CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   2D Airfoils at Low-Re (http://www.cfd-online.com/Forums/fluent/111200-2d-airfoils-low-re.html)

mrenergy December 31, 2012 11:27

2D Airfoils at Low-Re
 
Hello everybody
Happy New Year

I am working on a family of 2D Airfoils up to 10% camber and 5% thickness
investigating the LSB Cl, Cd, and BL parameters for Re from 70 000 to 200 000

I've finished ICEM-meshing

May anybody summarizes his experience in similar work (even by short remarks and advices) for ...

1- ICEM proper meshing criteria
2- FLUENT setting to get the best results

thanks for reading
any kind of help being appreciated
thanks in advance
GOOD LUCK for all
Best Regards

Mamdouh

mrenergy December 31, 2012 12:26

summary of my work on ICEM ...

11 to 15 times upstream
21 to 25 times downstream

Geometric series
250 to 300 points in both directions

on FLUENT
I am trying the different suitable models and settings and I am waiting for your advices

cfd seeker December 31, 2012 12:42

Few suggestions from my side
1. Try solving this problem on Full structured quad mesh. Don't start with unstructured tri elements.

2. Resolve the boundary layer properly so that you get drag values comparable to the literature results.

3. Start with SST kw turbulence model. On 70000 Re. No the flow over the airfoil will be transitional(confirm it from the literature). For transitional flow use k-kl-w or SST transition model.

4. For SST kw ensure wall y+ = 1 and for k-kl-w and SST transition ensure wall y+ <1 and also the sufficient mesh resolution in the stream wise direction also.

5. Use Pressure Farfield boundary condition.

mrenergy January 3, 2013 15:08

thanks a lot dear CFD seeker for your concern and fast response,
and sorry for my delay, I faced some technical problems in my laptop

I reached a mesh quality of 0.8, is that enough to consider it as a good mesh?

Minimum Orthogonal Quality = 8.01112e-01
Maximum Aspect Ratio = 8.98120e+03


how can I find the value of y+ ?

when FLUENT launched it force me to change the pressure far field BC ... this message appears

pressure-far-field boundary conditions can only be used with ideal gases.

finally, what about the constants and default values for the mentioned solution models? do you see to keep it unchanged or modify it?
Best Regards and Respect
Mamdouh

cfd seeker January 4, 2013 00:51

Quote:

I reached a mesh quality of 0.8, is that enough to consider it as a good mesh?
Mesh quality of 0.8 in ICEM is very good

Quote:

how can I find the value of y+ ?
Use flat plate boundary layer thickness formula to calculate the B.L thickness and then reduce it by an order of magnitude to have a good approximate for airfoil. Use this value as the size of O-grid in ICEM and use at least 10-15 layers of cells inside O-grid. You can also approximate the size of the first cell away from the airfoil using the wall y+ formula in the literature which is developed for flat plate. Wall y+ calculator is also available in this forum. But you can check true wall y+ only in fluent durning the solution. Go to Plots>XY Plots. And have fun :)

Quote:

pressure-far-field boundary conditions can only be used with ideal gases.
Yes Pressure far field boundary conditions can only be used when you set air as "ideal gas". Go to "Materials" and set "Air" as "Ideal Gas" in fluent

mrenergy January 4, 2013 12:10

thanks again and a lot

Far January 4, 2013 13:06

Quote:

pressure-far-field boundary conditions can only be used with ideal gases.
Use velocity inlet if flow is incompressible

mrenergy January 4, 2013 15:09

thank you again Dear Dr. Far

that what I already did, velocity inlet instead of pressure far field as the flow is incompressible.

but the results still so bad for all models S.A, k-w, k-e, k-kl, and sst

I'd like to ask about the reference zones and locations ... what is meant by it? and how can I adjust it?
beside ... what model(s) you suggest for my cases? and how can I adjust the constants that embeded in it?
thanks in advance
Best Regards
Mamdouh


All times are GMT -4. The time now is 19:35.