Hello I have a stupid question. How do you proceed to prove your model is not dependant of your grid? In my case I have an impinging jet on heated flate plate and each time I change my mesh (either I increase the number of cells when I keep the same grid or I build a new grid)my results change. I try to control the Y+ on the heated surface,but without result. Thanks for your help

Alexandre zza98ag@shef.ac.uk

I like your question because it is one of the core issue of CFD which has been around for over 20 years and will be so with us forever. I don't like to use the word "stupid" , but what you are donig is pretty close to that. I will answer your questions in a different way. (1). suppose your solution is everywhere constant, then you probably can use 3x3x3 mesh to get a good solution, (2). for the linear solution, the same 3x3x3 may be adequate to give you a good solution. (3) for the parabolic solution, you definitely would like to have a mesh bigger than 3x3x3. That is because you need at least 3 points to define a parabolic profile. (4). as your solution becomes more complex, you need higher order polynomial to represent the profile(solution), and that will define the minimum number of points necessary to retain the accuracy of the solution. (5) now you know that the minimum number of mesh points needed is a direct function of your solution complexity. (6) so, go back to your solution first, then study the solution profile to see if you can define your solution in a piece-wise continuous polynomial functions. In this way, you can put 3 points in the linear profile sections, and maybe 3 or 4 points in the parabolic sections,,and so forth. You can study in this way the complete profile of the law of the wall region. (7) in addition to the number of points needed, you also need to know the locations where these points must be placed in order to cover the right segment of the curve ( solution). (8) this is only the first step, after that, it's fairly straightforward . All you need to do is to put more points into each segment of the curve and check the change in the solution. Then you can plot skin friction ( or heat transfer ) coefficient at certain point against the mesh density ( total number of mesh points ). When this curve becomes flat , you have the converged solution which is independent of the mesh ( density and arrangement ). It is not difficult to do with today's computer capacity. ( except complex 3-D problems.) (9) Unfortunately, the computer is too small to handle 3-D problems in this way. So most of the time, the solution is a function of mesh, time, location, person, company, version,etc... (10) Currently, it is a common requirement to demonstrate the mesh independent solution before the paper can be accepted for publication. So you may want to review recent papers published in AIAA or ASME journals to get some feeling about how other researchers are doing in this area. (11) you can also use a simplified problem with known analytical or numerical solution to check out the minimum number of mesh points and its arrangement first, and then apply the result to your more complex 2-D or 3-D problems.The bottom line is you need to know your solution before you start your mesh generation. For complex 2-D, 3-D, or un-steady problem, you can only do it by try-and-error approach. (12). Getting a solution is not difficult, but finding the right answer is not easy. (100x100 is not uncommon for 2-D simple turbulent flow problem.)

Hi,

I hope that John does not make it a habit of calling people stupid on discussion forums. While some parts of it do make some sense, allow me to summarize a long and convoluted post:

"Refine your mesh until some paramater relevant to your problem no longer changes."

At this point you have enough, and you should have enough knowledge from the increasing levels of refinement to know what sort of accuracy is acceptable.

I had a couple of other comments about number 10 is John's post:

This is a ridiculous requirement. Basically ludicrous and obviously made up by someone who clearly does not understand that there are situations which arise in which there is no "converged" solution.

I think the AIAA also requires second order accuracy in space, which is also ridiculous. If you have a problem with shocks and so on, and you want monotone solutions, you cannot get better than first order in the region around the shock, i.e. Godunovs Theorem.

Therefore, publish in Journals which are smart enough to realize this, JCP, JFM, Physics of Fluids, and so on. Not in ASME, AIAA, whatever.

"Refine your mesh until some paramater relevant to your problem no longer changes."

Is a good approach. The net heat transfer coefficient may well reach grid independency before the htc profile does. It all goes back to want you want to get out of the cfd calculation.

Make sure your wall function/turbulence model allows for any number of cells in the boundary layer otherwise you may never reach independency.

Robin.

It is always smart to ask a question. Therefore, there is no such thing as a stupid question. But a decision to do something can be stupid, because a decision was made without asking a question. In other words, decision made without asking question is likely to be stupid. Only brave person knows how to ask a question after he has made a stupid decision. So much for the opening speach. Would you elaborate on why some wall function/turbulence models can only accept a finite number of points or cells in the boundary layer ,in your last statement ,Robin ?

