

adapt, Y+/Y*, then set your min/max Y+ values, adapt

and the mesh is refined. You then need to start the solution again.

cheers

at

Hi Thomson,

Thank you very much for your kind help. One more question: if I got my Yplus between 30~60, is it still necessary to test mesh dependance by refining the mesh(if I refine it the Yplus will be out of 30~60)? Because in Fluent User Manual it is said "using a excessive fine mesh near walls should be avoided because the wall functions cease to be valid in the viscous sublayer."(PP. 9-58) As a test, I have used a very fine mesh in the near wall regions and I got a flow pattern much like that of a laminar flow(i.e., much like that when specifying the flow is laminar although the Re based on the inlet height is about 5000!). Anyone has any idea about this and my X-Y plot problem? Much thanx in advance!

Cheers!

SP

It is important to keep the first node from the wall outside the laminar sub-layer region in the boundary layer. The wall functions were developed to avoid the need to do this.

If 30 < Y+ < 60 in my model I would tend to say that was ok unless I had data to compare it (i.e. skin friction heat transfer) with and if there was a significant difference then I would go for a low re turbulence model.

Just a thought about your XY plot are you trying to plot cell or vertex data. You cannot plot Y+ as node values

Allan

Hi Allan,

Thank you again for your quick response. Yes, the X-Y plot is a plot of vertex data because Fluent doesn't allow a X-Y plot of node data. I just wonder why I get the zero plot while on the Yplus contour they are non-zero? Where have I done wrong?

I adapted the mesh as you have said, the result is not very much different to that of the previous result, so I should say it's a mesh independent result? Anyway it's impossible to get all the Yplus at the first grid points near wall between 30~60, so it's okay?

Best regards,

Shengping

y+ should be between 30 and 300. y+ too small is wrong and often causes convergence-problems. Try xy-plot, nodal-values off. chris

About y* or y+ availability ============================== Although FLUENT does not provide y+ or y* as "field" variables (i.e., y+ and y* stored in FLUENT are those only at wall-adjacent cells), you can use the "custom field function" capability in FLUENT to define, at least, y* (= u*y/nu, where u* = C_mu**0.25 k**0.5) as a field variable. To do that, you need y, the wall distance. If you turn on the two-layer zonal model (or RSM model) temporarily, you will have access to the "cell wall distance" variable under "grid". Use it as the wall distance to define y*. You can then plot, display, or contour y* distribution in the whole domain.

y+ is a lot harder to compute than y*, because it is not a pointwise field function anymore as y* conveniently was. Computing y+ in the field needs the wall shear stress or friction velocity. Making available the wall shear at every interior computational cell is quite an overhead most commercial CFD vendors, including Fluent Inc., wish to avoid for competitive reasons.

Valid y+ range ================= The log region is generally known to range from 30 or so (some text books quote 50, 60) to a few hundreds in near-equilibrium, wall-bounded flows. The lower and the upper bounds of the log-layer depend upon the Reynolds number, pressure gradients, among others. As we go toward the upper bound, the so-called wake component (departure from the log profile) becomes significant. In strongly non-equilibrium flows (e.g., boundary layer flows under strong adverse pressure gradient), the width of the log region becomes smaller or even vanishes altogether (separated flows). For that reason, we recommend in our User's Guide the y+ at wall-adjacent cells had better be closer to the lower leg of the log region. By putting the first grid point toward the lower leg of the log region, we have a higher chance of hitting the log layer. And another premium is that the resulting mesh will better resolve the boundary layer which is critically important for successful prediction of wall-bounded turbulent flows.

Having said that, I know you don't have the luxuary of getting anywhere close to y+ = 30 or even 100 in many high-Re flows. As a rule of thumb, y+ = 1 corresponds to a physical wall distance of 10/Re_L. For the flow around ships, for instance, Re_L is order of 10**9. You probably should be content with y+ = 1000, which translates into 0.00001*L, quite a small distance. Resolving down to y+=30 or so would require an extremely fine mesh near the all. One fortunate thing, though, is that the upper bound of the log layer becomes moves outward (larger y+) as the Reynolds number increases.

