
[Sponsors] 
On grid independent solution for pulsatile flow 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 7, 2005, 15:01 
On grid independent solution for pulsatile flow

#1 
Guest
Posts: n/a

Hi all,
I am modelling a 2d pulsatile flow in a conical tube for an undergraduate project. This tube is about 15 cm long with a radius varying between 6.5 mm and 12.5 mm. I use a velocity inlet and a pressure outlet. I am trying to acheive an grid independent solution. To do so, I compare a grid having 200 000 cells vs. one having 800 000 cells. I have setup monitors for various quantities including the areaweighted velocity magnitude of points lying on the centerline (symmetry axis) of the tube. When comparing the 2 cases I get satisfying results. My problem is when monitoring the integral of wall shear stress on the wall of the tube. I get vary different values (30% error) when taking the cycle timeaverage. My question is does this mean that my grid is not fine enough? Can someone give an order of magnitude as to how many cells I should be using to obtain a gridindependent solution? From what I had read I tought 200 000 cells would be more than enough for a laminar case... Any comments would be much appreciated. Thanking you in advance for your time. David 

June 7, 2005, 18:16 
Re: On grid independent solution for pulsatile flo

#2 
Guest
Posts: n/a

Dave,
Here is an answer to your question. In order to be able to conclude a grid independent solution for this problem, you will need at least three meshes. Unfortunately, the actual size of them can not be known a priori. However, it is assumed in numerical analysis that an infinitely dense mesh will yield the exact solution of the PDEs being solved, minus the truncation error. That isn't possible of course, so there may be some guidance in the literature for what size to start with and perhaps that is why you chose your sizes as you did. 200k or 800k may be reasonable sizes, but they will need to be confirmed in comparison to other grid sizes and/or in comparison to realworld validation data. To conduct the grid independence analysis, start with the grid solution for which you have the most confidence. Then multiply that grid size by a factor of 1.3 either coarsening or refining. The value of 1.3 is known through experience to yield reasonable enough differences in grid sizes that if the calculated solutions are similar, then the actual solution is not dependent upon the grid. This is exactly what you are trying to prove. So, for the 200,000 cell grid, refining at 1.3 gives you 260,000 cells. Now comes the question of which direction to refine. In 2D, should it be X or Y or both? For complex situations, it may be important to find out if there are directional influences. For pulsatile flow, this may indeed be the case. However, to make some initial progress, I recommend a uniform refinement in both X and Y. Solve the new grid and check to see how closely the values agree. If they are relatively close, refine the grid containing 260,000 by a factor of 1.3 giving 338,000 cells. Again solve this grid and compare values. If they are not close, conduct this analysis on your finer grid for meshes of 800K, 1040K, and 1352K. Compare the values. In either the coarser or finer cases, you will be able to ascertain the percent relative difference ((newold)/old) x 100 between your values of interest. How closely your values of interest are to one another are an indication of the uncertainty in your solution due to the grid. The PRD may be 10% or it may be 90%, or the deltas between values may be small or large. How acceptably large they are will be decided by some qualitative metric, such as, "Decreasing the percent relative difference by an additional 5% (from 15% to 10%) will require solving the flow problem on an additional grid of 1500K cells. Based on the previous calculations, this will necessitate an additional week of computation time, which will cost X dollars." Or you may have realworld data to compare to. In that case, again, how closely you need to get to them will determine where you stop your simulations. As an example, lets assume you extract scalar values from three of your grids. They are, in order of increasing grid cell size, 16.23, 14.51, and 13.75. The absolute differences between these values are 1.72 and 0.76. The absolute percent relative differences are 11.85 and 5.53. From this we can see that the differences between solution values are decreasing as the total grid cell size increases. But do they continue to decrease or do they start to level off? If a fourth grid with even more cell sizes is added, and the extracted value of interest (extracted from same point in time and space as the other grids) is 13.56, the newest absolute difference is 0.19 and the newest percent relative difference is 1.4. So, we have 1.72, 0.76, and 0.19 for absolute differences and 11.85, 5.53, and 1.4 for relative differences. From these numbers we can see that there is not a constant rate of decrease. Instead, we see that the rate of decrease is changing from, let's call it "highly sloping" to "gently sloping". What this means is that we are seeing less and less change due to the grid on the solution. To continue refining the grid at this point is likely not economic because we are not seeing much difference with new grids of increasing cell sizes. At this point, we chose the solution from the grid having the greatest number of cells and assume based on our analysis that we have a reasonable "model" of our particular problem. Some may argue that the mesh of the next highest number of cells is chosen as the "final grid" because information is known for either side of it, and that's fine, too, but if the differences are small, then it probably doesn't matter. If they're "large," continue refining. Also, if realworld data are available, then the simulation result can be compared and perhaps even "validated." Now, recall that you have resolved the grids uniformly for X and Y, there may be a need to resolve only in one direction or the other, depending on the number of cells in the near wall region. The process described above is repeated when conducting directional grid independence analysis. Some references to check: Patrick J. Roache: Verification and Validation in Computational Science and Engineering, 1998; Celik & Keratekin: Celik, I. and Karatekin, O. 1997. Numerical Experiments on Application of Richardson Extrapolation with Nonuniform Grids. Journal of Fluids Engineering. Vol. 19, pp. 584590. Final piece of advice... do not go haphazardly into the process. Instead, decide which grids you will be refining, decide your refinement factor (1.3, for example), identify your boundary conditions, and write everything down into a table. Check off each grid as it is built and solved. When all are solved, then conduct the grid convergence analysis. Don't make any changes to the grids (other than grid size) as you conduct the simulations, including the number of iterations needed to reach convergence. When you are finished you will be able to see the difference in results and make a conclusion about the grid size as a parameter influencing the results of your simulation. The above procedure can be applied to any parameter in your simulation, such as time, number of iterations, inflow velocity, etc. The above are the basics of assessing grid independence. To determine a grid convergence that gives a useable value of uncertainty, that is, we can say that we are uncertain about only 10 or 5% of the result, requires several more steps, including demonstration of iterative independence. Best of luck, I hope this has helped. Aaron 

