Hello all.

I am using the K-E Low Reynolds Number (my Reynolds number is 3109) for my turbulence modeling. I have a pressure boundary and a fixed flow outlet boundary.

When defining boundary conditions at the pressure boundary, I have two options as far as turbulence goes: TE/Length, or Zero Grad. I do not have to supply any values when I choose Zero Grad. I have to supply two values when I select TE/Length: Turb. Intensity, and length scale.

This poses three questions for me:

What is the difference between the two options? Which one should I pick?

As for the TE/Length, what are turb. intensity and length scale, and what are appropriate values for them?

Thanks for any help

Cheers

Hello Ben,

I hope you choose the low Re turbulent model because your mesh is fine enough to have a y+ near 1 and not because Re = 3109.

HV

What is y+ ?

hi ben

y+ = friction velocity * wall distance / dynamic viscosity

y+ is a criterion to decide whether to use low or high reynolds number turbulence model modification because of their different near wall treatment. hi-re model makes use of wall functions which treat the near wall velocity profile as a logarithmic function (simply said) of y+. low-re modification is a bit more complex and makes use of additional sources to dump velocity near the wall.

the first approach leads to less cells needed within a computational domain because the y+ can be in a range of 30 to 500 and y+ is taken in the cell adjacent to the wall. the second one is more strict regarding y+ which has to be bellow 1. this fact causes significantly larger number of cells is required. this model is worth using when heat transfer is to be solved.

regarding your first problem with t/l or zero grad option: if you provide any values (t/l) these will be used in case of backflow at the boundary. if you set zero gradient then values required for proper definition of boundary condition will be taken from the cells adjacent to the boundary.

hope this will help you but more information is in manuals and literature

www.cfd-online.com/Books/ could tell you more

good luck

Ben, there is a little bit of explanation about turbulence modeling in star at their website, www.adapco-online.com. Under the feature article menu on the left hand side is a small write up on turbulence. Further down under User Services is a section labeled FAQ. In it they have a small write up on how to estimate y+. Unfortunately, adapco has not updated this site in awhile (except to take out the user forum section), so it doesn't cover all the turbulence models available in the latest vesion of star.

The star-cd Methodology manual in chapter 6 gives a little guidance for turbulence intensity and mixing length. For fully developed pipe flow turbulence intensity is on the order of 0.01 and mixing length is at least an order of magnitude smaller than the characteristic dimension of the cross section.

Tom

Could I safely use the Zero Grad. option for turbulence modeling? This way, I don't have to specify intensity or length scale, the code will calculate it, or so I'm told.

Thanks, Tom.

Ben

Hello, Ben

I would like to be sure that you choose the low-Re model not because your Re is 3109 but because your mesh is enough fine near the wall to use it.

You could find some information about low-Re model in the user guide.

HV

Fine enough along the flow direction, or perpendicular to the flow direction?

How do I know if it is fine enough? I didn't find the user guide very helpful.

Thanks for the help.

Ben

Perpendicular to the flow direction. By experience, you could know if your mesh is fine enough to use the low-Re model.

You use a low-Re model when y+ (it is in fact a local Re number near a wall)is low not because the "global" Re is low.

I think for your case that a high-Re model is enough.