
[Sponsors] 
Trying to perform test validity of Fluent with simulation of 2D airfoil 

LinkBack  Thread Tools  Display Modes 
April 24, 2011, 03:45 
Trying to perform test validity of Fluent with simulation of 2D airfoil

#1 
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Hello, everyone!
My English is not very good, hope I can describe my problems clearly. I am trying to do some simulation on deformation of an airfoil, before that, I tried to test validity of Fluent on 2D airfoil which I thought would have no trouble. BUT, I have got big troubles. Here are my cases, and the outside of the flowfield is about 50 chord length listed as following pictures. The airfoil has sharp trailing edge with no length, so I try to construct a Cgrid. The Reynolds number is 2 million. First, I used velocityinlet and outflow as boundary conditions. But the lift coefficients are about or even more than 10% less than the experiments using SA and other full turbulence models. For transitional SST models, the residuals and lift coefficient are quite unstable, and I am not sure it's the convergent results even its results are more accurate for the experiment. Then I used pressurefarfield as boundary conditions. But it is not easy for me to get a convergent results. Most of the time, the residuals are varying at about 0.1 or 1 order, and the lift coefficients are varying. I doubt maybe my mesh is too poor. So I try my best to get better meshes. But it doesn't work. Check the mesh quality with gambit, the biggest EquiSize skew is about 0.479, and the biggest aspect ratio is about 589 near the airfoil. (Wall plus <1) . Check the mesh quality with Fluent 12, the maximum cell squish is about 0.59. What other parameters should I check ? Which aspect can I improve my grid? Or what set should I do for fluent？ It is driving me crazy~ I ever thought Fluent could simulate the lift coefficients of airfoil under moderate angles of attack~ And someone simulates blunt airfoil using Ogrid whose cell squish is about 0.74 and biggest EquiSize skew is 0.54, can get convergent results quite easily. I divide the flow field into several blocks, but I check the transition of different blocks very carefully, there are no sharp changes. Any comment would be welcome~ Thank you~ 

April 24, 2011, 05:59 

#2 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
Your grid seems to be reasonable. One thing you can try at some point is to move your outer grid even further, i.e. 100 times. You'll see a small difference, but definitely not enough to make up your 10% error. In general, for 2D airfoils, I like to see the outer boundary quite far away.
Can you please specify what Mach number (incompressible?) and angle of attack you are running at. Also, what is the value of cl for which you are comparing? In general, at Re 2 million, I would assume the CFD lift results would compare well. Granted, drag may be off. Also, your airfoil is quite thick, so I'm not sure what to expect. Sometimes it can be very hard, or even impossible, to compare to wind tunnel results. If possible, try to compare to results for which you have a good description of the experiment. It can be difficult to model 2D shapes in the wind tunnel. For example, if the wing goes from wall to wall, a vortex can occur at the junction of the wing and the wall as the angle of attack increases. This causes the airfoil to see a reduced angle of attack. This will result in your CFD predictions being higher than WT for a given angle of attack. One suggestion of mine is to run multiple angles of attack and see how you compare to the lift curve slope. Also, if the data exists and you are in a region where a separation bubble occurs, try to compare to results which have been tripped at the leading edge or try results for a thinner airfoil. These comparisons will build confidence in the CFD and experimental results. 

April 24, 2011, 07:37 

#3  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
Sorry I didn't describe my model in detail. The airfoil is a wind turbine airfoil S809 whose relative thickness is 21%. Re=2 million, so if I use pressurefarfield, the Mach number is nearly 0.0876. In fact I have simulated angles of attack from 0 deg to 20 deg for the velocityinlet and outflow boundaryconditions. SA can help to get a convergent result, but is not able to get an accurate lift coefficient ( for example 5% error). The transitional SST can get an accurate result, but the residuals fluctuated so I am not sure whether it's a convergent result. For the pressurefarfield boundary conditions, as it is not easy to be convergent, so I didn't calculate it too much. Besides the accurateness of the CFD, what is frustrating me most is that it's too hard to get a convergent result under pressurefarfield boundary conditions. If you wish, I can send you my cases. Thank you again. The attachment is one of the results. 

