[shovaliye2]

hi. I want to simulate flow around hydrofoil.

type of solver is pressure based and transient, realizable k-e model with standard wall functions.

can you help me how to choose proper magnitudes of time step size, number of time steps and max iteration/time step? I'm new in CFD and ansys fluent.

also I have another question? should I change flow courant number in controls? the flow courant number is 200 and transient formulation is first order implict.

[vinerm]

Time-step depends on many factors, such as, Courant number. This is not same as the Courant number for which default value is 200. You can leave that at 200. Other important factor for flow around bodies is Strouhal number. If this is know for the foil, then you can determine the minimum time-step required. Otherwise, just look at the number of cells in the streamwise direction over the foil. Then determine the time required for the freestream to go from head to tail of the foil. The ratio of this time to the number of cells across the chord of foil gives you the time required by the flow to cross each cell. Ensure that the time-step is always smaller than this time-step. Number of time-steps have to be enough to ensure that the free-stream passes over the foil atleast five times.

[shovaliye2]

Originally Posted by vinerm

Time-step depends on many factors, such as, Courant number. This is not same as the Courant number for which default value is 200. You can leave that at 200. Other important factor for flow around bodies is Strouhal number. If this is know for the foil, then you can determine the minimum time-step required. Otherwise, just look at the number of cells in the streamwise direction over the foil. Then determine the time required for the freestream to go from head to tail of the foil. The ratio of this time to the number of cells across the chord of foil gives you the time required by the flow to cross each cell. Ensure that the time-step is always smaller than this time-step. Number of time-steps have to be enough to ensure that the free-stream passes over the foil atleast five times.

can I divide smallest cell size to freestream velocity in order to obtain time step?

[vinerm]

Yes, you can do that. Do note that you need to divide length along the freestream or an average size of the cell, not its volume.

[shovaliye2]

how can I find smallest cell size?

in setup of fluent I click on check mesh and this was the result:


Is this correct to calculate (minimum volume)^(1/3) for smallest cell size? or I have to use another method?

I did this and then divide that magnitude to 4.0092 which is flow velocity.


sorry for my questions, I am amateur in fluent and CFD and I really need to do this project.

[vinerm]

Usually, no one goes into this much detail. You can try with a time-step based on number of cells in the freestream direction and the freestream velocity. If you want to use cell size, then it is better to look at the distribution of the cell size. If you use minimum cell size, it is quite possible that the time-step turns out to be quite small. So, initialize the case, and then go to Plots > Histogram and then plot histogram of cell volumes. Look at the distribution. Pick up a volume that represents an average or median cell size. You can take cube root provided the cells are hexahedral. If those are tetrahedral then you have to take cube root of 72 times the volume.

Essentially, there is no fixed method. Most of the time, we work based on our experience. Start with a time-step that appears good for the case and then check if the solution is converging within 20-30 iterations in each time-step. If it is not, reduce the time-step, if it converging in less than 5 iterations, then increase the time-step. Fluent has an adaptive algorithm, you may try that as well.