CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Convergence and backflow problem in cavitation simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 9, 2016, 07:38
Default Convergence and backflow problem in cavitation simulation
  #1
New Member
 
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 3
burakaltintas is on a distinguished road
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.
burakaltintas is offline   Reply With Quote

Old   August 9, 2016, 12:51
Default
  #2
Member
 
Join Date: Jun 2009
Posts: 53
Rep Power: 10
mortazavi is on a distinguished road
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.
mortazavi is offline   Reply With Quote

Old   August 9, 2016, 20:03
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,853
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 11, 2016, 04:08
Default
  #4
New Member
 
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 3
burakaltintas is on a distinguished road
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?
burakaltintas is offline   Reply With Quote

Old   August 11, 2016, 06:02
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,853
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 11, 2016, 06:21
Default
  #6
New Member
 
Burak Altıntaş
Join Date: Apr 2016
Posts: 6
Rep Power: 3
burakaltintas is on a distinguished road
Thanks ghorrocks
burakaltintas is offline   Reply With Quote

Old   August 11, 2016, 10:00
Default
  #7
Member
 
Join Date: Jun 2009
Posts: 53
Rep Power: 10
mortazavi is on a distinguished road
please let us know if you have any progress in convergance.
mortazavi is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
2D Hypersonic Inlet in FLUENT - Convergence Issues Fraisdegout FLUENT 6 December 15, 2016 03:07
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


All times are GMT -4. The time now is 14:00.