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.

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.

Yes, it's interesting

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

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

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

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

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.

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

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

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

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

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

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

i will try now. thks for your help. bye

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

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

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

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

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