Dear Chris and Dr. Kim,

Thank you for your postings. I still have some questions about Y+ and Y*, could you explain it a little more further, Dr. Kim?

In Fluent User Manual, Page 9-49, after defining U* and y*, it is said:" The logarithmic law for mean velocity is known to be valid for y*>30~60. In FLUNET, the log-law is employed when y*>11.225. ... It should be noted that, in FLUENT, the law-of-the-wall for mean velocity and temperature are based on the wall unit, y*, rather than Y+. (!!!) These quantities are approximately equal in equilibrum turbulent boundary layers."

But then, on Page 9-58, you said: "It is known that the log-law is valid for Y+>30~60. ... A Y+ value close to the lower bound (Y+~30)is most desirable".

So what I should use as a criterion: Y* or Y+? Although you said "Note that Y+ and Y* have comparable values when the first cell is placed in the log-layer."(PP9-58), I must first decide whether my first cell is placed in the log-layer with one of the above two Ys!! And you said that in Fluent the log-law is based on Y*, not Y+, but after that in the guidelines(9.8) you always use Y+ as the criterion, what should I use?

On the other hand, in my project, the flow is ventilation in rooms, the Re is about 5000 based on the inlet wall jet height(U~0.5m/s). The problem is not that I cannot make all the Y+ below 60, but that I cannot make all of them above 30! If I want to make all of them above 30(say by mesh adaption with Y+ or Y*), I get only two mesh points in the spanwise of the jet, it's not a good resolution, yes? What should I do? Thank you all for your feedbacks in advance.

Regards,

Shengping

If you have no problem to resolve the walls well then why don't you use a low-Re model or a two-layer model with y+<1 everywhere? Then you don't need to worry about resolving some walls too well.

Hi Jonas,

The problem is: one of my friend developed a inhouse code for the calculation of ventilation in rooms, he utilises the standard K-e model with standard wall function, we want to compare the results with different codes. But I cannot get all the Y+ above 30, otherwise I should use a very croase grid near wall, it's evidently not appropriate. Is it not appropriate that I insist on using standard k-e model with standard wall function approach for this problem? In addition, when working with wall function, I should use Y+(=30~60) or Y*(=30~60) as criterion for the first mesh point?

Best regards,

Shengping

Y+ is most appropriate, but it shouldn't make much difference, Y+ and Y* should be fairly equal in the near-wall region where you are looking - if they are very different you have problems and then you can not expect the wall-laws to work well! Fluent, as Sung-Eun said, uses Y* just because it is more expensive to compute Y+.

Thank you, Jonas!

I can hardly make Y+ and Y* comparable, that means that it's not appropriate to use the wall function approach? Really the flow in my problem is too slow. Regards!

My apology for the confusion. Let me see if I clarify:

o FLUENT codes (both FLUENT 4.5 and FLUENT 5) does not use y+ (u_tau y/nu) at all for any purpose whatsoever, except the postprocessing (y+ at wall adjacent cells).

o FLUENT User's Guide refers to y+ only because most of the near-wall data and correlations have been catalogued in terms of y+, and because y+ is still the most widely used wall unit in the modeling community.

o The demarcation of the whole inner layer into "linear" (laminar) layer and the log-lauer with y* = 11.225 as a cut-off is a pure numerical artifact and is adopted in FLUENT (and many other commercail codes) solely for implementation's sake, i.e., a provision to prevent anomalous results when Y*. In reality, there is no such sharp division. There's always a buffer layer.