April 24, 2011, 07:47 

#4  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:


April 24, 2011, 08:21 

#5 
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
For the turbulent boundary conditions, I define turbulent Intensity 0.2% and Turbulent Viscosity Ratio 2. People around me said this is the parameter for low velocity wind tunnel. Does this set make any sense? Or, is it the source of the error or divergence?


April 25, 2011, 11:16 
Would anybody be so kind to help me?

#6 
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Hope my poor English won't stop your procedure to continue reading.
I try to construct a better grid, and try different topologies. But, still, it is not easy to get a convergent result using pressurefarfield BC. At the beginning of the calculation, the residuals fall down to 1e4, but as the calculation goes on, the residuals of continuity will increase to 1. If I use the 1st order discretization equation, there are no problem, but for 2nd order, the calculation is divergent finally. If I use 1st order equation at the beginning, and then change to 2nd order, the residuals will finally vary a lot as follows, ("1st order to 2nd order.png") but the lift coefficient seems even. I test the grid using SA model, when I look into the results, minus static pressure near the left side boundary (as shown in "minus static processure.png"), and the turbulent viscosity is much larger in the wake grid of the airfoil as follows ("turbulent viscosyty.png" ). Is this the cause of the divergence? How do people get a nice convergent results using Cgrid to simulate airfoil before? Could anyone be so kind to help me out? Any comment is welcome. Thank you~ 

April 25, 2011, 12:47 

#7 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
Hi didiean,
I'm not sure what the issue is with the outer B.C. I'm also not a Fluent user so I can't comment on the details of the B.C. I hope someone else on this forum will also help out. I looked into the pressure far field information on the ANSYS web site. The B.C. is based on characteristic variables so it should be OK. As described by the manuals it seems to be the standard non reflecting homentropic characteristic equations. What you are seeing at the left side of your B.C. (incoming) is something along the lines of what I associate with reflecting B.C.s (such as fixed far field). So I don't know what the story is. However, the characteristic B.C. can be sensitive to the time step. But, that usually occurs where the wake leaves the outer B.C. Also, I am assuming you are not running with some sort of Mach number preconditioning. However, since your Mach number is low, maybe this is activated. I don't know all the ins and outs of this, but, unless formulated correctly, characteristic boundary conditions are incompatible with Mach number preconditioning and will not converge. In regards to the turbulent viscosity in the wake, your solution is correct and it should not cause problems. Except.. If the velocities within the wake region have not had a chance to become sort of uniform and close to the freestream velocity, then the wake region will have difficulty converging with the outer boundary condition. In this case, the solution is to move the exit plane further way. But I think your grid is OK. As for your cl vs. alpha plots, your solutions are along the lines of what I expect, except I'm not sure why your SA lift curve slope is less than the transitional SST (I expected it the other way), but I'll associate this with my inexperience with thick airfoil solutions and transitional SST models. The lower cl max for the transitional SST model, the lower cl0 value for SA, and the unsteady solutions for the transitional SST model in the vicinity of cl max make sense. You can also compare your results to xfoil. I have no experience with the program, but I hear it does a good job for this class of problem. 

April 25, 2011, 13:30 

#8  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
The pressurefarfield BC is often adopted when simulating wind turbine airfoil as I know from others. Compared to inlet and outflow BCs, it has low chance to introduce reverse flow. I once doubt the validity of Cgrid together with pressurefarfield BC, but I have read some papers using this method, so, maybe, I have ignored some important sets. I once also doubted the quality of my grid, but I have made the grid satisfy the required parameters of FLUENT, for example, equisize skew, maximum cell squish, and so on. For simulation of airfoil using boundary layers, the aspect ratio of 600 may be not too big. I am not quite sure about the reason of the smaller lift curve slope of SA model, as I used 2nd order discretization and structured grid, the false diffusion shouldn't be the reason. Xfoil can simulate thin airfoil under moderate angles of attack well， but as I want to look into the flow field. so Xfoil won't help for this. 

