PLEASE READ... THIS IS LENGTHY BUT I NEED YOUR HELP.....

I'm working on modeling of Confined Impinging Jet Heat Transfer on a flat plate with nonlinear k-e model.

I have started to write my own CFD code for solving Confined Impinging Jet. For the biginning I used high reynolds standard k-e model. One of the resources that I'm using for confirming the accurance of my results is a paper from Chuang and Wei ("Computations for a Jet Impinging Obliquely on a Flat Surface", 1991, Int. J. Num. Meth. in Fluids, VOl. 12, pp 637-653). in this paper, authors have got a length of X=4W (W: width of jet nozzle) downstream of the jet nozzle as their computation domain and have obtained some graphs like pressure distribution on Impinged wall and symmetry axis and also contour plots for pressure, TKE, KEnergy dissipation, ...

The first thing that has made me confused is that; it doesn't seem that in X=4W the flow be fully developed and it can't be considered as a right Outlet region for computation domain. According to Heyerichs and Pollard paper ("Heat Transfer in Separated and Impinging Turbulent Flows", 1996, Int. J. Heat Mass Transfer, Vol. 39, No. 12, pp 2385-2400) this Outlet for computation domain must be considered at X=49W which in my code I considered this distance.

Anyway, in my code results, the graph for normalized pressure distribution on Impinged wall vs. normalized distance, starts from 1 in X/W=0 and falls to negative values in about X/W=1 and again goes up to zero and parallel to x-axis in X/W=10. Even with a Wilcox k-w model I got almost same results which are different from the Chuang results which normalized pressure approaches zero and parallel to x-axis in X/W=2.

This problem is conserved in other graphs and also contours. For contour plots, my results upto X=4W are almost similar to Chuang results, but in upper than X=4W which is not considered in Chuang Computation, extreme changes in all quantities upto X=20W can be seen which I think it must be considered in any computations for Impinging Jet.

The strange thing is that NONE of the papers that I have found, computed the domain upper than X=10W !!!!

So I can't still trust my CFD Code. Would you please help me about the proper regions for Outlet that should be considered and other points that I mentioned above for graphs and also contours.

Please tell me what the problem can be. I really appreciate any help in following:

1- Any Contour plots or Graphs of Impinging Jet that you may have

or in Internet sites can be followed.

2- Any papers regarding this matter that you may have find useful

for this matter and if it is available in Internet.

3- Do the results for a confined CIRCULAR-Jet are different of

results for a confined SLOT-Jet?

4- ...

Thank you in advance Amir

If you have a "confined" flow problem, then your problem specifiction is limited to the confinement - i.e., you can't arbitrarily extend out your domain. However, if you have an open air case, then you can/should extend the computational domain as far as possible until you reach a physical boundary condition that you can apply to your problem with good confidence. Obviously, if the flow at a point is not fully developed, for example, and you apply the f.d. b.c. you are solving the wrong problem.

1- Do not fall in the trap of many researchers who believe that the printed word is _the_ word. If by extending the computational domain you are getting different results, you may have actually discovered something worth publishing. However, in order for you to be confident I would strongly recommend that you try to "duplicate" the conditions of the papers that you are having problems with. That is, use the same "confinement" length and b.c. and see if you can reproduce the paper results. (If you can't, then you may have a problem with your code, or you may not! May be the person who wrote the paper has a bug in their code! Years ago when I was doing my masters, when I would take a paper to my advisor to discuss their findings, the first thing he would do was to check the names to see if the paper is written by someone with a serious track record. If the author was unknown, he would be extra careful with the results, and if known he would feel just a bit easier!)

So basically I'm recommending that you continue your own "research" and by process of elimination try to figure out what the sources of these discrepancies are.

2- Circular jet flow _is_ different from a slotted jet flow. The former is 3D (axisymmetric) and the latter is 2D. You can very this by checking any standard book on boundary layers - for example, Schlichting.

Adrin Gharakhani

Thank you Adrin for your concern and your reply. What I meant about computational domain is the distance from the centerline of the nozzle which should be considered as outlet boundary which abviously shouldn't be any selective distance.

As I wrote before I used X=49W. I have got same results all the times. But only problem is that I have to compare my results with some resources but most of them, like Chuang paper, have their outlet in X < 10W which from my results in this region (X=10W) the flow is not still fully developed.

I have also tried using the same "confinement" length and b.c. but I didn't get the paper results. Which again I inerprete the reason for this unsuccess, not-fully developed condition in X<10W.

