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

Convergence issues with Porous interface

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 10, 2013, 07:09
Default Convergence issues with Porous interface
  #1
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Hello

I am trying to model the strainer as a porous interface but am I can't get it to converge.

To obtain the a reasonably accurate solution, I have kept the mesh relatively fine but as a side effect, the Solver is picking up the small-length-scale oscillations which perhaps is forbidding the stable convergence. Also, perhaps owing to sudden change of pressure and related parameters across the strainer, the Solver is not able to successfully use the same time scale as in other parts of the domain.

To counter this, I have also changed the expert parameters for under-relaxation as :

ggi ap relaxation = 0.3
solver relaxation fluids = 0.6
solver relaxation scalar = 0.6
solver target reduction fluids = 0.001
solver target reduction scalar = 0.001

... but in vain,

I am using high resolution scheme for turbulence and advection with Auto timescale option.

Would increasing the time scales help? Or are there any other methods to tackle the porous interfaces?

Thanks
OJ
oj.bulmer is offline   Reply With Quote

Old   January 10, 2013, 09:29
Default
  #2
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
When you say porous interface, you mean a fluid/fluid interface where you mathematically insert a pressure drop to flow correlation? I did this before and had the convergence problems as well. I ended up just using a porous domain or fluid subdomain with a momentum source, this converged much better than the "porous interface" which I could't get to work at all.
evcelica is offline   Reply With Quote

Old   January 10, 2013, 10:26
Default
  #3
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Erik,

Yes, I used a the mathematical pressure drop flow correlation using the resistance coefficient from the handbook. And the reason being that the conical strainer is as thin as 5 mm in thickness, diameter is 1800 mm and length is 3000 mm. Using the strainer as porous domain means I need to have at least 3 cells along the thickness of the strainer, and this increases the cell-count quite substantially increasing the running time. And more importantly, it will take more time in pre-processing as well, affecting time lines.

Fluent has a quite cute feature called porous jump wherein you can calculate the pressure jump coefficient using given guidelines and you have an interface ready! I wish CFX was this easier.

How did you specify a momentum source (I assume negative)on a fluid subdomain?

Regards
OJ
oj.bulmer is offline   Reply With Quote

Old   January 10, 2013, 12:01
Default
  #4
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
Well in actuality your pressure drop is not going to drop only through the thickness of the strainer. I've modeled actual strainers/orifices before, and the pressure drops both before and after the strainer, so it is OK if the thickness of your porous domain if thicker than 5mm. you would obviously have to adjust the permeability and loss coefficients to account for the thicker porous region.
If you use the fluid subdomain and put it in the same domain as your fluid geometries, you would only need one cell of thickness in that part of the geometry, again it doesn't have to be, and probably shouldn't be, only 5mm thick because of my previous statement about the spatial pressure drop profile. To do this you just create a subdomain, pick your region, and then click the "momentum loss/porous model" box and fill in your variables for permeability and loss coefficient.
If it is not physically modeled, You can do the same thing to the entire domain, and use step functions or if statements so the momentum loss model equals zero everywhere except where you want it to apply.
evcelica is offline   Reply With Quote

Old   January 15, 2013, 07:52
Default
  #5
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
As an update, I tried the local timescale of 5 and proceeded with interface setting in CFX and to my surprise I got a nice convergence till O(1e-4). I then switched to Auto timescale and things seem to be running fine. I will update the forum with my final verdict.
oj.bulmer is offline   Reply With Quote

Old   January 24, 2013, 05:53
Default
  #6
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
Concludingly, yes, local timescale does make the solution stable. I ran with local timescale till residual values of O(1e-4) and then switched to auto timescale for final few iterations. All along, keeping a tab on the monitors and ensuring they are reasonably flat.

Essentially, the sudden change in properties across the interface creates the problems in having universal timescales. Essentially, from inlet to outlet, the no. of cells that intersect the flow are significant for local timescales. As long as you run sufficient iterations using local timescales, the convergence and the stability should be fine.

Cheers
OJ
oj.bulmer 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
Wind turbine simulation Saturn CFX 34 October 16, 2014 05:27
Interface between fluid domain and porous domain windhair CFX 5 September 5, 2013 20:45
Multiphase Porous Media Flow - Convergence Issues VT_Bromley FLUENT 5 March 23, 2011 11:38
2 stage axial turbine model convergence issues sherifkadry CFX 2 September 7, 2009 20:51
Grid size, convergence issues franzdrs Main CFD Forum 3 June 18, 2009 07:57


All times are GMT -4. The time now is 16:43.