Dear Rajeev

I am patil from india, IIT Bombay, Mumbai, (civil engg background). thk u for replying and giving good advice. As per your advice i tried to run fluent. but got some doubts

1. i want feed 73.6 ml (over a time of one minute) of dye tracer with 500ppm( property are same as that of water) into the tank containing liquid-water. therefore how to feed this exact quantity of dye tracer with 500ppm?

2.Mixture( liquid water-dye) pannel needs the mass diffusion Coeff. In my case both bulk fluid and tracer are having same property as that of liquid water. hence pl. give some idea about mass diffusion coeff. value for my case.

3. In inflow bc pannel if i start with mass fraction of dye as one(1)( as per your advice) what will be the correct meaning of this step. pl. explain the technical aspects of this.

4. Give some idea about mass fraction( As is required to be given the the inlet BC pannel of Speceis trnp model of fluent?

5. How much fluent 6 has costed you( assuming that you are using this for educational purpose)?

waiting for you reply.

Dear Patil,

Well if you want to feed the exact amount then what you can do is calculate the mass fraction needed for injecting.

Here is how you should do.

(73.6 ml/1000000)m3 * 500/1000000 * 1000 kg/m3 = 368e-7 kg of dye.

So if you want to inject it for 1 min then flow rate of dye becomes (368e-7/60)kg/s.

Now if you know your inlet flow rate. Let us call it x kg/s then you know the mass fraction dye to be injected over a period of 1 s (368e-7/60)/x .

This you should place in the mass fraction species flux.

Now if you want it to give this injection for 1 min. Simply let this mass fraction be present in the species flux for the required no. of time steps.

1min = no. of time steps x size of time step.

After that you should change the dye fraction to zero to get the RTD curves.

Finally you will need some post processing to calculate the volume fractions if that is what you are intending. Please let me know what type of system are you trying to model. Then we can share some information regarding that.

I am working in RDCIS, which is corporate Research Center for SAIL.

We bought Fluent 5.5 last year May 2001, with AMC of 2 years. So we got the update to FLuent 6.0 free of cost.

Binary Diffusion coefficient has to be provided when you are using Species Transport Model. Turbulent diffusivity part is calculated by the solver itself.

I was also in a fix whether to give some binary diffusivity or not. I tried with Binary Diffusivity as 0 and 3.05e-05 as given in FLuent. When binary diffusivity of 3.05e-05 was given the RTD curves where slightly flatter showing slightly more mixing. Whereas the value of 0 gave sharper curves. But calculation of volume fractions and MRT showed no appreciable change. So I concluded that in cases where forced convection is larger than the natural convection you can very well do with 0. I would say if your medium is water then you can use 3.05e-05 as the value without any problem. Or you can change it by some percentage points and see whether your results vary or not.

Let me know if my message clarifies your doubt.

dear Rajeev,

Your email has really helped me in understanding the tracer studies. I am working on flocculators in water treatement plants. Trying to compare the performance of different flocculators. For that i am using CFD software(Fluent). Detension time for flocculators is a imp parameter. Hence to understand the behavior of flocculator properly the tracer studies are required. In physical experiments i am inputing the salt soln as a tracer.

I will feed this 500ppm salt soln along with clear water into the flocculator for about 1 min. at the same time i collect sample at the outlet at an interval of 30sec and using that sample i will conduct the electrical conductivity test. Knowing the counductivity, i can calculate the concentration of salt in that sample. Like this i will prepare the graph of exit salt concentration V/S time in min. from this graph i can say that floccculator is having X% of dead space, y% of mixed flow , Z% of Plug flow, curve also give an indication of the short circuiting (i.e If the salt(tracer) concentration appear immedeatly at the outlet, that indicate bad behaviour of the flocculator) In expt, i am getting measurable quantity of tracer after 6 min and it will rise up 10 min. and then it countinue to fall down( to zero after 80min.) In similar fashion i want to conduct cfd simulation so that i can avoid the physical experimets.

I think within 2-3days i will try your ideas. I expect same help in future also. pl. keep contact. thk u bye

Dear Patil,

It is nice to hear that my message was of some help. It seems your problem and mine are quite similar. I am modeling flow of molten steel inside the tundish. You can compare the situation to that of a bath tub with multiple drainage holes. When the bath tub is filled with water and simultaneously drained you have to see the flow feature developed. To prevent short circuiting we provide dams in the bath of flow to increase the retention time.