I didn't understand what you mean of elimination process. Would you please explain me more.

Thank you for your help and your more upcoming helps. Amir

> As I wrote before I used X=49W. I have got same results all the times.

Obviously, if you are running the same problem you will get the same result unless your solution strategy includes random number generation, which I'm sure it doesn't!

>But only problem is that I have to compare my results with some resources but most of them, like Chuang paper, have their outlet in X < 10W which from my results in this region (X=10W) the flow is not still fully developed.

This really isn't a problem. If your code is bug-free and the solution methodology is proven (and if the same is true of the paper you are trying to compare your results with) then you should get the same results irrespective of the validity of the B.C. If you apply the same B.C.'s to the same computational domain then you should get the same result (giving room of course to differences in the accuracy of the numerical techniques involved). Period.

>I have also tried using the same "confinement" length and b.c. but I didn't get the paper results. Which again I inerprete the reason for this unsuccess, not-fully developed condition in X<10W.

Not a correct interpretation. See my explanation above. If you are truly solving the same problem then you should get the same result. I have to stress, however, that you have to consider the accuracy, stability and convergence rates of your technique and the paper's. If they are vastly different, then you shouldn't expect a good comparison. Be warned though that a higher order technique applied with a physically incorrect B.C. may not give a better answer than a lower order technique (and indeed the reverse may be true)

By process of elimination I'm recommending that you play around with different parameters and look for trends that may lead you to a possible source of error - if there isn't any then you should accept your solution to be correct.

Assuming that everything is OK with your code, I would tend to believe your results more (if there is a proof of solution convergence) since the larger computational domain should be physically more correct.

Adrin Gharakhani

(1). I am interested in knowing your problem and the mesh. (2). I think, for the confined jet impingment problem, you have two parallel walls with exit at x=49w, and a jet from one wall (width= w) located at x=0. How big is your computational domain? I mean (49w) x (spacing between two walls=?w).(3). could you tell me your mesh size and arrangement? (something like 4000 points ?) Could you tell me the meshes other authers used before and your meshes used in your calculations? I think, these are interesting information.

Hello John;

As you wrote, for confined Impinging Jet there are two parallel walls (walls gap=H) that jet is in one of the walls (jet width=W) emerging perpendicularly to the other wall.(axis of jet is y-axis and at x=0) Flow exits from 2 sides through the outlet boundaries at x=L (from axis of jet). But for computation, because of symmetric shape of geometry, just half of this domain can be solved.

In Chuang's paper:H=2W, L=4W. grids that have used (LxH): (1)64x46 (2)64x68. Reynold number=20000

In Pollard paper : H=2.6W, L=49W. grids (LxH): 92x30. Reynold number=10000

I have used these grids1)50x30 (2)100x60 (3)70x50 I've chosen width of W=0.1 for the jet and spacing between two walls is H=2W and outlet boundary at L=49W.(from axis of jet)

MY MESH: x-direction: 10 uniform grids upto x=W/2 (because of symmetry) and then non-uniform grids, expanding with a stretching factor of 1.05 to 1.2 So first 10 grids are in jet entrance (half of W which is in comp. domain)

y-direction: uniform grid

I wish I've not missed anything.

Hello Adrin;

Following to your good explanation;

(1) Can you suggest me what parameters are better to be checked in the Impinging Jet case, for comparing the results. for instance Cf, Cp, pressure, velocity, viscousity or KE distribution on Impinged wall or symmetry axis. In fact, it depends on the information that we have from the paper but some of them may be more effective than others in case of having several information from paper.

(2) Same question as above for applying the process of elimination and finding the possible source of error.

(3) I'm not so sure about the expression of Production term P (or G) and also source terms of U and V that should be used in wall boundaries and symmetry axis. For example is it only P=Tauw.Up/Yp for Ptoduction term or some of the terms of Production that use for internal grids are also included?

