drag force in two phase flow

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

 LinkBack Thread Tools Search this Thread Display Modes
 November 18, 2005, 13:33 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, 14:36 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, 12:40 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 20, 2005, 23:14 Re: drag force in two phase flow #4 Rui Guest   Posts: n/a Hi Ken, I'm modelling mould filling problems, which are transient free-surface (Polymer & Air) flows. I tried to solve a simple problem, the filling of a space between two parallel plates with a Polymer with constant density and viscosity: As you, I started with the Homogeneous Model, as the phases are completely stratified and the interface is well defined. This is also your case, and that's why I asked why you were using the Inhomogeneous Model instead of the Homogeneous. But with the Homogeneous Model I got bad results: (This is just partial view of the whole length. The Polymer is coloured red and the Air blue, the 3 contour lines denote volume fractions of 0.9, 0.5 and 0.1.The vertical line is the theoretical position of the interface at that instant.) As you can see, with the Homogeneous Model there is a "layer of Air" next to the wall. This is due to the no-slip BC which prevents the air from moving forward. This "layer of Air" will lead to an underestimation of pressure and heat transfer between the Polymer and the mould wall. With the Inhomogeneous Model and with the free-slip BC for the Air phase I got this: I modelled these cases with CFX-5.6, so I had to use the Mixture Model (the Free-surface Model wasn't available in CFX-5.6). But I had a problem, which I suppose you also have: What values to use for the Drag Coefficient (CD) and for the Interface Length Scale (dab)? If the phases are well stratified there isn't any theory to determine those values, or I can't think of any.However, if you insert into you'll get: Thus, the individual values of the CD and dab don't matter, but the quotient CD/dab. Itīs the same to use CD=5 and dab=1 mm, or CD=50 and dab=10 mm. I have tested this, and the results are exactly the same. So I kept the default value of dab=1 mm, and tested some values of CD between 5e-2 and 5e2. For the higher values of CD, the behaviour becomes similar to the Homogeneous Model, which makes sense as for high values of drag force between the phases the phases velocities tend to equalize. For low values of CD I observed oscilattions in pressure and longer computation times. I found CD=5 to be an "optimal" value. However, I think this value is totally problem dependent. Afer CFX-5.7 has been released I tried the Free-surface Interphase Transfer Model. Answering your question: No, I didn't see any literature where the interfacial area density was equal to the volume fraction gradient. And, as for the Mixture Model, I can't see any theory to determine the value of CD. As I did for the Mixture Model, I tested some values of CD, and I found CD=50 to be the "optimal value". But again, I think this value is totally problem dependent and perhaps mesh dependent. The computation time to run these problems is lower with CFX-5.7.1 and CFX-10 than with CFX-5.6.However, the Polymers that I'm working with are resins, which suffer a chemical reaction (the cure of the resin) while and after the mould is being filled, that I have to model. I really don't know why, and have been discussing it with CFX support without luck, but when modelling the mould filling with cure reaction, the computation time with CFX-5.6 is lower (about an half) than with CFX-5.7.1 and CFX-10. Because of this, and because my simulations take some days even for simple geometries with coarse meshes (I need a very small time-step ~5e-4 s), I have been using CFX-5.6, and haven't "played" again with the Free-surface Interphase Transfer Model. This why I got interested to know if you had achieved any improvement by using the Free-surface model. I would like to ask you what values of CD have you been using when using the Free-surface Interphase Transfer Model, and what values of CD and dab when using the Mixture Model, and if you have any reason to use those values. Regards, Rui

 November 21, 2005, 11:52 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, 15:28 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 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 Li Main CFD Forum 5 March 4, 2017 16:04 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

All times are GMT -4. The time now is 05:09.

 Contact Us - CFD Online - Privacy Statement - Top