
[Sponsors] 
March 25, 2020, 18:24 
GOE 387 2D simulation

#1 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Hello everyone, I am validating the 2D fluent results data of the Gottingen 387 against 3D wind tunnel data. However the results are far from the wind tunnel results. I have used a y+=1, the mesh started with 34000 nodes, then I optimised the mesh with 84000 nodes. I have use the kepsilon realizable, the komega SST and the transition kkl omega. For BC inlet=velocityinlet, and outlet=pressureoutlet. Simple solution starting with first order to stabilise the iteration (1000 iterations) and the changed to second order (2000 iterations). Pic 1 are the results with the transition kkl omega. Pic 2 are the kepsilon realizable and komega results. All of them converged. I tried to make a more robust mesh with 150000 nodes. However its presenting turbulent viscosity and reverse flow :S. I would appreciate any help to know why is not giving close results to the wind tunnel and suggestions to acquired it. And second, why the robust mesh is presenting the mentioned problems. Thanks a lot!!!!!!!!!


March 26, 2020, 03:48 
Material and Operating Conditions

#2 
Senior Member

What are the material properties and Mach number that you simulating it for?
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 08:59 

#3 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Hello vinerm, the material is fluid=air, only using density and viscosity, both changes at each AoA. But overall the density used was 2.30 and the viscosity 1.95E06. Mach number used varies as well from 0.061=21 m/s to 0.067=23m/s. thanks.


March 26, 2020, 09:12 
Material

#4 
Senior Member

Viscosity appears to be alright but why is the density twice the normal value? Is it low temperature or higher pressure?
Furthermore, a finer mesh is not robust, rather it is the other way around. Coarser meshes are robust as far as the robustness refers to the stability of the solution. Finer meshes may resolve better but there is a limit to that. Beyond that, resolution causes issues with RANS models. Since you are looking at only coefficients, I suppose the issue is with the reference values being used. Since coefficients are normalized values, Fluent uses reference values from the Reference Values Panel to determine these coefficients. Default values are not as per your requirement. You need to change those values to match with your case before reporting the coefficients. You do not need to rerun the simulations until unless these coefficients are used to modify anything. Just modify the values and replot the charts.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 09:50 

#5 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
All the values were taken from the wind tunnel test. The temperature is higher (312.15 K) than standard S.L. values and also the pressure= 136516.2 Pa. Thanks for the clarifications about the mesh, helps a lot. The picture attached shows the reference values used. The only value I have doubts is the depth one as is new for me, I put the wing span, is that correct?. Again, the reference values were taken from the wind tunnel experiment, thus I was expecting the same results.


March 26, 2020, 10:04 
Reference Values

#6 
Senior Member

Only area, density, and velocity are used for the prediction of force coefficients. Moment coefficient uses length in addition. Depth is used for 2D simulations as a dimension in third direction.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 10:12 

#7 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
The moment is giving good results, thus the length is ok. So, probably the area is wrong?. If the reference values taken are ok, do you think there might be another problem?. About the depth, the third direction could be the wing span?, or what do you mean with the third direction?. Thanks again.


March 26, 2020, 10:19 
Third Direction

#8 
Senior Member

Yes, the third direction is wing span (length along the zaxis).
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 10:24 

#9 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Thanks a lot for the clarification. I just double checked the values and are the same I just show you. If you happen to come out with another explanation of why the CFD results are not close to the wind tunnel ones I will appreciate it. Thanks again for you valuable help.


March 26, 2020, 10:31 
AoA

#10 
Senior Member

I looked at the graphs again. It appears the results are not matching for higher AoA values. Is there flow separation at those AoAs? Did you plot for those AoA values? Does it maintain the resolution?
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 11:37 

#11 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Yes indeed, they do not match at high AoA. Please find attached the velocity magnitude contours at 9, 12, 18, and 21 AoA. They are having a big flow separation at 18 and 21. I have no check the y+, I am going to and share it, thanks.


March 26, 2020, 14:08 
Modeling AoA

#12 
Senior Member

Are you modeling AoA by changing the direction of flow at the inlet? Because the airfoil appears to be always aligned with xaxis.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 14:16 

#13 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Yes, that is correct. I am changing the direction of the flow at the inlet.


March 26, 2020, 15:19 

#14 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Hello again vinerm, here are the yplus graphs for an AoA of 9, 0, 12, 18, 21. To be honest I do not know how to interpret them. It looks like the mesh is not ok neither in the leading edge nor in the trailing edge. The trailing edge has a yplus peek up to 140. I will appreciate your feedback, thanks.


March 26, 2020, 15:33 
Mesh

#15 
Senior Member

The values look alright, except at the trailing edge, however, that won't make a difference. So, the mesh is good, flow looks good, operating conditions are good. What could be the reason for coefficients to not match? One reason could be material properties. You are considering constant but the reality is always different. Though Mach number is below 0.3, I suppose even below 0.2, but you can try for one case with ideal gas. I am not sure if it will help but you don't have anything to lose by trying.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 15:42 

#16 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Thanks for your feedback, I am going to use ideal gas then and see what happens. On the other hand, can you expand your explanation about the yplus, because I see that the line is fluctuating a lot at the leading edge. Thanks.


March 26, 2020, 15:48 
Explanation

#17 
Senior Member

is a Re number based on shear velocity scale. For the length scale, half of the first cell thickness is used. Looking at the mesh, cell thickness appears to be constant, however, shear velocity is certainly not constant. It depends on the wall shear stress. The variations in the are not important as long as its value is maintained below 5 because that's the thickness of viscous sublayer.
__________________
Regards, Vinerm PM to be used if and only if you do not want something to be shared on the Forum 

March 26, 2020, 16:14 

#18 
New Member
Join Date: Aug 2018
Posts: 14
Rep Power: 3 
Clear to me, thank you very much. I will post in here the results with ideal gas.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Convergence Problem  Transient Simulation  gemxx  Main CFD Forum  0  July 15, 2018 09:36 
Mapping Field Data for Mesh Regions from Another Simulation  veterator  OpenFOAM PreProcessing  1  July 10, 2018 05:28 
Surface Source  Fixed Temperature?  robtheslob  FloEFD, FloWorks & FloTHERM  18  May 12, 2017 02:28 
Simulation FPEs  turbulence for transient and steadystate?  DaveR  OpenFOAM Running, Solving & CFD  5  March 5, 2017 15:06 
setting up a simulation with multiple interactions  phandy  OpenFOAM Running, Solving & CFD  1  October 6, 2014 03:16 