Can I calculate RTD when I am using a turbulence model or I have to use a different model. If different model has to be used to find the RTD then which one is most appropriate.

Has anyone tried the above problem. Please let me know the steps.

Thanks in advance Rajeev

I can't see the relationship between residence time and turbulence models ?

In my point of view, residence time deals with mean velocities. So, you can calculate a residence time for your flow with any turbulence model.

Can you give more precision on your problem.

Best regards

Are you referring to http://www.fluent.com/solutions/examples/x93.htm

then track the transient dispersion of a tracer species.

You can do it by particle tracking for the partilce of very small particle. Then slip velocity can be negligible, so that particle residence time is nearly same as gas residence time. Then you can obtain RTD.

For reference, my approach is as follow.

1) set the particle size very small(e.g., 1.e-09) 2) set the density of particle as mean of gas phase.

Sincerely, Jinwook

How can I achieve a dirac (delta) signal in the simulation?? Can I also realise that when I am using translational periodic BC ?

The best way to do it is to use the DPM model with very small particles. Also turn on the stochastic model so you can get a smooth RTD. With more than 500 particles you can get a pretty decent RTD, but be sure to turn off the length scale option and use the tracking steps (>20) so particles spend enough time in each cell. The average RTD should be close, but not exactly, to the mean residence time. If the display option takes a long time, then try the DPM sampling and histogram option. It is lot faster.

You can also use a fluid as a tracer. It's quite faster than particle tracking.

This is my method :

1. calculate your solution,

2. Enable multispecies model

3. Create a species "tracer" as a copy of your fluid.

4. "Inject" your tracer in the domain at a boundary or by using the patch command.

5. freeze your solution except for species (disble equation in flow solver) and then run in transient mode.

6. You can obtain a RDT by local value (probe) or mean value at bourdary (surface averaging).

Best regards

Two problem with this method: 1. Transient simulation is needed to compute RTD at the outlet, which could be quite time-consuming. 2. More cells are needed for accuracy due to numerical diffusion.

Thanks a lot guys.

One more question. What should be the correct steps.

1. Calculate the steady state flow field based on turbulent model. Once it converges. then

2. Switch on the DPM. Use the calculated flow field in step 1 and solve for unsteady state the particle concentretation at outlet to get the RTD.

Correct me if my steps are wrong.

Thanks again Rajeev

Not the particle concentration, but the time variable at each particle.

...and it does not have to be unsteady! or I am wrong?

Correct.