Convergence and backflow problem in cavitation simulation
 

Hi,

I am running steady, periodic cavitation case for the out-design parameters of a Francis runner. it has 4 million boundary layer mesh (unstructured), all y+ values on the blade are lower than 2. Max aspect ratios in layers are lower than 10000( I read that this is acceptable for boundary layer meshes).

I have two problem. Firstly, my single phase simulations,which are used as initial guess, were converged to 1e-5. However, the cavitation simulations have not converged to 1e-5. Secondly, some runs give backflow in both inlet and outlet, is it normal? if it is not normal, how can i cope with it.

Any help will make me happy!



A wall has been placed at portion(s) of an INLET |
| boundary condition (at 15.8% of the faces, 0.1% of the area) |
| to prevent fluid from flowing out of the domain. |
| The boundary condition name is: R1 Inlet. |
| The fluid name is: Water. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an INLET |
| boundary condition (at 15.8% of the faces, 0.1% of the area) |
| to prevent fluid from flowing out of the domain. |
| The boundary condition name is: R1 Inlet. |
| The fluid name is: Vapour. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 8.1% of the faces, 0.3% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: R1 Outlet. |
| The fluid name is: Water. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead. |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| ****** Notice ****** |
| A wall has been placed at portion(s) of an OUTLET |
| boundary condition (at 8.1% of the faces, 0.3% of the area) |
| to prevent fluid from flowing into the domain. |
| The boundary condition name is: R1 Outlet. |
| The fluid name is: Vapour. |
| If this situation persists, consider switching |
| to an Opening type boundary condition instead.

Most of the time it depends on the cavitation number. but I would say cavitation is not a steady state phenomenon so you have to switch to transient simulation.
The error is not normal at all.

It is not an error. It is a notice. FAQ: http://www.cfd-online.com/Wiki/Ansys...f_an_OUTLET.22

mortazavi is correct, most cavitation models I have done require transient simulations to converge.

Thanks mortazavi and ghorrocks, i know that cavitation simulation consist of 3 runs.

1. steady-state run without cavitation
2. steady-state run with cavitation, used 1 as initial guess
3. transient run with cavitation, used 2 as initial guess

is this wrong?

Additionally, I want to use Entrainment with opening pressure type boundary condition instead of outlet type boundary condition because it provides more convergent results and a run without backflow. However, I am not sure how it resolve the system. should i use it?

You can do it that way. But I would skip 2 and just go straight to 3.

If entrainment converges better and is a good representation of what you are modelling then it sounds like a good choice of boundary condition. The difference between outlet and opening is openings allow back flow. The entrainment option allows flow pulled into the domain to enter at a angle if the flow wants to - the default option only allows flow perpendicular to the boundary.

Thanks ghorrocks

please let us know if you have any progress in convergance.