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

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

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

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

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

Try your expression on the multiphase mixer tutorial.

If that doesn't work send it to support.

Neale

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

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

Hi Rui, Yes, the problem seems to be related to the naming and we are working on it.

Thanks anne

i want to know how to make multiphase model