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

Symmetry Boundary Condition for Flow Past a sphere

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

Like Tree6Likes
  • 2 Post By FMDenaro
  • 1 Post By flotus1
  • 1 Post By flotus1
  • 1 Post By flotus1
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 4, 2018, 22:53
Default Symmetry Boundary Condition for Flow Past a sphere
  #1
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Hi, I am simulating a case which there is a flow past a sphere and I want to know the drag coefficient on the sphere. Wanna know that if i use a quarter of sphere with symmetry boundary condition, will the flow field and the drag coefficient i get is same as the full sphere. I am confused because in certain range of Reynolds Number, there will be vortex shedding and somehow the flow field will not be symmetry (I guess?). Looking for some opinions thanks
Qkarl is offline   Reply With Quote

Old   March 5, 2018, 02:29
Default
  #2
New Member
 
Ali Berk Kahraman
Join Date: Dec 2015
Location: Istanbul, Turkey
Posts: 11
Rep Power: 9
abkahraman is on a distinguished road
The flow around the sphere is supposed to be axisymmetric if there is no turbulence or vortex shedding. So, if you know 100% that you will be operating below Re of vortex shedding, you should be fine. Still, I am not sure about this, so make sure to benchmark your results with the experimental papers on the literature.
abkahraman is offline   Reply With Quote

Old   March 5, 2018, 04:06
Default
  #3
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,257
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
For turbulent regime, you could apply symmetry BC.s only using RANS
FMDenaro is offline   Reply With Quote

Old   March 5, 2018, 06:38
Default
  #4
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Hi,

For my case, i will run the simulation with a wide range of Reynolds number (100-10^5), i guess it will be in the shedding region.

Can i know what do u mean by RANS model? I am doing a student project and just will simulate my case in k-w SST model. So is it okay for me to use symmetry BC?

Thanks in advanced
Qkarl is offline   Reply With Quote

Old   March 5, 2018, 06:45
Default
  #5
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,257
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by Qkarl View Post
Hi,

For my case, i will run the simulation with a wide range of Reynolds number (100-10^5), i guess it will be in the shedding region.

Can i know what do u mean by RANS model? I am doing a student project and just will simulate my case in k-w SST model. So is it okay for me to use symmetry BC?

Thanks in advanced
RANS is a statistical formulation for the NS equations. It is a steady state solution for the ensemble averaged field.
However, by definition, you cannot see the vortex shedding by using RANS.
juliom and Qkarl like this.
FMDenaro is offline   Reply With Quote

Old   March 5, 2018, 07:01
Default
  #6
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,209
Rep Power: 44
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
And your k-w SST model falls in the RANS category.
If you are using Fluent, you can also use an axisymmetric 2D model instead of some portion of a 3D model with symmetry BC. Saves time and/or allows for higher resolution.
Qkarl likes this.
flotus1 is offline   Reply With Quote

Old   March 5, 2018, 08:20
Default
  #7
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Hi,

This is my simulation for a full sphere with a Reynolds number of 10^5 with turbulence model k-w SST in steady state.
From the velocity vector, it seems like the flow field is not symmetry. I'm confused about it as I know k-w SST should be RANS model. Please give me some enlightenment thanks
Attached Images
File Type: png 28721614_10213250988967918_1782576949_n.png (93.7 KB, 32 views)
Qkarl is offline   Reply With Quote

Old   March 5, 2018, 08:38
Default
  #8
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,209
Rep Power: 44
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
RANS-solvers often have problems finding the steady-state solution for this case. This is due to the slow, large-scale vortex shedding behind bluff bodies like spheres. In terms of time-scale and size, they differ greatly from the turbulent eddies a RANS approach is supposed to suppress/model. Hence many RANS-solvers can not handle them very well. A 2D axisymmetric case would be a workarund. Or running an unsteady RANS or even LES simulation instead, but this might be beyond the scope of a student project. Especially if you want to simulate a wide range of Reynolds numbers.
By the way: unless your simulation is supposed to simulate a confined sphere, move the side-walls further away from the sphere and apply symmetry boundary conditions to them.
flotus1 is offline   Reply With Quote

