# coupled DPM

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

 June 27, 2001, 13:12 coupled DPM #1 Peter Kolb Guest   Posts: n/a I want to simulate the two-phase flow with coupled DPM. At the moment I have some problems with convergence resp. residual plot (especially the continuity) is fluctuant. Can anybody tell me if the fluctuations are normal and when convergence is reached? Or does anybody have an small example/tutorial where I can see how an optimal two-phase flow with coupled DPM is looking like. Yours sincerely Peter

 June 27, 2001, 14:42 Re: coupled DPM #2 Lanre Guest   Posts: n/a The residuals will "jump" or "fluctuate" if the mass/momentum/energy source released by the DPM phase into the continuous phase is relatively large during coupled DPM calcs. This is expected. What you want is for the trend to decrease after a large number of iterations. To improve convergence, try: 1. increase number of DPM calcs per continuous phase iterations from default 10 to 40 (max recommended) 2. spatially distribute your injection. If you are injecting a large mass/momentum/heat source into a single cell, you may experience convergence difficulties. Use surface or group injection. 3. if turbulent, increase the number of "tries" or stochastic attempts. Since FLUENT divides the mass flow by the number of tries, this is the recommended approach when modelling combusting (heat/mass transfer) using the DPM model. 4. If this is a buoyancy-driven problem with the DPM bubbles being the source of momentum, consider patching initial values of upward velocity in the approximate volume where you anticipate the bubble plume to be. mohammadkm likes this.

 June 28, 2001, 03:06 Re: coupled DPM #3 Livo Guest   Posts: n/a Lanre 1. increase number of DPM calcs per continuous phase iterations from default 10 to 40 (max recommended) I am assuming it is increase number of continuous phase iterations per DPM iteration. Could you explain why this value must be increased. In the Fluent manual they just say this value depends upon the physics of the problem which has no meaning for me. Thanks

 June 28, 2001, 09:58 Re: coupled DPM #4 Lanre Guest   Posts: n/a Since the DPM model is applied in the Lagrangian sense, the continuous phase flow field must first be solved. The number of continuous phase iterations performed before a DPM injection needs adjusting depending on the sensitivity (strength on mass, momentum and energy sources) of the DPM trajectories on the continuous phase. In short, the more contiuous phase iterations between each DPM calc will lead to a more stable solution. The flip side is that if the DPM injections drive the flow, convergence will take a little longer. This is why I did not suggest >40 continuous phase calcs between each DPM injection.

 October 2, 2012, 11:27 #5 New Member   hassan salem Join Date: Aug 2012 Posts: 5 Rep Power: 4 the no. of contiuous phase iterations between each DPM iterations depends on the amount of coupling between discrete and continuous phase...if this no.<3..this means there is strong coupling for example...so this no. depends strongly on the problem physics...

October 4, 2012, 10:27
#6
Senior Member

Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,097
Rep Power: 16
Quote:
 Originally Posted by hassansalem the no. of contiuous phase iterations between each DPM iterations depends on the amount of coupling between discrete and continuous phase...if this no.<3..this means there is strong coupling for example...so this no. depends strongly on the problem physics...
Finally, over ten years after its creation, the problem can be officially declared as solved. Thank you so much grand master of DPM, now Peter Kolb can arise from standby and continue working.

 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 Aimara FLUENT 0 April 25, 2007 16:23 harry Main CFD Forum 0 June 2, 2005 06:12 Doug FLUENT 0 March 1, 2005 17:37 vkt FLUENT 0 September 16, 2004 07:41 winnie FLUENT 0 May 15, 2003 22:12

All times are GMT -4. The time now is 02:48.