As for the species transport part I am getting everything fine. But while I am using steady-state k-ep model for flow simulation I find that my residuals remain quite high. (10e-00 unscaled) for continuity. However hard I try by bringing down the relaxation parameter or by using PISO scheme, the residuals remain very high although I get a good mass balance.

Let me tell you that I am using Cooper scheme for my geometry and I land with somewhere around 35000 cells for a tub of 2900 x 700 x 400 mm sized tub (tundish).

Is your solution domain as big as mine. It seems so from your time length scales. In how many cells you are calculating your domain and how is your convergence. Is it smooth or you are also facing my kind of problem.

Do reply,

Thanks Rajeev

dear Rajeev,

My tank size is 0.443mx 0.443m x 0.445m. I am also using cooper. But my cells are very fine( 4.2lakh), reason for such a large cells is the inlet pipe diameter(8mm). By exprience i feel that inlet affects soln a lot. hence at least some 10 cells should be present for better convergence. if i vary the size of cell using adaption, the benifit is very marginal. I feel that it is possible to reduce the cells further with little more effort and experience. Presently i am new to CFD. hence to avoid the "grid dependent soln", i usually go for finner cells. But i know that i am consuming lot for cpu time.But for a beginner it is required.

As a trial you can try the following 1. try to increase the number of cells near inlet and outlet Or at the place where velocity gradient changes fast.

2. Go for second order upwind.

3. reduce relaxation constants.

4. avoid sudden change in the cell volume(IT SHOULD BE VERY SMOOTH)

I feel residual should be less than 0.0001. I am getting this. In your case, you may be solving number of equations like conti, momentum, transport, energy, radiation, etc. hence Initially try negelecting some of the equations and the after getting good convergence(conti,xvel,yvel,zvel, mom,k,e) then go for transport, energy, radiation etc.... using the previoulsy converged values..

good luck.

bye

[kingjewel1]

Originally Posted by Thomas
;99157

I have made something similar in order to deduce the ventilation rate of a structure. I have used CO2 as a tracer gas. If you are interested I can describe you the procedure.

Hi Thomas,

Please explain your procedure.

[eswar_chem08@yahoo.co.in]

hi Rajeev sir, i am eswar doing m.tech chemical (nit trichy). my project is studies on static mixing, ( residence time distribution (RTD) and pressure drop). i am using CONGO RED (100 ppm) for RTD sudies, i complited my experimental work, know i have to validate experimental results using fluent. i finished gambit part.
my question is
1) for RTD studies i want inject 50 ml CONGO RED in continuous liquid flow, i have to find outlet concentration with respect to time intervals 5 sec, pease help me for project. send the answer to my mail.
( eswar_chem08@yahoo.co.in)

please give step by step procedure in fluent, this is first time i am using CFD

[yorelchr]

Originally Posted by Nico
;99852

just create a species with the same properties as the fluid and patch them where you want them at t=0

How do you patch?
I have 2 fluid species : the water and the dye (same properties as water).
When I want to patch I only have the choice with "fluid"...I can't select "dye"...

[yorelchr]

Originally Posted by eswar_chem08@yahoo.co.in

hi Rajeev sir, i am eswar doing m.tech chemical (nit trichy). my project is studies on static mixing, ( residence time distribution (RTD) and pressure drop). i am using CONGO RED (100 ppm) for RTD sudies, i complited my experimental work, know i have to validate experimental results using fluent. i finished gambit part.
my question is
1) for RTD studies i want inject 50 ml CONGO RED in continuous liquid flow, i have to find outlet concentration with respect to time intervals 5 sec, pease help me for project. send the answer to my mail.
( eswar_chem08@yahoo.co.in)

please give step by step procedure in fluent, this is first time i am using CFD

Hi eswar, did you have any answer for that? it seems that nobody on the forum does....trying to inject dye in liquid water...but no way!!!

[tarangbulchandani]

Dear Friends,

I want to do tracer studies for liquid solidd system where density of solid is less than that of liquid. Here I am injection solid using DDPM in Ansys 13. And i have to inject when tracer particle same as the density of solid to get the concentration profile. Can anyone help me up with this problem???

Waiting for the positive feedback.

Regards
Tarang

[rishi.chouhan]

hi Rajeev Kumar Singh,

I am doing the same mixing of nitrogen in liquid steel problem. Can tell step by step from usingVOF model to how to put tracer in species transport model. Please I new to this SOftware so I dont know these advance option???