Fluent: Tet Vs Poly mesh
I am modelling a flow through a closed channel flow in FLUENT. To check the grid independency, I have converted the initial tetrahedral mesh in to poly hedral mesh and run the simulation till the solution is converged. I have compared the pressure head loss values for both the cases and found out that the values (head loss) are differ in a big manner. That is, for example in Tetra hedral mesh case if i get a pressure Headloss of 10 cm of water column, i am getting a head loss of 16 cm of water column.
I haven't understood, why this is happening.
Please throw some light on this issue, as it is really very important for my work to proceed further.
Grid independence is usually determined by changing the size of the grid spacing. Switching the type of grid (as you have done) is not the appropriate way to check for grid independence. I would take whichever of your two cases has a courser grid and refine it. Then re-run the solution and compare the results. If the results change significantly you will need to refine the grid further and run again. Basically you need to continue refining until the results stabilize. This process can be quite time consuming. Best of luck to you.
Kevin Erhart, PhD
Central Technological Corporation
Just adding to some of Dr. Erhart's thoughts:
A grid-independence study is an extremely systematic process wherein the mesh is continually refined/coarsened from an initial mesh. Each mesh is a minimum of two times less or greater than the previous mesh.
For example, if I consider 2D axisymmetric flow in a pipe, I have to consider grid spacings in two directions-radial and axial.
Grid1-r=First point off the wall =0.01 and 200 axial points.
Grid2-r=First point off the wall =0.02 and 200 axial points.
Grid3-r=First point off the wall =0.04 and 200 axial points.
Depending on the results from Grids 1,2, and 3, I will decide upon Grid 4. If the results are converging to similar values, then I am on the right track by increasing the first point off the wall. If the results are diverging, then my 4th Grid will have 0.005 as the first point off the wall.
Further, if the flow features in the axial direction are not being adequately resolved, then a similar study will have to be performed in that direction as well, while keeping the r direction constant.
Also, the following points need to be kept in mind:
- The nature of the grid will have to remain exactly the same between grids.
- Only 1 characteristic of the grid can be changed per iteration.
- A minimum of 4 grids is required to conduct a complete grid independence study.
- Area of grid refinement needs to be done overall sense and in the particular region of interest.
There is a recent publication by Roache, Ghia, et al. which discusses grid-convergence index in detail. It might be useful to look at that.
Hope this helps.
Thank u both of you...
I have checked the grid independency with tet mesh. But i have read somewhere that the Poly mesh in Fluent gives more accurate results comparing to the Tet mesh. In my simulation ia m getting a different value from the Tet mesh (grid independency checked with refining) when compared to that with a poly mesh.
Which value is more accurate?? with tet mesh or Poly mesh...??
Thanks in advance
Before you can compare results you need to check the following in your grids:
- Do the 2 grids resolve all regions of interest in the similar manner. If one grid is very much finer than the other grid in the boundary layer, then the results cannot be compared. (As one with present the viscous solution to your problem, and the other will be the inviscid solution)
- What is the total cell count in both the grids? Are they the same in same parts of the geometry?
Your solution ultimately is independent of the grid. However, if one of the grids resolves the flow adequately, and the other doesn't then the solutions cannot be compared.
I would suggest that you make one more grid, and see if your solution is still changing. It could imply that you are still not in the asymptotic region for your solution, and might need to refine your grid further.
Also, what are the solution parameters you are looking at when comparing the grids?
The poly grid is not manually generated but, in Fluent there is option to convert the domain in to Poly elaments. So Fluent converts the Tet mesh in to Poly if we select this option. So I guess the flow is resolved in a similar manner.
If u have any literature on grid independency check in FLUENT, pls forward it to me.
Thanks in advance
Personally, I wouldn't let Fluent automatically do anything like splitting tet mesh into poly mesh or refining or coarsening the mesh, etc. as I would prefer to have control over the grid and the solver. And plus, I'm not too clear on how the above actions happen in Fluent as well.
My suggestion for you is to manually make the grids (as per your requirements and the requirements of a grid independence study) and use Fluent to only solve for the flow and not modify the grids.
I don't know whether one can generate a Poly hedral mesh in Gambit (or in Ansys-Meshing of the work bench)...Have u worked with poly hedral meshes before? if so let me know where can i find these options in Gambit or Ansys-meshing.
Hi Sowmya...so do you have any info about the poly meshes in Gambit or Ansys meshing or ??? it's very important for me to solve this issua as soon as possible to move forward. So let me know if u have any info and even if u don't know the details pls let me know that also....
Check for convergence error.
Sounds to me like you are suffering from convergence error. It doesn't matter what grid type you use, if the solution isn't converged then the results are junk.
I suspect that you are using the default convergence criteria of 1x10-3 and fluent gives you the message "solution is converged!". Well, don't believe it, only YOU can determine if a solution is converged!
Reduce your convergence criteria to 10x-18, run the solution for 10000 iterations. What you should see is that the residuals will level off at some point (provided your mesh quality is good i.e. max equiangle skew less than 0.85). One of the biggest problems in CFD lies in solutions which simply are not converged, I have read 10's of papers with results which I would question due to this.
By running simulations for 10000 iterations (assuming steady-state) this will be enough to identify where convergence has occurred. It may be after 500 iterations or 8000, you can't tell unless you do a greater number first to see when the residuals level off. When I ran vehicle aerodynamics simulations during my PhD, convergence occurred after 9500 iterations on a 6.7M cell grid, all the residuals just dropped prior to that, see attached image.
I assume that your meshes are nowhere near that big so convergence should be much sooner. However, check this!
In my experience, proper convergence occurs much faster with polyherdal cells but often the actual convergence level may be higher than the equivalent tetrahedral mesh. Personally I would be using tet cells first and then converting them to poly ones to check the results of grid independence in a fair comparison.
It is very tempting to use poly meshes because of their speed of convergence, however, keep in mind that fluent uses an agglomeration process by default which results in drastic coarsening of the cells compared to the base tet grid upon which it is based. Furthermore, there are very few publications showing how the respective performance of these cell types compare. As such, approach with caution!
As mentioned earlier in the thread, Roache's grid convergence index (GCI) is a good way of estimating the discretisation error i.e. the errors due to the grid not being fine enough. If you use three grids, coarse, medium and fine, ensure that the grid spacing is at least 10% (refinement factor, r = 1.1) finer in successively denser meshes. Ideally a refinement factor of 2 should be employed but as reported in many publications, this is rarely feasible as the cell count increases exponentially.
A good rule of thumb is that you should always produce the finest grid you can to begin with and coarsen from there.
One final point is that the quantity of interest is HUGELY important. If you are testing for grid independence of say the absolute pressure at a single point in a given solution domain, you may never reach grid independence if the gradients are high there. In such a case that actual pressure value is highly dependent on POSITION within the flow field ans well as the actual grid density.
As such, try to use quantities which represent the flow using solutions from a number of cells. For instance you might be interested in the average concentration of a species in an air volume surrounding a person. This would not only give more satisfactory results than the concentration at a single point but it would be more relevant to the problem. If you do need to know specific quantities in small locations then there is no option but to refine the grid there.
Hope this helps,
|All times are GMT -4. The time now is 03:32.|