# drag force in two phase flow

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

 November 18, 2005, 14:33 drag force in two phase flow #1 Ken Guest   Posts: n/a Hi, I am modelling free-surface flow (air-water). I am wondering how the drag force is modelled,if I set both air and water to be continuous (inhomogeneous, standard free surface model) and use "free surface" option for interphase trasfer with a drag coefficient given. Does CFX use the same relation for the momentum transfer coefficient as that in mixture model, cd=function(CD, A)? where A is the interfacial area density, equal to the gradient of volume fraction when "free surface" option is used. Thanks!

 November 18, 2005, 15:36 Re: drag force in two phase flow #2 Rui Guest   Posts: n/a Hi, Yes, you are correct. I have asked, a while ago, the same to the CFX support. When using the "free surface" interphase transfer option, the interfacial area density is: and the drag force is obtained with the same expression used for the "mixture model": May I ask you what kind of problem you're modelling and why you're using the Inhomogeneous Model? Have you noticed any improvement by using the "free surface" interphase transfer model instead of the "mixture model"? Regards, Rui

 November 19, 2005, 13:40 Re: drag force in two phase flow #3 Ken Guest   Posts: n/a Hi Rui, Thanks. I am modelling sewer flow. I used homogeneous at the begining, but for some flow the simulated velocity was not satisfactory and the water surface looked kind of funy, the definition of which i feel is debatable (volume fraction = 0.5). So I switched to inhomo and got better. I didn't see difference between mixture and "free surface". We don't have info/knowledge about air entrainment in this flow and i don't concern that very much. So no reason to use mixture model, which will bring more uncertainties when giving mixture length, etc. Just curious, what are you working on? Another question, did you see in any literature the equation of the interfacial area density equal to the gradient? Thanks. Best wishes, Ken

 November 21, 2005, 12:52 Re: drag force in two phase flow #5 Phil Guest   Posts: n/a Interesting stuff... nice summary. Regarding slowdown between 5.6 and 5.7, try setting the expert parameter 'mpf free surface drag factor=0'. This parameter was added in 5.7 to improve stability for some inhomogeneous free surface calcs, but it might also slow things down when its not necessary.

 November 21, 2005, 16:28 Re: drag force in two phase flow #6 Rui Guest   Posts: n/a Hi Phil, Thanks for your suggestion, but I'm already running the simulations (in CFX-5.7 and CFX-10) with the expert parameter 'mpf free surface drag factor=0'. I didn't mention it in my last post, but when I started using CFX-5.7 (and didn't change that parameter) the computation time to model just the filling problem (without cure reaction and heat transfer) was quite longer than with CFX-5.6. The maximum number of iterations per timestep (50) wasn't enough for the equations to converge, while in CFX-5.6 less than 10 iterations per timestep were usually enough to achieve the convergence target (1e-5). Then, by suggestion of the CFX support I set that parameter to zero, and I got a lower computation time than with CFX-5.6. The problems arise when I model the cure reaction, which may be described by: dC/dt=Scwhere d/dt represents total derivative, C is the degree of cure (it varies between 0 and 1), and Sc is the rate of cure. Sc=f(T,C), when C->1 Sc->0 I'm modelling this reaction with a Transport Equation for an additional variable (C) with a source term (Sc). The cure reaction is exothermic, and thus there's also a source term on the energy equation: Sh=k*Sc. The resin viscosity is a function of the temperature and the degree of cure. But even when modeling the simplest case with cure reaction I can imagine: Isothermal so Sc=f(C) and resin viscosity = constant, the computation time with CFX-5.7 and CFX-10 is about the double than with CFX-5.6. I think it's due to some "improvements" that have been made to multiphase simulations which don't really work in my case. As I need a quite small timestep (~5e-4 s), otherwise the equations don't converge, the simulations performed with a mesh with only ~5000 elements take 4 or 5 days with CFX-5.6 on a common PC (they will take 8-10 days with CFX-5.7 or CFX-10). I have tried parallel processing, but with 5000 elements the computation time is even longer. The only way I found to improve the computation efficiency was by setting the minimum volume fractions of both phases to 1e-5 (the default is 1e-15). But the improvement represents only about 15% reduction on the computation time. Due to this, unfortunatelly I can only model very simple geometries where I can use meshes with a small number of elements. I feel lucky because I have started modelling these problems with CFX-5.6, but at the same time I feel a bit disapointed because the computation time with the latest versions of CFX is longer and there's nothing I can do about it. Apart from this question of the computation time, I got good results, when compared with other numerical results and with experimental results, with CFX-5.6, 5.7 and 10. Regards, Rui

 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 ozzythewise Main CFD Forum 8 June 13, 2012 06:24 colopolo CFX 13 October 4, 2011 22:03 Martin Main CFD Forum 9 July 11, 2008 09:10 icedou FLUENT 6 July 10, 2005 02:52 Li Main CFD Forum 4 April 13, 2005 11:01

All times are GMT -4. The time now is 06:14.