[Crane_]

Hello everyone, I meet some troubles during my simulation of oscillatory flowing around cruciform cylinders.
I have simulated single cylinder in oscillatory flow successfully，whose length is 4D(D is the diameter of cylinder). Then I keep all the other conditions same, and simulated two cylinders (the lengths are 10D) in the form of a cross. However, it always stops running because the time step becomes too short during the simulating. At the beginning, I think it is caused by the mesh size, so I try to change the mesh size, including increasing the thickness of the first layer of grid on the cylinder surface and over all grid size, but it is useless.
I don't know what else might be wrong. I would appreciate it if someone could give me some advice. Please let me know if there is any information I need to provide.
Thanks.

[JulioPieri]

This kind of problem is usually caused by bad set-up and boundary conditions. Run using PISO instead of PIMPLE and check that your solution will likely diverge sooner.

Check your BCs, parameters and schemes.
Also, write smaller timesteps results and open them in paraview. See that velocity/pressure will likely be increasing a lot at some places in the mesh.

[Crane_]

Originally Posted by JulioPieri

This king of problem is usually caused by bad set-up and boundary conditions. Run using PISO instead of PIMPLE and check that your solution will likely diverge sooner.

Check your BCs, parameters and schemes.
Also, write smaller timesteps results and open them in paraview. See that velocity/pressure will likely be increasing a lot at some places in the mesh.

Thanks very much for your kind reply. I tried to chang the div(phi,U) from Gauss cubic to Gauss limitedLinearV 1 and decreased the initial timestep from 0.001 to 0.0001, and it works successfully now.
However, some other errors still exist. I observed the running image in paraview. It is found that in the outlet half of the computing domain, the speed image is very strange, while in the inlet half, everything is ok. What might be the reason?

[JulioPieri]

This is typical in bad setup of BCs. You might be using some bad set of BCs.
Use upwind scheme first, before choosing higher order.

Did your first case, with 4D run smoothly? The results were ok?
Double check your boundary conditions to see if the 10D case is the same.

zip your case, I can take a look at it

[Crane_]

Originally Posted by JulioPieri

This is typical in bad setup of BCs. You might be using some bad set of BCs.
Use upwind scheme first, before choosing higher order.

Did your first case, with 4D run smoothly? The results were ok?
Double check your boundary conditions to see if the 10D case is the same.

zip your case, I can take a look at it

My 4D case ran smoothly and the force coefficients results agreed well with other's results.
The follow zip file is my case. Thank you very much for your help.

[JulioPieri]

Hello, here are my observations:

1) The cyclic boundary condition is a very troublesome one. Since you have cyclic on every side, the flow is excessively free to move. Try switching to symmetry BC, as it constrains the normal velocity, likely stabilizing the simulation. Consider using wall as well. I believe it wouldn't affect your case, since you (probably) trying to look close to the cylinders, right? 10D away from boundary is far enough from wall BC as well.

2) your patches are cyclicAMI and your bc is cyclic. Is it even running? OpenFOAM usually complains when the setup is like this.

3) You are running straight LES case? Try firs running laminar, then some RAS model and see if the case goes. This is the usual strategy: first run it simple, then add complexity gradually.

4) Are you sure of all your fvSchemes and fvSolutions entries? You seem to have a lot more stuff than the solver is using. But since it's a custom solver, it might use it, I don't know.. This doesn't affect the solution, but it points that the file is being copied from other cases, bundling up hypothesis that may make it hard to find any error. I'd start a fresh file if the previous suggestions don't work.


Hope this helps.

[Crane_]

Originally Posted by JulioPieri

Hello, here are my observations:

1) The cyclic boundary condition is a very troublesome one. Since you have cyclic on every side, the flow is excessively free to move. Try switching to symmetry BC, as it constrains the normal velocity, likely stabilizing the simulation. Consider using wall as well. I believe it wouldn't affect your case, since you (probably) trying to look close to the cylinders, right? 10D away from boundary is far enough from wall BC as well.

2) your patches are cyclicAMI and your bc is cyclic. Is it even running? OpenFOAM usually complains when the setup is like this.

3) You are running straight LES case? Try firs running laminar, then some RAS model and see if the case goes. This is the usual strategy: first run it simple, then add complexity gradually.

4) Are you sure of all your fvSchemes and fvSolutions entries? You seem to have a lot more stuff than the solver is using. But since it's a custom solver, it might use it, I don't know.. This doesn't affect the solution, but it points that the file is being copied from other cases, bundling up hypothesis that may make it hard to find any error. I'd start a fresh file if the previous suggestions don't work.


Hope this helps.

Hello, thanks for your reply.
I chose the cyclic boundary based on other's literature and now I think I need to try switching to symmetry BC. The cyclicAMI BC was not used in my case because I didn't use the command 'createPatch', and it was only an attempt in my past. For the fvSchmes and fvSolutions entries, I really don't know them very well now. I need to learn them.
I'm really lucky to get these experience from you.