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

Free surface flow in counter current limitation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2013, 10:57
Default Free surface flow in counter current limitation
  #1
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
Hello, I am trying to do a simulation of 2 flows (water and air) flowing counter currently in a horizontal hot leg. I have problems of convergence with steady state, so now I am trying a transient one. I have defined constant velocity inlets for both water and air, an outlet for the water with pressure condition, and an opening for the air. Even with the transient simulation, it is becoming really hard to get convergence. Can you give me any advice? I have selected a 1ms timestep. Thanks.
j.zamorano is offline   Reply With Quote

Old   April 17, 2013, 19:48
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Please post an image of what you are modelling and the CCL or output file.
ghorrocks is offline   Reply With Quote

Old   April 22, 2013, 04:52
Default
  #3
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
http://www.subirimagenes.com/otros-f...-8398648.html][/URL]

Left: air constant velocity inlet
Bottom: water constant velocity inlet
Bottom: water outlet (pressure difference 0 Pa)
Up: air opening (dinamic pressure 0 Pa)

Solver control:
Transient, 1 sec total time, 1 ms timestep, Upwind, second order backward euler, 1E-04 residual target.

Free surface model: air and water continuous fluids, 2F model for drag coefficient, homogeneous turbulence, k-epsilon model

Last edited by j.zamorano; April 22, 2013 at 04:54. Reason: Canīt see the picture
j.zamorano is offline   Reply With Quote

Old   April 22, 2013, 04:57
Default
  #4
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
Is this enough information? If you need the output file or the CCL please give me your e-mail, and I will send it to you.

Thanks
j.zamorano is offline   Reply With Quote

Old   April 22, 2013, 10:00
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Why have you chose a 1ms time step? Unless you have actually done a sensitivity analysis on that time step size and determined it is what you need then it is bound to be wrong.

So let the solver work the time step out for you. Use adaptive timestepping, homing in on 3-5 coeff loops per iteration.

Are you using surface tension?

Why are you using a highly inaccurate spatial discretisation scheme (upwind) but a very accurate temporal scheme (2nd order back eular)? If you just want quick and dirty results then run 1st order in time as well. If you want an accurate answer you will need to run a better spatial discretisation than that.
ghorrocks is offline   Reply With Quote

Old   April 22, 2013, 10:28
Default
  #6
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 219
Rep Power: 5
RicochetJ is on a distinguished road
If you let the solver work out the time step via adaptive time stepping I've found the time step it selects is usually prohibitively small, such as 1e-8 s (that is if you converge to 3-5 loops).
RicochetJ is offline   Reply With Quote

Old   April 22, 2013, 19:25
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That is because it needs small time steps! There are very few simulations where this does not find the correct time step.

The only exception to this is when you are happy to sacrifice accuracy to just "muddle" through a tricky bit of the simulation and don't care about accuracy. An example could be when you first start the simulation up, or when an aggressive action occurs which you do not care about the details (eg a fast combustion event).

If this slows the simulation too much then
* Check that your mesh is not too fine
* Check your convergence is not too tight
* Get a faster computer
* Get more computers and run parallel.
ghorrocks is offline   Reply With Quote

Old   April 24, 2013, 10:34
Default
  #8
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
I am new in CFX, What parameters should I take to make adaptive timestepping? Max Courant number?
j.zamorano is offline   Reply With Quote

Old   April 25, 2013, 08:04
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No. Courant number only has a tenuous link to convergence in CFX as it is an implicit solver.

The recommended approach for adaptive time stepping is homing in on 3-5 coeff loops per iteration.
ghorrocks is offline   Reply With Quote

Old   April 25, 2013, 11:31
Default
  #10
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
I am not using surface tension forces, should I? I think the diameter is too big and this forces are too small (0.05 m). I am using free surface model, should I change it to mixture model?

Thank you so much
j.zamorano is offline   Reply With Quote

Old   April 25, 2013, 19:49
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Only use surface tension if it is important for the flow you are modelling. It is an expensive model and will slow you down a lot, so only use it if you have to.
ghorrocks is offline   Reply With Quote

Old   April 26, 2013, 07:33
Default
  #12
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
http://www.subirimagenes.com/imagen-...-8405900.html][/URL]

This is happening to me when I try to do a transient simulation. Does anyone know what happen? The program says something about overflow
j.zamorano is offline   Reply With Quote

Old   April 26, 2013, 08:23
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is a floating point error (which then caused lots of other errors including crashing the parallel run) - this is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F
ghorrocks is offline   Reply With Quote

Old   April 30, 2013, 07:44
Default
  #14
New Member
 
Javier
Join Date: Apr 2013
Posts: 7
Rep Power: 3
j.zamorano is on a distinguished road
I am having quite good results with steady state simulations. Now, I am doing transient ones. I want to reach the second state of the picture by improving the gas velocity. But, although the function for the gas velocity inlet is well defined, when I plot the results it shows everytime the first state (left). Can be this because problems of convergence? What should I do?

http://www.subirimagenes.com/otros-t...-8411961.html][/URL]
j.zamorano is offline   Reply With Quote

Old   April 30, 2013, 20:32
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,775
Rep Power: 77
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I do not understand your problem. What are you seeing and what do you expect to happen?
ghorrocks is offline   Reply With Quote

Reply

Tags
ccfl, convergence, counter current, free surface

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 04:24
CFX gravity driven free surface flow tutorial mechovator CFX 37 July 27, 2009 11:28
free surface flow in non-inertial reference frame Tiedingg FLOW-3D 1 February 26, 2009 20:51
Free surface vortex flow Guillaume CFX 3 August 25, 2005 21:52
Free surface flow simulation question Jane Luo FLUENT 1 April 23, 2004 05:26


All times are GMT -4. The time now is 08:18.