April 25, 2011, 14:28 

#9 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
OK, so I gather you are using a density based method, i.e. compressible, since you are using a characteristic B.C. (i.e. pressure far field). I also assume Fluent's density based method has the basic restriction that you should not go below a certain Mach number unless you use Mach number preconditioning. Originally, I assumed your Mach number, M=0.0876, was high enough that you didn't need preconditioning. Maybe I'm wrong. One thing you can try is to bump up the Mach number to 0.2 and see what you get. Maybe the oscillations you see at the boundary will disappear. Or, you can try an incompressible solver.


April 25, 2011, 16:09 

#10 
New Member
Corrado
Join Date: Mar 2009
Posts: 15
Rep Power: 10 
Hi,
maybe my suggestion could appear trivial, but...why don't change the flow domain from cgrid to classical rectangular domain, keeping boundary condition, solver, turbulence model, etc., unchanged ? 

April 25, 2011, 17:12 

#11  
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
Quote:


April 25, 2011, 19:49 

#12  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:


April 25, 2011, 20:03 

#13 
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Thanks for your advice. But the rectangular seems almost the same with the Ctype domain at the wake area of the airfoil, besides, Ctype domain may have a grid with higher quality on the left of the airfoil. On the other hand, as you see, the outer of the domain is nearly 50 chord length, so maybe the outer shape won't influence too much.


April 25, 2011, 20:34 

#14 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
I think it is best to use the pressurebased method with a compressible solver. For me, it doesn't make sense to have a characteristic B.C. with incompressible flow.


April 25, 2011, 20:40 

#15  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
I still get another question, as you see, Re=rou*u*L/miu, when I want to simulate an one meter length airfoil at a fixed Reynolds number, the velocity will be fixed. But from the point of Mach number, it will change with the velocity and the sound velocity but not the chord length. So, if I decrease the chord length from one meter to 0.1, under the fixed Re, the velocity will increase to 10 times of the original one, and then the Mach number will increase to 0.876 which I think is quite different from what I am investigating. When I looked into the results with high residuals, I found that the density, temperature also varied on the left outer side of the domain . Well, when I increase the Mach number from 0.0876 to 0.15 (The velocity is nearly 52 m/s as calculated by FLUENT itself), it does seem get a convergent results. The residuals is decreasing now, and the lift coefficient is almost unchanging. Why does this happen? 

April 25, 2011, 20:45 

#16  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
Well, maybe I have misled you. From one version of FLUENT, it is using the density/pressurebased solver instead of compressible/incompressible solver. 

April 25, 2011, 21:59 

#17  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
I tried to reduce the chord length of the airfoil from 1 to 0.5, kept the Reynolds number constant and the Mach number became 0.17. But unfortunately, it didn't get convergent well as I had expected. Here is the problem, if I keep the chord length as 1, and only change the Mach from 0.87 to 0.15, a convergent result is obtained. Nearly the same Mach number appears different results on convergence/divergence. 

April 26, 2011, 04:53 

#18  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
Well, as I change the chord length of the airfoil, and then using Standard discretization instead of Two order, a convergent result is obtained. But if I change to Two order for pressure, then the residuals increase again, but still on an accepted level. Maybe, simulation using pressurefarfield is not easy to get convergent. But I am not quite sure about the reason. Are Riemann Invariants valid at low Mach number? As you have done similar calculations, maybe some low Mach number preconditioning should be done, but I haven't read some materials on this for FLUENT, though there is LowRe damping for Fluent 12. I wonder whether similar conditioning can be added into FLUENT. 

