Vorticity creates convergence problems?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 11, 2014, 09:48 Vorticity creates convergence problems? #1 New Member   Ingmar van Dijk Join Date: Nov 2014 Posts: 5 Rep Power: 11 Dear all, I am new to this forum but have been doing CFD for a few years. Normally I calculate fairly simple quasi-one-directional systems that converge easily, but right now I am running into problems. I am simulating a boiler behind a gas turbine. The gas turbine outlet conditions are my inlet conditions. The high inflow velocity that flows past an open area creates strong vorticity, and any model that has this vorticity seems to create convergence problems. A figure of the model: http://i.imgur.com/uiGcLr2.png I tried: Refining the circulation region, has very limited effect, the circulation is captured by at least a few hundred elements across Switching to double precision - No effect Running for a long time - Continuity Residual flatlines at 5e-3 for at least 500 iterations (and in 50 iterations it reaches these values) I am using a thin boundary layer, 5 elements, 1mm first layer, Omega-SST turbulence model. I understand this should go well together with any thin boundary layer? And advice on reducing my residuals is highly appreciated. Further refinement is difficult since I'm running 1.5~2M elements already.

 November 11, 2014, 09:50 #2 New Member   Ingmar van Dijk Join Date: Nov 2014 Posts: 5 Rep Power: 11 I should also add that I looked at the difference two different points in the flatlined convergence, say 120iterations apart. The solutions were indeed quite different, and thus I cannot trust the calculation yet.

 November 12, 2014, 09:45 Switched to K-Epsilon Realizable - Enhanced Wall Treatment #3 New Member   Ingmar van Dijk Join Date: Nov 2014 Posts: 5 Rep Power: 11 Switched to K-Epsilon Realizable - Enhanced Wall Treatment, which gives me much better convergence. All values are below 1e-3 and all my pressure and uniformity monitors have leveled out and also change less than 1e-3 per iteration. Perhaps this is a simplified conclusion, but it seems that the K-Omega SST doesn't work well with large vortices in a calculation. Perhaps because it was originally written to only work well in the boundary layer? (Before adding wall functions). Any thoughts on this are appreciated =). Kind regards,

 November 12, 2014, 10:28 #4 Senior Member     Rick Join Date: Oct 2010 Posts: 1,016 Rep Power: 26 Hi, thanks for sharing your solution. I think the transition model needs a transient approach: this could be the reason. It is possible that your problem is not steady and the k-omega sst could't find a steady state solution. jamalf64 likes this. __________________ Google is your friend and the same for the search button!

 November 12, 2014, 10:38 #5 New Member   Ingmar van Dijk Join Date: Nov 2014 Posts: 5 Rep Power: 11 Indeed the location and size of the vortex kept changing when using the SST model, however the "transition model" is the 4 equation one that's heavier than k-w-SST or k-e right? Are you sure about the transient solution requirement? I'm going to do some more tests, and compare k-w-SST and k-e-realizable for an easier model, that does converge for both. I'm hoping they are at least the same if properly converged... I'll see what I can share here.

 November 12, 2014, 10:48 #6 Senior Member     Rick Join Date: Oct 2010 Posts: 1,016 Rep Power: 26 This is a comment of Thomas Frank, from Ansys Inc.: A k-omega SST model delivers in most cases a more exact solution, it can resolve boundary layers down to finely resolved meshes with y+ <=1 and it is usually less dissipative (i.e. produces a smaller amount of turbulent viscosity). The price for this is that a k-omega SST model usually tends to predict already transient flow behavior where a standard k-eps model produces so much of turbulent viscosity that it stays in steady-state flow regime. People find that convenient. But in fact it can hide the true nature of the investigated flow phenomenon from being discovered by the simulation, so it can be a bit dangerous to rely on (exclusively). jamalf64 likes this. __________________ Google is your friend and the same for the search button!

 November 12, 2014, 10:50 #7 New Member   Ingmar van Dijk Join Date: Nov 2014 Posts: 5 Rep Power: 11 Wow, very interesting, definitely going to dig into this! Thanks!

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post recnice OpenFOAM Running, Solving & CFD 3 October 9, 2013 12:19 colopolo CFX 13 October 4, 2011 22:03 nasdak CFX 2 June 29, 2009 01:17 StudentAndrew CFX 6 November 21, 2005 06:49 Chetan FLUENT 3 April 15, 2004 19:13

All times are GMT -4. The time now is 03:22.

 Contact Us - CFD Online - Privacy Statement - Top