# Convergence issues with Porous interface

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

 January 10, 2013, 07:09 Convergence issues with Porous interface #1 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 Sponsored Links 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

 January 10, 2013, 09:29 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 659 Rep Power: 13 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.

 January 10, 2013, 10:26 #3 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 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

 January 10, 2013, 12:01 #4 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 659 Rep Power: 13 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.

 January 15, 2013, 07:52 #5 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 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.

 January 24, 2013, 05:53 #6 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 13 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Saturn CFX 45 February 8, 2016 05:42 windhair CFX 5 September 5, 2013 20:45 VT_Bromley FLUENT 5 March 23, 2011 11:38 sherifkadry CFX 2 September 7, 2009 20:51 franzdrs Main CFD Forum 3 June 18, 2009 07:57