April 26, 2011, 16:19 

#19 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 479
Rep Power: 12 
I have never used Fluent so the comments I make are either a result of what I've heard or read, or what I guess. Each CFD code is very unique in how they implement things. CFD is much more of an art than a science. So I hope I don't mislead you in regards to your Fluent runs.
In regards to compressible flow, in general, Mach=0.087 should not require Mach preconditioning. Fluent may be different. When the Mach number gets down to 0.01, then difficulties definitely arise. For compressible flow, there are two pathways for the solution to advance, one is by pressure waves (speed of sound) and the other is fluid velocity. A solution is difficult to obtain when the fluid velocity becomes much slower than the speed of sound. The system becomes stiff. In general a solution can be obtained by decreasing the time step. But it is not assured that a real life solution will converge and, when it does, it takes a very long time. For your problem, I'm surprised that it is having difficulties converging at Mach 0.087 so I suspect there may be something else interfering with the solution process. In regards to Riemann invariants, I'm going to say that technically they apply at very low Mach numbers as long as the entire solution methodology is compressible. However, it may be possible that during the process of converging they are sensitive to the solution (or residuals) and therefore may throw the convergence process off easily. Therefore, they may not be robust at low Mach numbers. Of course it is very probable that someone has mathematically analyzed them and can tell you a lot more about than I and also suggest mathematical ways to increase the robustness. In regards to Reynolds number and convergence, changing the Reynolds number should affect how the solution converges close to the airfoil, not at the outer boundary, except where the wake leaves the boundary. If the wake gradients are benign when they cross the outer boundary, then changes in Reynolds number (i.e. viscosity) should also not change the solution convergence process at the outer boundary. What angle of attack are you having difficulty converging the solutions at? Again, I'm not well versed in Fluent, so what I say next may not apply at all to your problem. Anyway, I assume that you are trying to overcome convergence difficulties with your problem by reducing the time step. I also assume that you are using local time stepping (CFL) to converge the problem. Fluent must have ways of accelerating the solution process. Local time stepping should be one, and, looking at your grid, this should be OK. Local time stepping can cause problems when grid cells in the field become small. Small cells next to the boundary is OK. However, small cells in the wake can cause problems. But I don't think this applies to you. Another one is multigrid. It is possible that multigrid is causing problems. Try turning it off and see what happens. It will take longer (10x?) to converge. Also, from what I understand, Fluent has a coupled and uncoupled solution methodologies. In general, when there are supersonic pockets then the coupled solution methodology must be used. Obviously you don't have supersonic pockets. However, a coupled solution methodology should increase the stability of the solution process. I realize that your grid is made up of several grid segments. However, I assume Fluent is solving it as one block. Are you solving this on a single machine or many machines? If you are solving this on multiple machines, then Fluent might create a multiblock problem out of it. If Fluent is solving this as a multiblock problem, then the time step may need to be cut back. In general, this is an issue with higher order methods. But, again, I'm don't know the details of how Fluent works. I also hope other people help out. I'm running out of ideas. 

April 26, 2011, 20:29 

#20  
Member
Felix
Join Date: Mar 2011
Posts: 50
Rep Power: 8 
Quote:
For pressurefarfield BC, I just try to simulate flow field around an airfoil at 0 deg AOA. When I use velocityinlet & outflow BC using Transition SST model (turbulence model with transition model), small separated bubbles attach on the airfoil. But I don't think that's the reason of my divergence using pressurefarfield BC, as the full turbulence model cannot catch that bubble during calculations before. In present, I am using steady solver, which in FLUENT I haven't found any panel to set local time stepping or something like that. As you mentioned multigrid, I leave them defaults. Maybe, I should investigate the set and see whether any set will help. The reason I divided the domain into several blocks is that I want to simulate the motion of some parts of the airfoil. If I leave them as one block, there are large angles which in Gambit the BL doesn't work well, so I divide it myself. I am also using Gridgen recently, I think it works well in structured grid and doesn't need to divide the domain to obtain fine grid for this simulation. Recently I am just simulating it on single machine, but for the very case, multiple machines simulation is OK. Well, there is only one good and precise simulation result, but thousands of wrong results. Maybe the problems I meet is too weird and unique. Thank you all the same~ You do help me a lot to understand and analyze this problem. 

Tags 
airfoil, pressurefarfield, structured 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Airfoil 2D cfd simulation  Cocorito90  OpenFOAM Running, Solving & CFD  14  December 19, 2016 04:43 
OpenFoam Airfoil simulation  replacing Fluent with OpenFOAM  shereez234  OpenFOAM Running, Solving & CFD  1  November 3, 2015 04:54 
Problem with restart solution in shape_optimization.py  robyTKD  SU2 Shape Design  21  May 29, 2013 09:26 
LSR (Land speed record) car simulation on FLUENT  Maxime31850  FLUENT  2  May 1, 2013 11:15 
Flapping Airfoil Simulation in fluent + Udf  RajeshAero  Main CFD Forum  1  February 8, 2011 05:50 