CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

GOE 387 2D simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 25, 2020, 18:24
Thumbs up GOE 387 2D simulation
  #1
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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 k-epsilon realizable, the k-omega SST and the transition k-kl omega. For BC inlet=velocity-inlet, and outlet=pressure-outlet. 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 k-kl omega. Pic 2 are the k-epsilon realizable and k-omega 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!!!!!!!!!
Attached Images
File Type: jpg pic 2.JPG (82.7 KB, 5 views)
File Type: jpg pic1.JPG (69.5 KB, 7 views)
File Type: jpg Robust mesh 2.jpg (194.2 KB, 6 views)
File Type: jpg Robust mesh.JPG (113.0 KB, 3 views)
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 03:48
Default Material and Operating Conditions
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 08:59
Default
  #3
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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 1.95E-06. Mach number used varies as well from 0.061=21 m/s to 0.067=23m/s. thanks.
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 09:12
Default Material
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 09:50
Default
  #5
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Attached Images
File Type: jpg Ref..JPG (37.1 KB, 3 views)
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 10:04
Default Reference Values
  #6
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 10:12
Default
  #7
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 10:19
Default Third Direction
  #8
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
Yes, the third direction is wing span (length along the z-axis).
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared on the Forum
vinerm is offline   Reply With Quote

Old   March 26, 2020, 10:24
Default
  #9
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 10:31
Default AoA
  #10
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
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 y^+ 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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 11:37
Default
  #11
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Attached Images
File Type: jpg -9.JPG (58.7 KB, 1 views)
File Type: jpg 12.JPG (180.3 KB, 1 views)
File Type: jpg 18.JPG (166.3 KB, 1 views)
File Type: jpg 21.JPG (64.3 KB, 1 views)
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 14:08
Default Modeling AoA
  #12
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
Are you modeling AoA by changing the direction of flow at the inlet? Because the airfoil appears to be always aligned with x-axis.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared on the Forum
vinerm is offline   Reply With Quote

Old   March 26, 2020, 14:16
Default
  #13
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
Yes, that is correct. I am changing the direction of the flow at the inlet.
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 15:19
Default
  #14
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Attached Images
File Type: jpg yplus -9 zoom.JPG (95.8 KB, 2 views)
File Type: jpg yplus 0 zoom.JPG (94.7 KB, 2 views)
File Type: jpg yplus 12 zoom.JPG (96.9 KB, 2 views)
File Type: jpg yplus 18 zoom.JPG (96.0 KB, 2 views)
File Type: jpg yplus 21 zoom.JPG (94.5 KB, 2 views)
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 15:33
Default Mesh
  #15
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
The y^+ 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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 15:42
Default
  #16
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
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.
Herjhoa is offline   Reply With Quote

Old   March 26, 2020, 15:48
Default Explanation
  #17
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 1,305
Blog Entries: 1
Rep Power: 21
vinerm is on a distinguished road
y^+ 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 y^+ 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
vinerm is offline   Reply With Quote

Old   March 26, 2020, 16:14
Default
  #18
New Member
 
Join Date: Aug 2018
Posts: 14
Rep Power: 3
Herjhoa is on a distinguished road
Clear to me, thank you very much. I will post in here the results with ideal gas.
Herjhoa is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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 Pre-Processing 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 steady-state? 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


All times are GMT -4. The time now is 01:05.