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

Varying Inlet Angle of Attack for Structured Hexahedral C-Grid around an Airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 22, 2010, 02:46
Default Varying Inlet Angle of Attack for Structured Hexahedral C-Grid around an Airfoil
  #1
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Hi all -

This topic has been covered several times in various forms.
angle of attack CFX
introducing angle of attack on ICEMCFD HEXA
attack angle in CFX

However, I'd still like a little more information.

I've created a "structured" (the quotations are there because CFX does not accept structured meshes, so it's technically an unstructured hexahedral) C-grid in ICEM-CFD. I'm wondering two things:

1) In terms of my inlet boundary condition, I believe the proper implementation would involve specifying the curved section (O-grid) as the inlet. In the picture below, this is the sloppy red line.



The green lines are periodic conditions. The blue line is a specified static pressure. Would this be the best way to implement the boundary conditions?

2) I'm going to be parameterizing the angle of attack. I know there are several ways to change the AoA. Since I'm happy with my mesh and spent countless hours on it, I'd rather not rotate the geometry, whether that geometry is the airfoil itself or the airfoil within a cylindrical domain that acts as a stationary rotor with a GGI connection to a larger domain. Both of those methods would require re-meshing, which I'd like to avoid.

I would rather just change the inlet conditions to reflect the new AoA, as shown below.



I'm afraid that although this second method is simpler, it would cause problems. For one thing, the incoming flow would not be orthogonal to the sides of the cells at the leading edge of the airfoil, as shown below. I believe that this may cause numerical errors or an altered AoA compared to the desired value.



Additionally, I'm sure there are other issues I'm not taking into consideration at the moment (I'm exhausted).

Essentially, I'm wondering if my simple AoA parameterization method is an accurate enough way to simulate changing AoA, or if I should do it differently. Although various journal submissions specify they use a C-grid, they never mention where they implement certain boundary conditions or why.
Josh is offline   Reply With Quote

Old   June 22, 2010, 04:21
Default
  #2
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
Hi,
I think your ideas to change the AoA are the best.
You can't think to remesh everytime you need to change the angle of attack.
Obviously when the AoA increases, the quality of mesh decreases but if the AoA is not so big it is not a problem.
I think you are studying tubulents flow fields. A way to check the quality of mesh, when you change the AoA, is to verify the y+ value. You will note that, increasing the AoA, also the y+ will increase. When y+ value will go over its desiderable value, you have to remesh.
Let me know!
mach000 is offline   Reply With Quote

Old   June 22, 2010, 12:11
Default
  #3
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Thanks for the response.

I assume that the AoA changes the y+ because y+ is dependent on friction velocity, which is proportional to shear stress, which is proportional to du/dy. As AoA increases, so, too, would the velocity gradient, correct?

I will likely be modelling from 0 < AoA < 12 degrees, since we will be modelling stall in the low Reynolds number flow regime. I'll check my y+ values as I go along. Just out of personal experience, do you think 12 degrees is too large of an angle and that the mesh quality will be significantly affected?

I know from literature that somewhere around 8 degrees, I'll have to switch from steady to unsteady simulations in order to capture the intermittent bursting of the laminar separation bubble. Perhaps I'll switch meshes at that time, too.
Josh is offline   Reply With Quote

Old   June 22, 2010, 12:37
Default
  #4
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
You are right, about y+ but if your simulation is laminar, y+ as no sense.
about the angle of attack, 12 degrees is probably not so big to change the mesh, but i think it depend by the difference between the numerical and experimental, or theoretical results.
About unsteady simulation, obviously, if you need to capture an intermittent phenomenum, you need an unsteady simulation.
You can run steady simulation until the Cl increases. When you notice that it decreases, you can switch to an unsteady simulation
mach000 is offline   Reply With Quote

Old   June 22, 2010, 13:49
Default
  #5
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Thanks for the advice!

I'll be modeling in the transitional regime, so the flow over the airfoil will be laminar to a certain point, then transitioning, then fully turbulent toward the trailing edge.
Josh is offline   Reply With Quote

Old   June 22, 2010, 13:50
Default
  #6
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Also, are my boundary conditions appropriate? I'm not really asking in terms of what they are, but rather where they are. That is, is my periodic condition correct where it is, or should it be extended to the left to cover more of the curved region (therefore reducing the inlet flow area)?
Josh is offline   Reply With Quote

Old   June 22, 2010, 14:07
Default
  #7
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
the BC are the same that I usually use...so I think they could be good.
Transitional simulation, ok. I had some simulation like your some years ago but on a flat plane.
It's not very simple to calculate the transition points on the airfoil. You need to use SST turbulent model and the y+ as to be less than 1
mach000 is offline   Reply With Quote

Old   June 22, 2010, 14:25
Default
  #8
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Yes, my max y+ value will be less than one and I will be using either the SST-SAS model with Gamma Theta Transitioning or the SST-DES model. I have read several papers that produced excellent results with both. The original SST and DES models alone are insufficient for transition prediction in flows with significant amounts of separation. The SST is too diffusive and the DES will fail if the timesteps and grid are insufficiently refined. Conversely, the SST-DES and SST-SAS have a fail-safe - if the gird and/or timestep are too coarse, the model will switch from LES to RANS.
Josh is offline   Reply With Quote

Old   June 22, 2010, 14:34
Default
  #9
Member
 
Ciro Cannavacciuolo
Join Date: Mar 2009
Posts: 35
Rep Power: 8
mach000 is on a distinguished road
if I remember well I used SST-SAS model with gamma theta and I remember well that you have to pay attention to the turbulent level at the inflow
mach000 is offline   Reply With Quote

Old   June 22, 2010, 14:56
Default
  #10
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
You do remember well! The model is extremely sensitive to the freestream (inlet) turbulence due to its reliance on the omega equation for resolving the near-wall flow.
Josh is offline   Reply With Quote

Old   June 22, 2010, 20:01
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,931
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Your AOA approach is fine. Just do a sensitivity study to check that your boundaries are far enough away for the accuracy you require.
ghorrocks is offline   Reply With Quote

Old   June 22, 2010, 21:27
Default
  #12
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Will do. I'll be performing sensitivity checks on the domain size, mesh resolution, mesh quality, freestream turbulence intensity, and the turbulence model and its parameters.

My starting domain has a farfield of 20 chords. According to the literature, that should be sufficient, but I'll be sure to check it.
Josh 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
Structured Airfoil Grid Generator A.S. Main CFD Forum 1 September 30, 2008 18:29
Airfoil boundary condition Frank Main CFD Forum 1 April 21, 2008 18:36
Divergence problem when airfoil exceed pitch angle zonexo Main CFD Forum 2 April 4, 2007 04:22
RANS-Sim. of airfoil: inlet condition of epsilon? Norman Cook Main CFD Forum 3 November 19, 2006 12:30
Grid Independent Solution Chuck Leakeas Main CFD Forum 2 May 26, 2000 11:18


All times are GMT -4. The time now is 07:30.