How to introduce a tracer
 

Basically, I am using the FLUENT software to simulate the air flow in a gas turbine enclosure. The main objective if the simulation is to optimize the efficiency of the ventilation system in the enclosure. There are three silencers where the air flows into the enclosure. The hot air due to the heat generated by the gas turbine will be exhausted through 6 outlet duct. I am going to simulate the repalcement of the 'old air'(hot air) with the 'new air'(fresh air). In order to do the simulation, I have to introduce a tracer in the enclosure. This tracer has the same properties as air and is represented by a passive scalar(presence ratio). At a time referenced as t=0s, the tracer value will be set to the value of 1 at the silencers wheareas it is 0 elsewhere.Then, I can follow the tracer with time, which show how the air is replaced in the enclosure. The efficiency of the ventilation system can be determined since a ratio of 1 for the tracer can be read as only 'new air' and 0 only 'old air'. If anyone know the method to put a tracer by using FLUENT, I will be pleased if you can tell me something on that. Thank you.

Re: How to introduce a tracer
 

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.

Re: How to introduce a tracer
 

Yes, it's interesting

Re: How to introduce a tracer
 

I am very interested. I will appreciate if you can tell me the details of the procedure. Thank you.

Re: How to introduce a tracer
 

can you help in this topic. how to introduce tracer?? waiting for yor reply. bye

Re: How to introduce a tracer
 

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

Re: How to introduce a tracer
 

HI, CAN YOU EXPLAIN ME IN DETAIL( i.e. STEP BY STEP)? IT WILL BE VERY MUCH HELPFULL FOR ME WAITING FOR YOUR REPLY. BYE

Re: How to introduce a tracer
 

if you just want to study the dispersion of let's say some dye in your flow field you can first solve the flow field and then switch on the species (define -> species) in materials you define lets say a dye with the same properties as the fluid e.g. water-liquid by replacing the name 'water-liquid' by 'dye' and deleting the chemical formula, press change/create do not overwrite the existing species. You now have a material with exactly the same properties as water-liquid. In the mixture panel you still have to select some properties of the mixture (in materials under Material type you can select mixture) and the species so delete all species in the mixture (next to Mixture species it says 'names' next to this there is a button 'edit') exept for dye and water-liquid make sure water-liquid is last in the list because this will be the bulk fluid. Now you can put the dye species in the flow field by first marking the region where you want them to be by choosing Adapt->region fill in the coordinates and press mark, then goto Solve->initialize->patch and choose dye, fill in the value and select the register to patch and press Patch,now solve (iterate) the dye and flow field with the unsteady solver and you will get the dispersion of the dye in time.

Re: How to introduce a tracer
 

hallo nico, thks for giving step by step procedure. sorry for responding very late. i have some more question in my mind. i want put some small quantity of dye in the tank as slug dose(putting dye instantly or over a very small time say 30 sec), and then want study the exit concentration at the outlet. hence, how to put dye instantly or over time less than 30 sec? i am waiting for step by step procedure help. thks l.g.patil

Re: How to introduce a tracer
 

Another option: You don't have to patch. You can use the Discrete Phase Model and create a injection from e.g. a surface. Once you have created an injection of particles with the same properties as your other stuff has, you have various possibilities to sample them, e.g. at another surface. (report/discrete phase/sample and histogramm. So first you have to sample. This can take very long and is NOT possible in batch-version. Afterwards you can plot e.g. histogramms of the concentration.

Good luck, Yvonne

Re: How to introduce a tracer
 

hallo Yvonne, please give me some more information about tracer injection. i have read your answer but i could understand completly. pl give me step by step procedure. Previous suggestion was very clear, i could do that very easily. hence i request you to give step by step procedure. thks

Re: How to introduce a tracer
 

Hi again! You can't use the online help or the fluent user's manual? It's written there step by step. If not, I will try to write everything more helpful:) Yvonne

Re: How to introduce a tracer
 

hi, presently mannuals are not with me. hence .. pl...

i wanted to plot outlet exit concentration verses time(unsteady)but fluent stores the results at required time intervals in a seperate files.(filename0001,filename0002,...etc.) hence how plot the concentration v/s time? is there any shortcut method or command to plot? waiting for your reply

Re: How to introduce a tracer
 

Hi rslgp (what does it mean?)

Ok, step by step: Selcect a tracer weith the same properties, as Nico explained. than Define/models/discrete Phase: number of steps (start with about 500) injections: create, surface, inert particle, turbulentdispersion: stochastic tracking (1 try) shut everything with OK

than Report/discrete phase/sample, click the surface and the injection, Compute, when finished reprt/discretephase/histogramm/read there should be a dpm-file with your surface-name, select! Click time and than PLOT You should get your wanted diagramm. But you can also use the dpm files in excel and do further work with them.

Hope that was more helpful, good luck, Yvonne

Re: How to introduce a tracer
 

i will try now. thks for your help. bye

Re: How to introduce a tracer
 

Hi again! Just a question: are you and Hsing-Ping (or kevin-1) the same person?Its a little bit confusing. Yvonne

Re: How to introduce a tracer
 

hi, i am l.g.patil from india, presently doing PhD at IIT bombay. bye

Re: How to introduce a tracer
 

hi, Yvonne, what value i have to input for mass diffusivity of water in mixture pannel? what is meaning of binary diffusity of water(the value given in fluent=3.05e-05)? i am using k-e model. therefore i feel that i have to give turbulent diffusity coeff. there pl. give correct value to be inputed into mixture pannel(water-dye, dye has same property as that of water-liquid) waiting for your reply. bye

Re: How to introduce a tracer
 

Hi! Puh, I had the same problem and I'm not completly sure, whether my solution is right or not. As I understood it, the binary diffusivity means the diffusivity water,liquid-water-vapour. If you have water,liquid-water,liquid, it should be something like 3e-9. If there's no data existing for your specific problem, I would use this. If there's is anybody having a better idea...please reply:) Hope this will help, bye, Yvonne

Re: How to introduce a tracer
 

Hi Patil,

This is Rajeev from India, Ranchi, Jharkhand

I guess from the messages here that you were trying to generate the RTD curve for your system.

I had done the same for steel flowing in tundish. Generally I use species transport model. In the model when you take mixture, try to generate a mixture of non-reacting species with your major medium as the last one. For example in my species model I use n2 and liquid steel. I remove all others. Then I change the property of n2 to that of steel and finally the property of mixture to that of steel.

After this you create monitor surface at your outlets. I used mass fraction of n2 x 1000000 to convert my values to ppm, and I was monitoring them at each flow time. Write this in a separate file.

Finally before you start go to the inlet boundary condition and change the species flux to 1.

Run the solution for 1 time-step. Stop it. Again go back to inlet boundary condition and change the species flux to 0. Then run your solution for the total number of time steps.

So this way you can create a small injection.

The files written the monitor surface panels will give you the concentration at the outlet which you can use for your analysis.

Hope this helps. Bye

Rajeev

Re: How to introduce a tracer
 

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.

Re: How to introduce a tracer
 

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.

Re: How to introduce a tracer
 

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

Re: How to introduce a tracer
 

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

Re: How to introduce a tracer
 

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

Hi Thomas,

Please explain your procedure.

pulse tracer input
 

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

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"...

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!!!

Tracer studies for solid particles
 

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

RE; RTD using Tracer in species trasport model
 

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???