o The difference between y* and y+ is that y* adopts u* = sqrt(sqrt(C_mu)*k) as turbulent velocity scale, whereas y+ uses u_tau(= sqrt(tau_w/rho)) as turbulent velocity scale. y* recovers y+ in the log region of equilibrium boundary layers and fully developed pipe/ducts flows, where u*/u_tau tends toward 1.0 (This is the definition of equilibrium layer!). In the viscosity-dominated near-wall region, say y+ = 1.0, u*/u_tau is much smaller than 1.0 and consequently y* will be much smaller than y+, inasmuch as the turbulent kinetic energy is typically very small (correlation data show k/u_tau**2 = 0.05 y+**2).

o You might wonder then why FLUENT uses y*, not y+, causing troubles and confusing people who are get used to the universal law of the wall. The reason is that the y* based law of the wall performs sigificantly better than the universal law of the wall, expecially for non-equilibrium flows (strong pressure gradients, separated flows, rapidly changing wall-bounded flows with strong streamline curvature, etc.). One quick example. Consider a backward facing step where the upstream cold flow reattaches to the bottom wall being heated. You would expect that the heat transfer will be maximum at or near the reattachment point where the cold flow first hits the hot wall. If you use u_tau as turbulent velocity scale and use the temperature law of the wall based on u_tau frequently shown in the textbokks, you end up predicting a "minimum", instead of maximum) heat trnasfer coefficient at "reattachment" point.

For your room flows, I suggest you use one of the low-Re k-epsilon models offered in FLUENT 5. You can activate the low-Re model using the "define/models/viscous/low-re" and "define/models/viscous/ low-re-ke-index" text commands. The model indices are;

Abid(0), Lam-Bremhorst(1), Launder and Sharma (2), Yang & Shih (3), Abe-Kondo-nagano(4), Chang-Hsieh-Chen(5).

You can use two layer model. But I'm a bit concerned that your Reynolds number (I'm not quite sure what length scale is sued for the Reynolds number) seems to be very low and the whole domain is in Re_y<200. If it's the case, the two layer model redices to the one-equation model of Wofstein. I think you'd better model epsilon equation.

Dear Dr. Kim,

Thank you for your kind help. I will try your LRN models and two-layer model. Fortunately, I have some experimental data for this case, so I can compare the performance of different models. The Re I mentioned is based on the jet height, it's a 2D jet in a 2D room.

Best regards!