June 8, 2005, 10:54 
Re: On grid independent solution for pulsatile flo

#3 
Guest
Posts: n/a

Hi Aaron, Thank you so much for your comments. They really give me a good explanation.
One other question: At some point you mention :"Don't make any changes to the grids (other than grid size)[...]". Does that mean that grid adaption should be avoided. In my case I used it because some of the cells near the wall did not have a good aspect ratio near the wall (both for the 200k and 800k grids). Is this a potential source of more trouble that need to be? Best Regards, David 

June 8, 2005, 13:50 
Re: On grid independent solution for pulsatile flo

#4 
Guest
Posts: n/a

David,
Refining the grid through the adaption step in FLUENT is a very good method for locally optimizing cell sizes to achieve realistic solution values that are *expected* based on the solver, models, and BCs that have been applied. However, if there is a change made to one of the refined grids but not to the others, *will* you be able to ascertain whether any change in solution was due to the refinement or was due to the adaption? The answer is probably not because it may be difficult to determine where the change in solution came from. Thus, it would be best to conduct the grid analysis only grids that have the same kind of refinement. If you believe that grid adaption is necessary, then do that on the grid for which you have the most confidence in the solution. Then export that grid from FLUENT back into GAMBIT so you can see what it looks like and also have the ability to make changes to it. Using the adapted grid as a template, refine according to your chosen refinement factor being sure to maintain a grid that has a similar adaption appearance as the originally adapted grid. This may require some creative GAMBIT work, but it should be possible if you define edges to be the length of the refined area and then force the mesh to scale appropriately along that length and into the heart of the computional domain, i.e. toward the center. This can be done by applying the appropriate "size function" to the edge and meshing inward. Maintaining the cells as quadrilaterals may be difficult, but I would urge you to try. If you must go to trishaped cells, then make sure all of your grids are trishaped. Or if you can keep them as quads, again do that for all grids. One way to apply different sizes to different regions is to subdivide the computational domain into multiple faces. Use edge meshing to obtain the desired structure of the mesh, then mesh the interiors afterward. Hope this helped. Aaron 

June 8, 2005, 17:20 
Re: On grid independent solution for pulsatile flo

#5 
Guest
Posts: n/a

Many thanks Aaron, Your comments are very much appreciated!
Best Regards, David 

March 25, 2022, 04:33 
Difficulty in obtaining grid independent value

#6  
New Member
Vidya Muthulakshmi M
Join Date: Aug 2020
Posts: 4
Rep Power: 4 
Quote:
Hi, Very useful reply. But I am getting increased error with increased mesh density. Can someone let me know what can be the reason? 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
initialize flow field with steady state solution  holg  FLUENT  0  July 13, 2009 18:10 
Mesh independent solution  CFX Begineer  CFX  0  October 27, 2002 11:54 
Combustion Convergence problems  Art Stretton  Phoenics  5  April 2, 2002 06:59 
Discussion about Mesh independant solution  Seb  Main CFD Forum  13  May 22, 2001 14:37 
Grid Independent Solution  Hesham M. Aly  FLUENT  2  October 5, 2000 09:24 