|
[Sponsors] |
Convergence and backflow problem in cavitation simulation |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
|
August 9, 2016, 07:38 |
Convergence and backflow problem in cavitation simulation
|
#1 |
New Member
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 10 |
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. |
|
August 9, 2016, 12:51 |
|
#2 |
Member
SMN
Join Date: Jun 2009
Location: CANADA
Posts: 71
Rep Power: 16 |
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. |
|
August 9, 2016, 20:03 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,718
Rep Power: 143 |
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. |
|
August 11, 2016, 04:08 |
|
#4 |
New Member
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 10 |
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? |
|
August 11, 2016, 06:02 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,718
Rep Power: 143 |
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. |
|
August 11, 2016, 06:21 |
|
#6 |
New Member
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 10 |
Thanks ghorrocks
|
|
August 11, 2016, 10:00 |
|
#7 |
Member
SMN
Join Date: Jun 2009
Location: CANADA
Posts: 71
Rep Power: 16 |
please let us know if you have any progress in convergance.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
2D Hypersonic Inlet in FLUENT - Convergence Issues | Fraisdegout | FLUENT | 6 | December 15, 2016 02:07 |
Convergence and backflow problem in cavitation simulation | burakaltintas | CONVERGE | 2 | August 9, 2016 07:42 |
Buoyancy issue in free and forced convection problem | sosat1012 | CFX | 4 | June 4, 2015 11:12 |
Backflow at outlet in a Eulerian gas-solid simulation | audrey | CFX | 10 | October 25, 2012 06:15 |
Modeling Backflow for a 3D Airfoil (Wing of Finite Span) | Josh | CFX | 9 | August 18, 2009 11:31 |