Shengping

(1). I like your questions. I think you are getting very close to the dark side of the wall function ( or the various implementation of it) and the turbulence modelling in general. (2). I will give you a couple of positive suggestions first. (3). First of all, you can run the flow-in-a-room problem from the low Reynolds number end. The other way to say is that run the problem as is with a constant viscosity model. Naturally, you can vary the viscosity level to simulate the flow. You really should do this first, and get a few Reynolds numbers computed. I would suggest that Re=100, Re=400, Re=1000, Re=5000, Re=10000 are good numbers to try. This is very important because it will establish the "clean" baseline solutions. Any code should at least pass this stage, and you don't worry about the Y+ or Y*. (4). The next thing you can do is that, since you are using a two-equation model, you want to make sure that the flow field is turbulent all the time, everywhere. This may not be the results you want, but this is the way the turbulence models are created. Assuming that the room size is fixed, assuming that the inlet and the mesh is also fixed, then there is one parameter you can change, that is the inlet velocity. So, what you should do is to make sure that the Reynolds number at the inlet is very high such that the turbulence model and the wall function you are using is guaranteed to work. You need to give the code a chance to get a solution within its range of validity. (5). For the high Reynolds number range, you can run Re=1.0E+07, Re=1.0E+06, Re=1.0E+05, so that the conditions required by the code are satisfied. You must be able to obtain at least one solution, otherwise, the code is useless. (6). At this point, you can look at the results in the overlapping range of Reynolds number to see how the solution behave, and don't worry about whether the wall function condition is satisfied everywhere. (7). After having said that, I'll give you some short comments about the use of the wall function. (8). The wall function was experimentally established for the velocity profile, especially in terms of the U+, Y+ etc. The detail is available in the Schlichting's book of The Boundary Layer. Other than the cases of adverse pressure gradient boundary layer flows, there is a rather large portion of the boundary layer profile belongs to the log-profile family. So, normally one does not have to be concerned with the outer limit of the Y+, as long as it is within 50 , 300. In this case, there is a factor of six in the cell size range, and it should not create any real difficulty as long as one has properly meshed the near-wall region. There is a safety factor of six in this case. (9). The use of the wall function for adverse pressure gradient cases or the general complex flow cases is not recommended. (10). First of all, the boundary layer separation problem creates the vanishing wall shear stress, and thus makes the wall function approach invalid. But this does not prevent the brave people from using it. One way to avoid this zero wall shear stress problem is to calculate the wall shear stress from the turbulence kinetic energy variable, k ( if it is being computed in the model, otherwise you can't compute it). Since k is always positive and non-zero, the derived wall shear stress is always positive and non-zero. Unfortunately, k is not a vector and it can not tell you the flow direction. So, the derived wall shear stress does not have a direction. (11). Is the wall shear stress really related to the near wall turbulence kinetic energy? The answer is a "limited yes". So, in the non-adverse pressure gradient cases or non-separating flow cases, one can use either the direct evaluation of the wall shear stress based on the near wall velocity, or the turbulence kinetic energy variable. The mehtod is still not valid for marching through the separating point into the reverse flow region. (12). But, in early days, researchers at the Imperial College realized that since they were promoting the use of the two-equation k-epsilon turbulence models, the k-variable is readily available to replace the near wall velocity for the calculation of the wall shear stress. And even though, it is not valid throulgh the flow separating point, the computed wall shear stress is always non-zero and thus avoid the singularity of the log-law-of-the-wall profile. At least now one can get a solution, regardless of whether it is valid or not. (13). In the heat transfer cases, it turned out that the heat transfer in the separating point region can be linked more closely to the turbulence kinetic energy behavior. And thus the use of k is preferred in this region. (if you are not using k as one of the variable, you will have to do something else.) (14). With the above two discoveries, the use of k and the related Y* is necessary in a general purpoose code, so that any general flow cases, with or without flow separation can be computed (does not mean that the solution will be right!) within the framework of the wall function approach. (15). That's why I call it the black art of turbulence modelling. Even though the solution is based on the invalid assumptions, at least you have a solution to begin with, so that you can argue the accuracy of the results. Hope this will provide some additional information about this difficult field of turbulence modelling.

Yea, you could say that, if Y+ and Y* are very different that probably means that your grid points are not in the inner log-layer (y+ ~ 30-200). It could also mean that you have a boundary layer that is very far from equilibrium. In any case, this indicates that wall-functions won't work well. Use a low-Re model instead that can be integrated down to the wall.

Dear Dr. Kim,

Thank you for your kind help. I will try your LRN models and two-layer model. Fortunately, I have some experimental data for this case, so I can compare the performance of different models. The Re I mentioned is based on the jet height, it's a 2D jet in a 2D room.

Best regards!

Shengping

Dear Dr. Chien,

Just want to tell you that I apreciate very much your nice suggestions and kind help, I will follow the steps you suggested to "probe" this problem to get some "feelings" about turbulence modeling, but I just have experimental data for Re=5000.

Regards,

Shengping

In order to solve your plotting problem, deselect the node values flag in the top left corner of the panel. I think that you may be trying to plot averaged y+ values which does not work and so plots everything on the 0 axis.

Hello Dr.Kim,

I too have a problem including a jet but a round one with a similar Re of about 5000 related to the nozzle diameter. The jet enters into a mixing duct where more than 75% of the domain lies within the zone Re-t<200 due to the entrained ambient air.

At the moment I am using the 2 layer approach at the wall together with the realizable-k-eps model which the User's Guide advises to use in the case of round jets.

My question is whether you can evaluate which error is worse the one depending on the "exorbitant" use of the 1-equation model or the one related to the use of a not "whole" appropriate low-Re-k-eps model.?

Thanks in advance

Volker