# CEL for Multiphase

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

 June 19, 2004, 11:53 CEL for Multiphase #1 Anne Guest   Posts: n/a Hi All, I am simulating a Solid-Liquid system using Eulerian-Eulerian scheme. I would like to specify [in CFX5.6] a drag law for the system. The drag depends on the particle Reynolds number (ie Re=U.d.mu/roh). where U and d are the particle velocity and diameter, respectively. How do i [if possible] specify the velocity of the particles using CEL? I am encoutering some problems when i specify the velocity as it appears in the output file (ie U-Mom-Solid) I can not see a similar problem in the acrhives. Please assist. regards, anne

 June 19, 2004, 19:53 Re: CEL for Multiphase #2 Jeff Guest   Posts: n/a Anne, Using Eulerian-Eulerian, you should have two phases (lets say "Water at 25 C" and "Solids"). The velocities of each phase are accessed by "fluid.u", "fluid.v", and "fluid.w" . You have to be really careful with the fluid name because they're case sensitive. Set a CEL variable that is equal to the square root of the sum of the squares of the three velocity components for the solids phase. As an aside, most drag equations are based on the slip velocity between the phases, not the particle velocity. In this case, you'll want to calculate: slipu = Water at 25 C.u - Solids.u slipv = Water at 25 C.v - Solids.v slipw = Water at 25 C.w - Solids.w slip_vel = sqrt(slipu^2 + slipv^2 + slipw^2) Then use slip_vel to calculate your Reynolds number. Hope this helps, Jeff

 June 21, 2004, 05:17 Re: CEL for Multiphase #3 Anne Guest   Posts: n/a Hi Jeff, Thanks for your kind response. Yes it was an oversight , that velocity was indeed the relative velocity. Now, i have done as you suggested, however, it appears I am still not communicating well with the PRE. Does the order of the commands matter? This is what i have done: Expression editor: ================================================== == ykolmog=(KinVis^3/max(ed,1.0e-14 [m^2 s^-3]))^.25 CDo24=10.56 [kg kg^-1] dp=150.0e-6 [m] KinVis=8.93e-7 [m^2 s^-1] Brucato1=CD*max(Kolmodp,1.0e-14) CD=CDo24/max(Rep,1.0e-14) Rep=SlipVel*dp/KinVis SlupU=Water at 25 C.u - Mynickel.u SlupV=Water at 25 C.v - Mynickel.v SlupW=Water at 25 C.w - Mynickel.w dp/max(MyKolmog, 1.0e-14 [m]) SlipVel=sqrt(SlipU^2 + SlipV^2 + SlipW^2) ============================================= PRE: (P/s there is a warning in Pre about 'Brucato') MOMENTUM TRANSFER: DRAG FORCE: Drag Coefficient = Brucato Option = Drag Coefficient END __________________________________________________ _ SOLVERS SAYS: Collecting array CBCP * subdirectories or data are missing Begin contents for /FLOW/BOUNDCON/ZN2 IZN = 2 CBCP(13) = BCP1,BCP2,BCP3,,BCP9,BCP10,BCP13,BCP15,BCP16,BCP17 ,BCP18,BCP19,BCP21 NBCP = 13 End contents for /FLOW/BOUNDCON/ZN2 | ERROR #001100279 has occurred in subroutine ErrAction. | Message: | Stopped in routine COLLECT_ARRAY __________________________________________________ _____ How do i make Pre understand my commands? regards, Anne

 June 21, 2004, 08:58 Re: CEL for Multiphase #4 Juan Carlos Guest   Posts: n/a Hello Anne, I am surprised by the error you are getting. It seems your boundary condition setup is damaged somehow. Are you using the CEL variable names that correspond to a reserved name, ie. Boundary condition/subdomain,domain, monitor point, etc.. Does it happen if you set Drag coefficient to a constant, for example? Still keeping you CEL setup.. That error is not very common..Your next step is to pass it to support, and they can quickly take a look for you.. Juan Carlos

 June 21, 2004, 10:08 Re: CEL for Multiphase #5 Anne Guest   Posts: n/a Hi Juan, Thanks for the quick response, Juan. When i set a constant drag coefficient with my CEL set up, as you had asked, I get the same error message. However, all is fine if I use, say, GIDASPOW drag coefficient. As you could see from my earlier posting, I am using variables like 'ed', (kinetic energy dissipation) and the velocities of the two fluids, which are solution dependent. I had arbitrary set some values for the respective velocity components and ed, in the Expression editor and I could see that all variables were solved. Where could the conflict be? thanks for your time, Anne

 June 21, 2004, 23:45 Re: CEL for Multiphase #6 Neale Guest   Posts: n/a Try your expression on the multiphase mixer tutorial. If that doesn't work send it to support. Neale

 June 22, 2004, 08:14 Re: CEL for Multiphase #7 Anne Guest   Posts: n/a Hi Neale, Thanks for your suggestion. The CEL does not work with Tut 15 (the multiphase mixer tutorial) either. I will hear what support says. anne

 June 23, 2004, 06:07 Re: CEL for Multiphase #8 Rui Guest   Posts: n/a Hi, I,ve been working with multiphase (Liquid and Air) flows, with CFX-5.6. I don't know if this is the reason for the error you get, but when I want to set some expression as function of the velocity, I have to write, for example, "Water at 25 C.Velocity u" (as this variable is shown in Post), instead of "Water at 25 C.u" (as it is described in the manual). When I write the *.def file, Pre tells me there is an error, but then the Solver works fine, Rui

 June 24, 2004, 06:35 Re: CEL for Multiphase #9 Anne Guest   Posts: n/a Hi Rui, Yes, the problem seems to be related to the naming and we are working on it. Thanks anne

 June 25, 2004, 03:58 Re: CEL for Multiphase #10 aris Guest   Posts: n/a i want to know how to make multiphase model

 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 Gloria Gaynor CFX 11 November 26, 2012 07:29 vmlxb6 CFX 1 March 18, 2011 07:39 jiguozhao CFX 1 March 18, 2011 07:38 bornspur CFX 2 February 3, 2009 03:24 Elian81 CFX 2 September 25, 2007 05:31

All times are GMT -4. The time now is 17:25.