In the manual of CFX4, the default source term of the transport equation is multiplied by volume fraction. So When I add other terms as source term, should I divide the volume fraction? If that is right, how about the momentum equation? Does anyone know it?

Hi neil,
Pay attention on units you're using. Suppose that you want to modify your V Velocity Equation. If you use a source term like this:
-m*V/K with m and K your own parameters.
The resulting unit must be Force/Volume -> [N/m3]. Take a look at the transport equations and you will check the units.
Continuity: Mass flow rate / volume -> [Kg/(s*m3)]


About linearization, I suggest you to take a look at Patankar's book (Numerical Heat Transfer and Fluid Flow, 1980).


Good luck, cfd guy

Hi, cfd guy the question puzzles me, when I want to add user scalar transport equation , the source term doesn't deal with volume fraction , i don't know whether the source term is divided by volume fraction. would you clear me out? thanks in advance.

zhu

Hi zhu,
I don't know your specific scalar transport equation but I can say that depending the equation you have, you can't divide it by volume fraction or any parameter. In my previous post I said that care must be taken with units. Volume fraction only matters in a two-phase flow (at least), so you'll have two scalar transport equation, one for each phase. Perhaps your question is about linearization. Did you take a look at specific books?
Regards, cfd guy

hi, cfd guy, thanks i think my question isn't about linearization. i want to know whether the source term of two-phase flow is multiplied by volume fraction in program. for example, user scalar transport equation of A phase is as follow.

a(r*density*scal)/a(t) + v.[r*density*U*scal-dif*v(scal)]=r*(B-P)+C*(scal of B phase-scal of A phase) r,scal, dif,B,P is volume fraction ,user scalar,diffusivity of A phase, respectively. B-gravity, t--time. v--laplacian functor. C--interphase exchange coefficient

In mathematical models chapter of the cfx use guid ,the generic scalar advection-diffusion equation takes the form is given. In the equation the source term S is multiplied by volume fraction.when the source term S is added in subroutine usrsrc,whether the source terms S is automatically multiplied by volume fraction during run the program?

so,in subroutine usrsrc,after linearization, whether i specify the source term S is equal to [r*(B-P)+C*(scal of B phase-scal of A phase)], or [r*(B-P)+C*(scal of A phase-scal of B phase)]/r? i don't know. looking forward to your post.

zhu

Hi zhu,
I think I finally understood your question, sorry. It's a good question. The equation you mentioned is Eq. 3-328 from the online manual (PDF File, CFX-4.3 and 4.4 versions) and 12.10.1 of the Solver manual.1 from the printed manual (CFX-4.2 Version). If you take a look at the first term on right hand side (RHS) of the 3-328 equation you'll see r(alpha)*S(alpha), where r and S are volume fraction and source term of phase alpha, repectively. I believe, I'm not sure, that the code multiplies r(alpha) with the source terms (SP and SU), ie. if you have a source like this: phi(alpha)*r(alpha)/K(alpha), where phi and K are the scalar variable and a specific constant of alpha phase, you can put this source term in two ways:
SP = -1/K(alpha) ----> (Remember that r(alpha) is multiplied later)
or
SU = phi(alpha)/K(alpha) ----> (You should take care using this implementation. Remember the linearization).
Well, I believe that the code does like I mentioned above. I may be wrong. Commercial codes are "black boxes" and, unfortunately, you can't have full control of them. Your question also applies with the Volume. Once I had the similar doubt, however my problem was with volume of cells, not the volume fraction, when I was applying some source terms into an equation.


If you're still in doubt you should contact some CFX office. I'm also interested in their answer. Good luck! cfd guy

hi, cfd guy, thanks,

I consult CFX office, they say that volume fraction isn't considered in sourse terms, in the program code, the source term s isn't multiplied by volume fraction.that is ,if a source like this: phi(alpha)*r(alpha)/K(alpha), where phi and K are the scalar variable and a specific constant of alpha phase, SU = phi(alpha))*r(alpha)/K(alpha) .

p.s. i have a question about volume of cells. whether the source terms is multiplied the volume of cell. such as , convection-diffusion=s, i want add one term phi(alpha)*r(alpha)/K(alpha) in the s, whether the term multiplys volume of cell? thanks. zhu

Hi zhu,
I'm glad you had an answer, after all this question seems to be easy to obtain an answer, but as I said before the cfd codes are black boxes. All I can say about volume of cells is that you must satisfy the units of your transport equation. We'll keep the same example used before, but we're gonna add this source into the V velocity equation. Source Term: phi(alpha)*r(alpha)/K(alpha)
Note that "phi" has dimension of L*T^-1 (velocity, m/s in SI units). r is dimensionless (volume fraction). And SUPPOSE that K has dimension of T*M^-1 (s/Kg). Thus, the source term will have dimension of Kg.m/s^2 [Newton]. This dimension must be guaranteed for the momentum equations. However SUPPOSE again that K has dimension of T*L^3*M^-1 (s.m3/Kg). In this case your source term must be multiplied by the volume of cell.
SU = phi(alpha)*r(alpha)*VOL(CELL)/K(alpha)
or
SP = -r(alpha)*VOL(CELL)/K(alpha)
Well, I believe that's it. Kind regards, cfd guy

Hi,cfd guy and Zhu.

I am glad to see your discussions about the problem. However, I still have some ideas about the first question. If the volume fraction should not be divided by user, is it suitable for the momentum equations or general scalar equations or both? Thanks

neil

I mean if the volume fraction should not be divided by user in both the momentum equation and user scalar equations.

hi anyone i am using CFX5.5 to simulate an coaxial jet mixer. i want to plot radial velocity profile at specific axial point. i observe that i can plot radail profile at the inlet, outlet, and the defult but i can not plot at specific point for example if i have pipe x=2m long and diameter of .05m and i want plot radial profile at point x=0.5m. if you don't mind explain how to do that in cfx5.5 in detail.

thank you.