On the item number 10, I think, as long as the method used is clearly stated and the validity and usefulness of the results are demonstrated, the paper should be accepted for publication. This is my personal opinion. Certain types of problem are not diffusion dominated or related. For FD formulation, it is relatively easy to extend the upwind difference over several nodal points. I am not sure that is the case for the FV formulation ( or even FE formulation ). Also with the mesh independent approach, the errors produced by different methods will become less important in the whole issue. I think the key issue is the usefulness of the final results or findings, not the issue of 1st or 2nd order method used. Second order accurate scheme does not necessarily equal to the more accurate results. It depends on the type of problem and on how it is implemented. Is a 3-D coarse mesh result using 2nd order method more accurate than a 3-D fine mesh result using 1st order method ? The basic requirement is that the solution should be repeatable. This is not the case for most 3-D results today, regardless of which method used.

I think the question must be 'How many wall function implementations allow for any number of cells in the wall boundary layer?' The have been some that only use the law of the wall in the first grid cell next to a wall and then standard eddy viscosity approaches in all further grid cells. This is fine for massive spaces (HVAC applications) where often only one grid cell can be afforded in the boundary layer, not so good for smaller scales. I admit the majority of approaches will look at local conditions near all wall cells then choose to employ the relevant algorithms, but not all .....

To cut to the chase ...... If you look at a turbulent flow over a surface mounted cuboidal obstruction there is a wealth of flow detail that exists in reality (wrapped horseshoe vortex, top and side seperation and (possible) reattachment, heat transfer at a turbulent stagnation point, etc.). To obtain a grid independent solution to resolve ALL of these details on a single obstruction would result in a model that is so weighty as to exile itself from any industrial environment.

If you look at a force cooled PCB with 20-30 components mounted on its surface from which cfd results are required to industrial accuracy levels and to industrial timescales, you quickly realise that a totally grid indepenedent solution is not going to be efficiently achieved.

So what then? Well, you can start to investigate the fact that the net heat transfer coefficient from a single obstruction is more dependent on the flow Reynolds number than on the exact prediction of surface profiles of htc. You can also start to question the accuracy of a theoretical grid independent k-e solution when applied to a case where only a fraction of the grid can be afforded around a single component. You can also start to relate innaccuracies of net htc predictions to known innaccuracies of power dissipations of components (i.e. power dissipations are often only known to within +/- 10 to 15% !).

Industrial cfd is a pragmatic affair. There are industries where an inaccuracy of more than 1% is intolerable. Then there are those insdustries where BCs are only known to within 15%. What then happens to academic cfd methodologies?

A good paper to look at is:

'The LVEL turbulence model for conjugate heat transfer at low Reynolds numbers'

Agonafer, Gan-li and Spalding EEP-Vol. 18, Application of CAE/CAD Electronic Systems, ASME 1996.

I'm sure that there are many people out there who have many comments to make ......

Robin.

'All models are wrong, some though are more useful than others'

Attributed to a very wise man (not me).

Now , suddenly we have this problem bigger than Mars Mission. Is that a one Billion problem or a six Billion problem ? If everyone on the Internet can get their workstations or PC linked together and work together, we may be able to solve the complex 3-D problems in industries. ( assuming that in the future these workstations will come with the necessary hadrware and software, so you can just plug it in the phone line ) At the same time, we need short term solutions . Any suggestion ? Apparently, the brute force approach is not going anywhere ? I don't think it's going to work by pretending that a wall is always flat and smooth. If someone is planning to go to Mars, we better do something to come up with practical solutions. agree ?

> At the same time,
> we need short term solutions. Any suggestion ?

In X years we should be able to do DNS on conjugate heat tranfser problems at high Re. Nos. We could wait and bide our time, telling all those in industry to be patient, put away their cheque books and resort to envelope engineering techniques for the forseeable future.

Alterantively we could accept the inherent deficiencies of current CFD technology, quantify potential sources of error and foster a sense of trust between engineers and CFD vendors (whilst constantly researching and updating the technology).

The market is big and growing at a healthy rate. CFD developers/scientists should really start to look at the needs of those industries that could benefit from CFD, educate that market that they need CFD then tailor a CFD code to meet those needs. CFD should be a means not an end.

Robin.

I must say that the detail approach to the short term solution is still wide open. With more companies using commercial codes ( based on what I have seen in the last 8 years), the research and development activities in CFD have largely disappeared ( for various reasons)in these companies. With competition, code developers are forced to focus on the sale. It is hard to link the responsibility to any particular engineer or position. There are really only three alternatives1). use commercial codes, (2). develope your own in-house code, (3). do nothing. To get everybody involved in the black project or black box is not practical. So, I think we are still in the dark age.

Take a look at a recent AIAA paper by Patrick Roache entitled "Verification of Codes and Calculations", AIAA Journal, vol.36, No.5, 1998.

This is a great overview paper, and among other thing, introduces the reader to the "Grid Convergence Index" . GCI is a simple method for uniform reporting of grid convergence studies without any restriction to integer refinement, e.g. grid doubling.

