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

2D Airfoils at Low-Re

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

Like Tree1Likes
  • 1 Post By cfd seeker

Reply
 
LinkBack Thread Tools Display Modes
Old   December 31, 2012, 11:27
Red face 2D Airfoils at Low-Re
  #1
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 4
mrenergy is on a distinguished road
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 is offline   Reply With Quote

Old   December 31, 2012, 12:26
Default
  #2
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 4
mrenergy is on a distinguished road
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
mrenergy is offline   Reply With Quote

Old   December 31, 2012, 12:42
Default
  #3
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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 likes this.
cfd seeker is offline   Reply With Quote

Old   January 3, 2013, 15:08
Default
  #4
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 4
mrenergy is on a distinguished road
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
mrenergy is offline   Reply With Quote

Old   January 4, 2013, 00:51
Default
  #5
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
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
cfd seeker is offline   Reply With Quote

Old   January 4, 2013, 12:10
Default
  #6
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 4
mrenergy is on a distinguished road
thanks again and a lot
mrenergy is offline   Reply With Quote

Old   January 4, 2013, 13:06
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
pressure-far-field boundary conditions can only be used with ideal gases.
Use velocity inlet if flow is incompressible
Far is offline   Reply With Quote

Old   January 4, 2013, 15:09
Default
  #8
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 4
mrenergy is on a distinguished road
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
mrenergy is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Two-equation turbulent models: low re airfoils truffaldino Main CFD Forum 51 March 19, 2012 19:57
Low Drag airfoils for Supermileage vehicle Himanshu FLUENT 1 December 25, 2005 09:51
DNS -low Reynolds number Airfoils Pat Main CFD Forum 2 January 21, 2005 15:17
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12
Low Re Airfoils Chan Main CFD Forum 0 September 23, 2003 21:22


All times are GMT -4. The time now is 02:58.