[jackss]

I am trying to determine my timestep size in ansys fluent for a transient flow through a pipe. I am uncertain about something; do I need the cube root of the max volume in the cell or to i need these values in the picture? Can someone kindly help me here pleasee!

N.B. I am using the LES solver

[aero_head]

Hello Jack,

From what I have read on the forums, a good rule of thumb is to set time step size < delta_x/u
where delta_x is the smallest cell size and u is the velocity. So you can use the reported min. cell size in your photo divided by the velocity.

Here is some information from Far on this thread: How to determine time step size and Max. iterations per time step.

First few general rules:

1. It is better to lower the time step instead of increasing the no of iterations

2. Lowering the time step will enhance convergence.

3. Use better initial conditions (get from steady state solution)

4. If you experience difficulty in getting convergence for desired time step, use lower time step for initial transients. once you get good convergence gradually increase time step to required value.

5. Adaptive time stepping will give you faster and automatic transient simulation to desired time step.

6. Use 2nd order implicit scheme.


Now few situations:

1. LES, explicit and implicit schemes.

For LES, the condition for time step selection is based on cournt number and CLF < 0.2. For explicit scheme, used when you have advantage of faster convergence for flows where flow delta T is of same order as dictated by CFL otherwise use implicit scheme.

For explicit scheme delta T is determined by CFL < 1 by stability constraint.

For implicit scheme delta T is determined by the flow feature you are interested in.

[jackss]

Hey thanks so much for responding. Can you further explain what you are saying with the LES flows ? Note that I am working with a 3D model. Say my velocity is around 100m/s , and say my minimum element size is 2mm, then solving for delta T ( with CFL=1), then a suitable time step size would be 2e-5 ? Kindly correct me if i'm wrong please, i reallly need the help, thanks !

[aero_head]

Hello Jack,

From my last post, for LES flows, the timestep would depend on if you are using an implicit or explicit scheme. A common guideline for LES is to keep the CFL number below 1.0. You can find even more rigorous guidelines recommending CFL ~ 0.5. The CFX manual also recommends this range. From one of ghorrocks' posts, I recall him saying LES simulations will resolve the turbulent eddies to the level of the inertial sub-range. Therefore you need to resolve to this same range and then filter out the inertial sub-range. LES can be pretty tricky.

Your timestep seems good to me, I have run similar simulations to yours using a similar timestep.

Again, it's just a starting point. Usually, it is good use 1/20 of the expected characteristic period as the timestep. After a first simulation, you could then vary the timestep and check if there is any influence on the solution, to be sure that you have achieved a solution independent of the timestep.

[jackss]

Hey, I have been working on this still. I was able to get some okish results for my model. I am simulating flow through a pipe. For the low velocities, around 60 m/s, the results were goodish based on the formula we discussed etc. However, at the higher velocities around 150 m/s, I am not getting good results at all. Can you suggest anything that I may try ? Or is there something that I am doing wrong ?


For some more info:
My mesh is tetrahedrals with about 40 inflation layers. The CFL number is around 1 i guess because i used this equation (CFL=(ct)/x=1) when choosing timestep size and mesh size. The diamter is around 73mm . Can you suggest anything ? I tried the brick elements but I wasnt getting good results at all...

[FMDenaro]

Originally Posted by jackss

Hey, I have been working on this still. I was able to get some okish results for my model. I am simulating flow through a pipe. For the low velocities, around 60 m/s, the results were goodish based on the formula we discussed etc. However, at the higher velocities around 150 m/s, I am not getting good results at all. Can you suggest anything that I may try ? Or is there something that I am doing wrong ?


For some more info:
My mesh is tetrahedrals with about 40 inflation layers. The CFL number is around 1 i guess because i used this equation (CFL=(ct)/x=1) when choosing timestep size and mesh size. The diamter is around 73mm . Can you suggest anything ? I tried the brick elements but I wasnt getting good results at all...

One of the reasons for problems in LES is that the stability constraint is influenced also by the eddy viscosity model. I suggest to use smaller time steps.

[jackss]

smaller time step size ? I have been using a smaller time step size, but results seem to be similar , therefore it is not helping the solution. Any thing again ?

[FMDenaro]

without details is not possible to understand your problem... are we talking about a numerical instability issue? Or you are not satisfied by the final results?

[jackss]

Not satisfied with the final results, please let me know what info you need

[FMDenaro]

Originally Posted by jackss

Not satisfied with the final results, please let me know what info you need

And among the different parameters governing an LES solution why are you focusing your attention on the time step?