CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

How to properly set up an opening in buoyancy driven problems

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

LinkBack Thread Tools Search this Thread Display Modes
Old   July 21, 2014, 11:31
Default How to properly set up an opening in buoyancy driven problems
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 14
lavoz is on a distinguished road
Dear forum members,

I'm trying to setup an opening being the only boundary beside walls in a completely fluid domain. The fluid's density is independent of pressure but temperature sensitive. So I'm dealing with a buoyancy driven problem, the smooth no slip walls are defined with a heat transfer coefficient and an outside temperature lower than the initial domain temperature.

How to setup the opening? Due to temperature expansion, fluid will enter and exit through the same boundary, so an Opening should be my option of choice. For mass and momentum I chose Entrainment with a Relative pressure of 0 Pa and the Pressure Option set to Opening Pressure. For Turbulence I chose Zero Gradient and for Heat Transfer I chose an Opening Temperature equal to the initial domain temperature.

Concerning the buoyancy, I set the reference pressure also to 0 Pa and the reference density to an value between the density at the initial and opening temperature and the density at the outside temperature of the walls.

I constantly run into c_fpx_handler: Floating point exception: Overflow so I'm very grateful for any helpful suggestions.

Almost forgot, my mesh is high quality (4.4e+06 hexahedrons, block structured in ICEM) and the analysis type is transient, initial time step was set from 1e-09s to 1e-01s, all resulting in overflow. The attached image shows the fluid domain mostly covered by (cooling) walls marked in green and the opening with hemisphere shape colored grey supplying hot fluid. Gravity acts in negative y-axis direction.
Attached Images
File Type: jpg fluidDomain.jpg (26.2 KB, 28 views)

Last edited by lavoz; July 21, 2014 at 14:40. Reason: The usual, I forgot something
lavoz is offline   Reply With Quote

Old   July 22, 2014, 06:11
New Member
Join Date: Dec 2013
Posts: 5
Rep Power: 10
wang is on a distinguished road
i think there may be something wrong with your reference pressure ,it should be not 0pa,you can try 1 atm(101325pa).
wang is offline   Reply With Quote

Old   July 23, 2014, 03:46
Default No one with any (other) suggestions?
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 14
lavoz is on a distinguished road
First of all, thank you for your response.

Unfortunately, your suggestion did not help with my problem. Since the density of my fluid isn't pressure dependent, I didn't think that the buoyancy reference pressure would make any difference.

For additional information, I attached the solver's output file. As mentioned before, the mesh is still of descent quality, in the meanwhile I reduced the mesh density for a quicker trial and error process.
Attached Files
File Type: txt CFX_solverOutput.txt (40.3 KB, 7 views)
lavoz is offline   Reply With Quote

Old   July 23, 2014, 04:41
Senior Member
Matthias VoŖ
Join Date: Mar 2009
Location: Berlin, Germany
Posts: 449
Rep Power: 18
mvoss is on a distinguished road
The whole domain is filled with fluid? The sphere acts like a basin and the fluid gets sucked into the tank-like structure?
mvoss is offline   Reply With Quote

Old   July 23, 2014, 05:44
Default Clarifications
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 14
lavoz is on a distinguished road
Exactly, the entire domain is fluid (oil, temperature dependent but pressure independent material properties). Everything marked green is wall thatís cooling down the fluid (with decreasing temperature the density increases resulting in a volume reduction compensated by the opening).

The half sphere at the bottom acts like a source of hot fluid and Iím interested how much fluid is circling around in a steady state. The initial conditions of the fluid are not important to me, Iím not interested on how the steady state is reached.
lavoz is offline   Reply With Quote

Old   July 23, 2014, 07:06
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,231
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Some comments:

* Your material properties do not have a continuous derivative. This often causes convergence difficulties. If you round off the discontinuous bits that can help convergence.
* Set your initial and minimum time step to 1e-10[s]. If it needs small time steps let it use them. If will automatically increase them if it can.
* Why do you run for 10 time steps? Make that lots to run to convergence. But I suspect this is just for development.
* Your boundary location is too close to the flow feature. You will need to move it back to somewhere the flow is simpler.
* I think you will find the pipe to the closed reservoir does not play any significant part in the final steady solution. So I would not bother modelling it.
* I doubt there is a steady solution for this anyway. It will probably be a periodic flapping flow.
* You have a tight conservation target (1e-3). Are you sure you need it this tight? Usually if you are using a transient simulation to march to a steady solution you use loose criteria to do the time steps quickly. It should start converging as you approach a steady result, or you might have to tighten it as you approach it.
* Consider making a coarser mesh to do this development work on. Once you have the basic model working remesh to a finer mesh for accuracy.
ghorrocks is offline   Reply With Quote


buoyancy flow, opening boundary

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Buoyancy Driven Flow sunilpatil CFX 1 March 19, 2013 05:38
Installation problems indy OpenFOAM Installation 7 April 3, 2009 10:40
Install problem in linux navaladi OpenFOAM Installation 11 July 17, 2008 03:24
Installation problems shellbell1999 OpenFOAM Installation 9 April 6, 2006 14:29
OpenFOAM installation on SUSE92 problems derath OpenFOAM Installation 1 April 3, 2006 07:44

All times are GMT -4. The time now is 03:52.