Old   March 5, 2018, 08:51
Default
  #9
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Actually now I am trying to find out the drag coefficient on the sphere when a flow past through it and compare with the theoretical value. What I need is just the drag coefficient and maybe some turbulence effect which result smaller wake region and reduction on the pressure drag. after that, i will try to simulate flow past a golf ball. i knew that using RANS model somehow might not get an accurate result for the golf ball case due to the small vortices induce. But for both the sphere and golf ball case, does the symmetry boundary still can apply and will it affect the drag coefficient i get?
Qkarl is offline   Reply With Quote

Old   March 5, 2018, 09:02
Default
  #10
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,209
Rep Power: 44
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
This really sounds like you should move the lateral boundaries further away to reduce blockage effect. And make them symmetry instead of wall.
Yes, as long as you are using a RANS approach you can simulate a slice of the 3D model and apply symmetry boundary conditions to the new computational boundaries. This should even help your solver finding the symmetrical solution.
Qkarl likes this.
flotus1 is offline   Reply With Quote

Old   March 5, 2018, 10:01
Default
  #11
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
This really sounds like you should move the lateral boundaries further away to reduce blockage effect. And make them symmetry instead of wall.
Yes, as long as you are using a RANS approach you can simulate a slice of the 3D model and apply symmetry boundary conditions to the new computational boundaries. This should even help your solver finding the symmetrical solution.
"This really sounds like you should move the lateral boundaries further away to reduce blockage effect. And make them symmetry instead of wall."

Can you further explain this? I am not really understand. Sorry for stupid question
Qkarl is offline   Reply With Quote

Old   March 5, 2018, 10:15
Default
  #12
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,209
Rep Power: 44
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
I assume that you want to compare your results to the results for the flow around an unconfined sphere. These are the results you usually find in literature unless the source explicitly states that the flow had some kind of confinement.
If your sphere has a projected surface of 1mē and the projected surface of your computational domain is lets say only 10mē, the flow around the sphere is significantly accelerated due to the blockage effect. Blockage ratio in my example is 10%. instead of 1m/s at the inlet, the flow around the sphere now has an average velocity of 10/9 m/s. This will introduce a systematic error to the drag coefficient you find.
Even worse than that, the additional acceleration could change the nature of the flow, e.g. change the position of the separation point. So simply changing the reference velocity to account for blockage will not be sufficient.

For simulations of high-Re external flows where the physical setup is unconfined, a blockage ratio of 2% or less is good practice if you don't want to do a sensitivity analysis. For very low Reynolds numbers you might even need less. Using wall boundary conditions on the outer walls instead of symmetry only makes things worse because the flow in the core is accelerated even more.
piu58 likes this.
flotus1 is offline   Reply With Quote

Old   March 6, 2018, 02:21
Default
  #13
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Hi, just did some finding in the blockage ratio. So, now i should/can conduct my simulation with quarter of the sphere with the blockage ratio less than 2% which mean the inlet surface should at least 50x larger than the projected area of my quarter sphere. Then, all of the 4 side walls should set at symmetry BC. Am i right?
Qkarl is offline   Reply With Quote

Old   March 6, 2018, 04:11
Default
  #14
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,209
Rep Power: 44
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
Correct.
And instead of a rectangular domain, I would rather use a cylindrical domain. This will yield better results if you ever need to use block-structured aka "structured" grids. But i am probably nit-picking here
Qkarl likes this.
flotus1 is offline   Reply With Quote

Old   March 6, 2018, 04:32
Default
  #15
Member
 
Join Date: Apr 2017
Posts: 32
Rep Power: 7
Qkarl is on a distinguished road
Okay. Got it. Thanks a lot.
Qkarl 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
Problem in setting Boundary Condition Madhatter92 CFX 12 January 12, 2016 05:39
Time dependant pressure boundary condition yosuke1984 OpenFOAM Verification & Validation 3 May 6, 2015 07:16
CFX fails to calculate a diffuser pipe flow shenying0710 CFX 7 March 26, 2013 05:13
meshing F1 front wing Steve FLUENT 0 April 17, 2003 13:37
Regarding SYMMETRY boundary condition Praveen Athanki FLUENT 0 March 27, 2000 14:30


All times are GMT -4. The time now is 12:13.