Symmetry Boundary Condition for Flow Past a sphere
 

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

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.

For turbulent regime, you could apply symmetry BC.s only using RANS

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.

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.

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

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.

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?

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 :D

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 1m² and the projected surface of your computational domain is lets say only 10m², 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.

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?:)

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 :o

Okay. Got it. Thanks a lot. :)