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

Free surface in mixing vessel

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 22, 2012, 13:46
Default Free surface in mixing vessel
  #1
New Member
 
Germany
Join Date: Aug 2012
Posts: 3
Rep Power: 4
blubb1612 is on a distinguished road
Hi all,
I'm quite new to CFX. I want to simulate the flow in a mixing vessel. It's a steady state simulation. The vessel has no inlet and no outlet. I only set boundary conditions for the walls and an opening boundary condition.
And here is my problem. It's a free surface problem and I don't know which opening boundary condition setting is the best for my problem.

The baffled vessel only contains water. The aim of the simulation is to determine the mixing time, so I want to include a scalar tracer after simulating the steady state flow. Later I also want to include a particle tracking.

I'm very thankful for every hints.
blubb1612 is offline   Reply With Quote

Old   November 22, 2012, 14:01
Default
  #2
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Hi. It sounds like an interesting problem. Have you gone through the relevant CFX tutorials? There are some covering free surface flows, scalar transport, and particle tracking. If you haven't given those a try, you should. If you have some specific problems, post them here.
cdegroot is offline   Reply With Quote

Old   November 22, 2012, 15:33
Default
  #3
New Member
 
Germany
Join Date: Aug 2012
Posts: 3
Rep Power: 4
blubb1612 is on a distinguished road
Thank you for your reply.

I already have done some tutorials concerning this problem...
My problem is that I don't reach convergence. I already read about this problem in relation with free surfaces.
I hope I can get a hint which mass and momentum options for the opening condition I should use to avoid this problem as much as possible. I think the air don't affect the fluid flow very much. On the other side I think it is not possible to model the liquid surface as wall because in this case the fluid flow in the vessel would definitly not be the real one.
blubb1612 is offline   Reply With Quote

Old   November 22, 2012, 15:49
Default
  #4
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
The easiest thing to converge will be if you use a homogeneous model (both water and air share the same velocity field). Start with this. At the top of the domain use an Opening boundary condition with a relative pressure of 0 Pa. Set the volume fraction of air to 1 and the volume fraction of water to 0.
cdegroot is offline   Reply With Quote

Old   November 22, 2012, 15:50
Default
  #5
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Where is this opening boundary condition? Is it at the top of the vessel?

Also, you said you have a free surface problem but your vessel has water only. Do you intend to calculate the free surface position from the pressure level at the top? This might be valid only if the swirl in the fluid isn't too strong, otherwise the free surface height might be important and this simplification might deliver incorrect results. If swirl is not strong, them this can be a good first analysis simplification, but in this case it would be better to use a free-slip wall at the top boundary condition. After you get your results, you can estimate the actual free surface height from the pressure levels.

This simplification is only a good idea if you plan on doing this type of simulation several times and want to cut your total time, in which case I recommend you also do at least one simulation with an actual free surface to check how good your results are and tune your model. If you're only doing one simulation, than just use an actual free surface with the homogeneous model and the free surface algorithm turned on. The computational cost won't be that much higher and your results will be better.

Cheers
brunoc is offline   Reply With Quote

Old   November 22, 2012, 16:00
Default
  #6
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by cdegroot View Post
The easiest thing to converge will be if you use a homogeneous model (both water and air share the same velocity field). Start with this. At the top of the domain use an Opening boundary condition with a relative pressure of 0 Pa. Set the volume fraction of air to 1 and the volume fraction of water to 0.
Hey Chris, looks like you pressed the 'Submit' button before I did

But I agree that an actual free surface simulation with the homogeneous model is the best option.
brunoc is offline   Reply With Quote

Old   November 22, 2012, 16:02
Default
  #7
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Yes definitely do a real free surface simulation! There really shouldn't be any great difficulties getting this to converge.
cdegroot is offline   Reply With Quote

Old   November 22, 2012, 17:04
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Surface waves can often make steady state free surface simulations hard to converge. This simulation does not have inlets or outlets (which are a frequent source of small numerical noise which then become surface waves which cause convergence problems) so that might help a bit.

But in my experience you often have to do free surface simulations in transient simulations and run them out to steady state, rather than doing a steady state simulation.
ghorrocks is offline   Reply With Quote

Old   November 28, 2012, 11:16
Default
  #9
New Member
 
Germany
Join Date: Aug 2012
Posts: 3
Rep Power: 4
blubb1612 is on a distinguished road
Hi,

thank you for your advices.
At the moment I have made a free surface simulation as you described and it works. I have reached convergence.

Now I want to include an additional variable to simulate mixing times.
Therefore I definied an expression for the injection of the tracer: Tracerinjection=0.1*step((t-0.1[sec])/1 [sec]) [kg s^-1]
Because I had no inlet in my vessel I have defined a source point where I include the tracer.

I run this simulation as transient and set 'solve fluids', 'solve ernergy' and 'solve tubulence' to false. I use the result file from the steady state simulation as initial value. Is that right?
I have defined some monitor points. For this points I get a pulse response curve which I should analyse to get the mixing time. But the results are not these I predicted. There is a first peak and some smaller ones after that but it doesn't reaches a constant value at the end.

Are there any advices concering this problem with the additional tracer.
blubb1612 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
Thermocapillary free surface flow zakifoam OpenFOAM Running, Solving & CFD 6 August 24, 2014 03:24
free surface model sjtusyc CFX 3 September 5, 2012 18:33
governing equations for liquid mixing with free surface? phsieh2005 Main CFD Forum 3 October 6, 2009 20:37
curve of vortex of free surface in mixing tank bioman66 CFX 1 June 30, 2006 06:19
Modeling Free Surface Flows Elliot Schwartz Main CFD Forum 5 August 25, 1998 21:03


All times are GMT -4. The time now is 19:10.