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

3D Naca wing divergence

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 9, 2013, 14:54
Default
  #21
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,258
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I was thinking of more smooth mesh. Here it is...
Attached Files
File Type: zip NACA wing 09 03_Far2.zip (38.1 KB, 4 views)

Last edited by Far; March 9, 2013 at 15:43.
Far is offline   Reply With Quote

Old   March 9, 2013, 15:35
Default
  #22
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
I was thinking of more smooth mesh. Here it it . ...
How are those curved edges made? Splines curves?
Bollonga is offline   Reply With Quote

Old   March 9, 2013, 15:47
Default
  #23
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,258
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Blocking > Edit edge (s) > Link edge

Source edge : The edge whose shape you need to copy to other edge.

Target edge : Whose shape is to be changed

Factor : 1 -3 . I've used factor of 3
Far is offline   Reply With Quote

Old   March 10, 2013, 08:18
Default
  #24
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
I have used pressure based coupled solver. Other options used are : High order term relaxation. 2nd order flow scheme. Cournt number 20,000.

up and down boundaries are slip walls. Did not specify the turbulence level, used default settings.
It works for me too! You're the man!

I've applied this same setup with k-epsilon Realizable model to the 3D flat plate case with 70 angle of attack I've been dealing with. It's working too! I think the key is the courant number modification.
How does it afect to increase it from default 200 to 20,000?

What is the different between slip zero shear stress wall and symmetry BC?

I'm using default k and epsilon at the inlet but I'm gonna need to modifiy them. Would this make me change the mesh or reducing even more under-relax factors?

For how long should I maintain the reduced under-relax factors? It's making my simulations pretty slow...
Bollonga is offline   Reply With Quote

Old   March 10, 2013, 10:14
Default
  #25
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,258
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
I've applied this same setup with k-epsilon Realizable model to the 3D flat plate case with 70 angle of attack I've been dealing with. It's working too! I think the key is the courant number modification.
It is cournt number for pressure-based coupled solver which couples continuity and momentum equation only. So the definition is not same as the cournt number we study in CFD course.


Quote:
How does it afect to increase it from default 200 to 20,000?
Fluent guide says, you can increase it to 200,000 and it worked for me for transition modelling of low pressure turbine. In fact this model was used first time for the the low pressure turbine case (i can give you that paper which made use of Fluent's pressure based coupled solver) due to fact that there is strong coupling of continuty and momentum equation. And when Simple type algorithms are used (which couples pressure - velocity fields loosely) they introduce errors for this class of problems and make the convergence difficult.


Quote:
What is the different between slip zero shear stress wall and symmetry BC?
Both are same except that you need plane surface aligned with any plane for symmetry condition while slip condition can be applied to any surface. In fact I use slip condition due to my past practice. Some friends here always use symmetry condition. But in my point of view results should be same.

Quote:
I'm using default k and epsilon at the inlet but I'm gonna need to modifiy them. Would this make me change the mesh or reducing even more under-relax factors?
Why you want to change them? Do you want to match some test conditions for which you have specific values of turbulence parameters. Any how , you dont need to change any thing.

Quote:
For how long should I maintain the reduced under-relax factors? It's making my simulations pretty slow..
For pressure based coupled solver, we don't have option for URF!

Last edited by Far; March 10, 2013 at 10:33.
Far is offline   Reply With Quote

Old   March 10, 2013, 11:54
Default
  #26
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Quote:
Originally Posted by Far View Post
Why you want to change them? Do you want to match some test conditions for which you have specific values of turbulence parameters. Any how , you dont need to change any thing.
Yes, I need to match some test turbulence conditions.

Quote:
Originally Posted by Far View Post
For pressure based coupled solver, we don't have option for URF!
In the solution controls panel there's the option to modify explicit relaxation factors for momentum and pressure and under-relaxation factors for density, body forces, k, epsilon and turbulent viscosity. I've reduced to half all that values. Once the solution is converging, can I change them to default without risking the convergence?
Can I change to 2nd order schemes for k and epsilon to get a more accurate solution?
Bollonga is offline   Reply With Quote

Old   March 10, 2013, 12:06
Default
  #27
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,258
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
In the solution controls panel there's the option to modify explicit relaxation factors for momentum and pressure and under-relaxation factors for density, body forces, k, epsilon and turbulent viscosity. I've reduced to half all that values. Once the solution is converging, can I change them to default without risking the convergence?
Ah those parameters. You can play with them. Generally speaking, I use default values.


Quote:
Can I change to 2nd order schemes for k and epsilon to get a more accurate solution?
I don't think turbulence needs second order accuracy. If you are not modelling transition type of flows, results wont change much. In transition dominated flows, I have observed no separation at all when used first order turbulence discretization.

Just think, you have already averaged out the quantities and now you want to add the averaged change in mean flow due to turbulence. How accurate would be averaged quantities with 2nd order accuracy . Probably you will get same averaged values
Far is offline   Reply With Quote

Old   March 10, 2013, 15:08
Default
  #28
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 271
Rep Power: 7
Bollonga is on a distinguished road
Even if it's converging, CD and CL are far from their correct values. I guess I have to let the simulation run longer. The problem is it's too slow!
I'm simulating the transient case for the 70 inclined flat plate with adaptive timestepping from 1e-3 to 1e-6 but it's always take a timesetp between 1e-5 and 1e-6 s. I've put 50 iterations per timestep.
I need at least 1s of simulation and it taking 1 day to do 4e-4s...
Bollonga is offline   Reply With Quote

Reply

Tags
3d wing, airfoil, divergence, turbulence

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
Divergence problem Smaras FLUENT 13 February 21, 2013 06:03
3d vof Smaras FLUENT 2 February 19, 2013 07:58
[ICEM] Blocking For Swept Wing air_engineer_arsenal ANSYS Meshing & Geometry 13 July 24, 2012 11:52
Quarter Burner mesh with periosic condition SamCanuck FLUENT 2 August 31, 2011 11:34
NACA wing Imanuel CFX 2 July 22, 2005 01:48


All times are GMT -4. The time now is 19:36.