Dear gueynard

I have read many suggestion useful for your problem and they are very helpful. I however wonder whether you problem is steady or unsteady flow. I have found several work wher the study was performed under steady flow assumption and found that the solution is changing for an interval of iteration number. It is good if you could monitor your convergence history to see that there is an absence of any anomaly

Hope this help

At the begining, people invented a 1-foot transonic wind tunnel. They were able to run the test and get the transonic results. And they were very happy. Later on they build a 4-foot transonic wind tunnel, and they were able to put a bigger model in the tunnel. So, they were able to get more data points, and they were happy. One day, they decided to build a 16-foot (test section=16x16) transonic tunnel so they can put the real thing in the tunnel. They succeeded in getting the results. One day, a young student tried to plot three sets of results on one graph paper and noticed that they don't match. Then, he talked to a CFD expert and was able to get the CFD results back. When he plotted the CFD data on the test results, he discovered a new law :" all results are wrong." You don't need millions of dollars to build wind tunnels to prove the new law, by adding more mesh points in the mesh, sooner or later , I think, there will be results which are right. The first step in the mesh generation must be : to determine the total number of mesh points and arrangement which will give you the right answer. I think, something like the " road test for drivers license" is required for those who are preparing themselves for the CFD job. It is too late for this century.

[engineer.iman]

although this is a very old post, it is very rich in information.
my supervisor asked me to do grid independence study as he said most journals that publish CFD work they request this study to be presented with the model. how ever the way he explained to me is to compare my mesh with another one that is double the number of cells. that is it, is that sufficient??

[som87]

I'll be giving a short explanation.
Suppose you are calculating incompressible flow i.e. flow properties to be computed are u,v, w & p.

Now say you got (M X N X O ) number of grid (at x, y &z direction). For k number of iteration, calculate and record the final flow property calculated. Now change the grid number to 1/2 each direction one by one and again record the flow variable. Then repeat this step again and you'll have a plot of how much is the deviation of your calculation depends on the grid number.

----grid independence test finished till your calculated variable doesnt change within a allowable range---

[engineer.iman]

Originally Posted by som87

I'll be giving a short explanation.
Suppose you are calculating incompressible flow i.e. flow properties to be computed are u,v, w & p.

Now say you got (M X N X O ) number of grid (at x, y &z direction). For k number of iteration, calculate and record the final flow property calculated. Now change the grid number to 1/2 each direction one by one and again record the flow variable. Then repeat this step again and you'll have a plot of how much is the deviation of your calculation depends on the grid number.

----grid independence test finished till your calculated variable doesnt change within a allowable range---

Thank you very much for the enlightening explanation, i'm gonna follow your advice and see how it will go.
another question: is there any way that i can compare the different solutions in Fluent; a plot or table? or do i have to export the results to some other software to compare?

[som87]

I do not work with fluent much these days.
how about exporting in ASCII format and reading the data via fortran/matlab?
Also, you can create some point/line/rake if you are only interested in some specific zonal parts

Sorry, not much help in that regard:s

[notpolarbearfood]

Originally Posted by som87

I'll be giving a short explanation.
Suppose you are calculating incompressible flow i.e. flow properties to be computed are u,v, w & p.

Now say you got (M X N X O ) number of grid (at x, y &z direction). For k number of iteration, calculate and record the final flow property calculated. Now change the grid number to 1/2 each direction one by one and again record the flow variable. Then repeat this step again and you'll have a plot of how much is the deviation of your calculation depends on the grid number.

----grid independence test finished till your calculated variable doesnt change within a allowable range---

Hi, posting for the first time and I realize this post is a couple months old.

I wanted to follow up on this "allowable range". I've been doing a grid independence study (unstructured). I am using a coefficient of drag to test for independence, and so far, after 12 iterations of refinement, only 1 sig fig is constant. I am looking to publish my findings and would like advice on what a typical "allowable range" is, or if there is an industry/academic standard for % variation or % error.

Cheers

[Aeronautics El. K.]

In my opinion, you should use the grid convergence index (GCI).
See:
http://arc.aiaa.org/doi/abs/10.2514/...rnalCode=aiaaj
and
http://www3.nd.edu/~jjwteach/60130/C...oache_1994.pdf

Lefteris

Originally Posted by notpolarbearfood

Hi, posting for the first time and I realize this post is a couple months old.

I wanted to follow up on this "allowable range". I've been doing a grid independence study (unstructured). I am using a coefficient of drag to test for independence, and so far, after 12 iterations of refinement, only 1 sig fig is constant. I am looking to publish my findings and would like advice on what a typical "allowable range" is, or if there is an industry/academic standard for % variation or % error.

Cheers