[Sakun]

Hi everyone,

I have some doubts regarding time step calculations and i am using CFL = (u * Δt/Δx) formular. I use CFL number as 1 , for u i am using 383.9 m/s but Δx is what confusing me. According to some resources Δx represent the meaning of ,characteristic length, x direction cell length, minimum grid size, and cell length. So I don’t know what definition to choose in this case.

My Δx, Δy, and Δz mesh sizes around my blade (wall) are below,

∆Y 1.66E-06m (Y+ = 1)

∆X 1.99E-04m (X+ = 120)

∆Z 4.98E-05m (Z+ = 30)

So, what value should i use for my time-step calculations ?

Also, i have seen some people are using cube root method as well, can someone explain this method as well, and are there any other methods that ANSYS has recommended to calculate time-step ?



Highly appreciate for the guidance.

[LuckyTran]

Keep in mind the Courant number is a field, not just one value. These are just suggestions to calculate the limiting Courant number. If you are absolutely lost, then just calculate the Courant number in every cell using the local L and local U and find the worst Courant number.
Each cell has a Courant number that goes by the local velocity u and local cell size dx. But your stability limit is determined by the cell with the highest Courant number (i.e. the weakest link in the chain). So the limiting Courant number will go like dx.
Cube root method is used because for a grid of polyehdral cells, there isn't a well defined connectivity in any particular direction to get dx of each cell. It is a waste of time to calculate dx just for the purpose of computing a Courant number which you don't really need to solve the physics so they use cube root as a surrogate.
Courant number also needs to be done with the 3D velocity vector u,v,w and summed over dx,dy,dz and cube-root is another way to quickly get a length scale

[Sakun]

Originally Posted by LuckyTran

Keep in mind the Courant number is a field, not just one value. These are just suggestions to calculate the limiting Courant number. If you are absolutely lost, then just calculate the Courant number in every cell using the local L and local U and find the worst Courant number.
Each cell has a Courant number that goes by the local velocity u and local cell size dx. But your stability limit is determined by the cell with the highest Courant number (i.e. the weakest link in the chain). So the limiting Courant number will go like dx.
Cube root method is used because for a grid of polyehdral cells, there isn't a well defined connectivity in any particular direction to get dx of each cell. It is a waste of time to calculate dx just for the purpose of computing a Courant number which you don't really need to solve the physics so they use cube root as a surrogate.
Courant number also needs to be done with the 3D velocity vector u,v,w and summed over dx,dy,dz and cube-root is another way to quickly get a length scale

Thank you very much indeed for your well explained reply LuckyTran,

My mesh is hexahedral and will the cube root method suitable for this case as well ?
If so, do i have to take the minimum volume value (2.52781e-15) from the volume stats in fluent (attached picture) to cube root [ (2.52781e-15)^(1/3) ] and substitute that for dx in the CFL number formula (CFL = [u * Δt/Δx]), in order to find Δt?
(Correct me if i am wrong )

Regards,

[LuckyTran]

You really don't need to go through all this trouble. Just start the simulation and then Fluent has a Courant number field. All these formula are just to steer you in the correct direction.

The minimum volume is not necessarily the limiting cell because it could be a near-wall cell where the velocity is 0. Really there is no general answer, only you know where your mesh is small and large and what the velocity in each cell is.

A mesh where the smallest cell is 6 orders of magnitude smaller than the largest cell is probably a terrible mesh, but hey, you do you. Still, that shouldn't distract you from the fact that Fluent will tell you exactly what the Courant number is in each cell.

[Sakun]

Originally Posted by LuckyTran

You really don't need to go through all this trouble. Just start the simulation and then Fluent has a Courant number field. All these formula are just to steer you in the correct direction.

The minimum volume is not necessarily the limiting cell because it could be a near-wall cell where the velocity is 0. Really there is no general answer, only you know where your mesh is small and large and what the velocity in each cell is.

A mesh where the smallest cell is 6 orders of magnitude smaller than the largest cell is probably a terrible mesh, but hey, you do you. Still, that shouldn't distract you from the fact that Fluent will tell you exactly what the Courant number is in each cell.

Thank you very much again for your reply,

Actually i cannot begin the simulation without calculating the time-step size, so that is why i am kind of lost in determining the Δx in CFL formula .

Regards,