(1).Very good. You are the only one who can state your problem clearly. (2). For the 100 x 60 mesh, you have 60 points distributed across the channel (H=2W). You should stretch the mesh in y direction on both walls in such a way that it satisfies the first Y+ point requirement for the turbulence models selected. For low Reynolds number model, Y+ should be =< 1.0. For standard two-equation model with wall function, Y+ >= 100 ~ 200. For two-equation, two-layer model, Y+ =< 5. These are just ballpark numbers, so you should try a few variations. (3). Since the jet also has two walls ( only one is included in the simulation because of symmetry), you need to distribute the mesh in the same way. You could rotate the upper wall mesh 90 degrees to cover the jet exit area. After that, flip the mesh inside the jet along the jet wall to give you the mesh downstream the jet wall. After that point, you can smoothly stretch the mesh to the channel exit. (4). So, you are likely to have 20 mesh points stretched from the symmetry plane to the jet wall. And another 20 points stretched in the same way from the jet wall in the x-direction for the same distance (W/2). (5). At this point, you must determine the jet exit velocity profile. It is important to fix this condition. It depends on the flow configuration before the jet exit, whether the boundary layer is thin, or fully developed, or somewhere in between. (6). You can not compare two results with different inlet conditions. Regardless of what you do, you have to define the jet profile clearly. It is a good idea to extend the jet wall one jet width above the jet exit and specify the condition there to avoid the problem around the corner. (7). Looks like that it is a good idea to put 60 x 60 mesh inside the region of 2W x 2W near field region. (8). In other words, you should try to resolve the near field with fine mesh first.

I can't give you specific sugggestions because I can't claim to be an expert on jets. Anyway the process of looking for clues of convergence or bugs, etc. is usually independent of the flow physics.

But let me recommend, when comparing results try to avoid others' mistake of comparing integral quantities (like Cp, Cd, etc.) to claim victory (in case of a match). I can give you two totally different profiles that give the same integral values. So, if the integral quantities don't match you have a problem (maybe), but if they do match, my comment is so what!

As for checking your results with your own (looking for bugs, convergence, etc.) you should look at the variables that you solve for at every point and try to look for anamolies. I really can't help you in this direction - that is your job, every case/problem is different/unique.

Sorry I can't be of much help

Adrin Gharakhani

The gap between the two walls appears to be quite small. I would expect that the jet will experience a very strong curvature, depending on the momentum of the impinging jet. This has direct consequence on your choice of gridding.

First, I agree with John Chien that you need to resolve the near field as accurately as possible. Because you have large curvatures you are going to have large gradients and if the flow is not resolved well you are going to have high numerical diffusion.

But let me suggest that by blindly concentrating grids here and there you are not "guaranteeing" a better solution. For example if the inlet jet profile is uniform I don't see why you'd need 10 grid points near the axis of symmetry. When you tell me that you have doubled your grids you are not telling me anything about how much closer you are to convergence, because you could be wasting resources on the wrong sub-domains. So, what to do?

I would look at the vorticity field at a particular grid resolution and for refinement purposes I would concentrate my grids in regions with high vorticity (that is basically the outer boundary of the jet). So start spending your computational resources in regions with the highest vorticity on down. Basically, do manually what adaptive gridding would do for you.

Adrin Gharakhani

(1). Good suggestions! (2).It is not my intention to enter into the discussions, because I am really very busy. (3). The vorticity will be coming from the jet velocity profile itself. (4). If one is using the law of the wall, he is going to have uncertainty about how the jet boundary layer meets with the recirculating flow on the upper wall, because on both walls there are gaps next to the wall. (4). When these two stream meet at the corner, a jet is formed which will have a new shear layer with high velocity gradient. So, if you don't have fine meshes on both sides of this shear layer, the jet is not going to be captured properly. (5). Except for the fully developed flow at the jet exit, one is likely to have potential core flow region surrounded by the turning shear layer,which also form the boundary for the separation bubble. This convection and diffusion of the shear layer ( or vorticity) will determine the near flow field until the end of the separation bubble. At that point, the non-equilibrium boundary layers on the walls will take over the development of the channel flow. (6). The channel flow development downstream of the separation bubble is basically of parabolic type, that is the information basically propagates in the downstream direction. So, just like the boundary layer calculation, one can stop at any location. There is no need to place the exit boundary condition at the place where the flow will reach the fully-developed profile. (7). To solve the problem properly, in view of the existence of the large separation bubble next to the jet, the use of a low Reynolds number model is recommanded. (8). This is not a simple problem. You do have a strong confined turbulent flow separation. In addition, there is a high gradient 2-D shear layer to capture. (9). It is a good idea to look at the wall skin friction and heat transfer coefficient distributions, in addition to the wall pressure. Plotting the skin friction coefficient distribution in terms of the mesh density and arrangement will easily convince you the degree of difficulty of this problem. Most people run into difficulties not because of the code but because they don't have fluid dynamics background of these problems. (10). Sorry to interrupt your discussions. "The only way to solve a fluid dynamic problem is to learn more about the fluid dynamics part of the problem."