# how to simulate compressible swirling flow?

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

 May 20, 2007, 14:00 how to simulate compressible swirling flow? #1 ravi Guest   Posts: n/a hello i need to simulate the flow of air that is injected tangentially (using nozzles of 1mm dia) into a cylinder of radius~2.5mm and length~10mm. The speed at the nozzle outlet is around 200m/s. Please suggest how can i give boundary conditions, what kind of mesh should i create? and how should i set-up the problem in fluent? are there any tutorials available that are similar to this problem? any other guides that can help me? thanks

 May 20, 2007, 17:26 Re: how to simulate compressible swirling flow? *NM* #2 k Guest   Posts: n/a

 May 22, 2007, 08:36 Re: how to simulate compressible swirling flow? #3 Neil Guest   Posts: n/a Hi Ravi, To get the desired inlet velocity I would use a pressure inlet BC setting Pstat to chamber pressure and an appropriate P0 (total pressure) so that there is a pressure drop across the injector to induce a velocity. This can easily be found from using the isentropic flow equations. Apart from this you will need to use a pressure outlet for the outlet. With regards to the mesh I would use a predominantly Hex mesh using the cooper hex/wedge scheme for the majority of the chamber but use tet elements in the regions where the tangential injectors meet the chamber. This will require a bit of geometry decomposition but if done right the amount of tet elements used can be reduced quite significantly. If you can I would also extend the outlet of the domain so that reversed flow conditions during iterations can mostly be avoided. This is assuming youre working in 3D, which I would advise because although it is easier to create a 2D mesh to use with the 2D axisymmetric swirl model in Fluent it is not accurately modelling the tangential injectors as it treats them as a ring as opposed to specific injectors. With model setup in Fluent I would use the Coupled (density based solver if 6.3) implicit 3D solver. Employing a sequential modelling setup for turbulence to get good convergence before changing the model to increase accuracy. Firstly solving for laminar then k-e RNG then RSM using 1st and 2nd order for both. This will take ages to run under the coupled solver but in my experience its the only way to stop residual divergence. Start your solid URF at around 0.2 and CFL at 0.5 so that initial calculations are stable but soon after this you can start increasing the CFL and later the solid URF, just experiment with the CFL so you get an understanding of what values to use with reference to the gradient of the residuals. There is I think a presentation on the Fluent learning CFD website which is on cyclone separators which is useful for understanding the need for the RSM model, if not it can be found at other websites if you search enough. Hope this helps Neil

 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 Munni Main CFD Forum 6 December 7, 2015 12:33 rw511 CFX 3 May 22, 2011 19:48 jehanzeb FLUENT 5 August 3, 2004 08:04 Mihai ARGHIR Main CFD Forum 0 April 7, 2000 04:58 R.D.Prabhu Main CFD Forum 0 July 17, 1998 17:23

All times are GMT -4. The time now is 09:57.