The flow is steady. I have computed the field of velocity. How to obtain residence time distribution function (RTD) using Virtual Reality or plot it by Autoplot? Certainly, I can add "pulse input traces" in the INLET and solve transient problem for concentration with stored velocity field. The outlet curve of concentration after normalizing is the residence time distribution function curve as it described in Y. Yang, D.T. Hartman, M.A. Reuter "CFD Simulation of Residence Time Distribution of a Rotary Kiln Waster Incinerator", PHOENICS Journal, 2001, Vol.14, No.1, pp.82-111. But the method is long. I think there should be more convenient and short way of computing residence time distribution by tools of PHOENICS interface, e.g. VR or Autoplot. Say, we can plot streamlines in VR Viewer without adding particles and solving transient problem, as the streamlines are determined if the steady field of velocity is fixed. So, the residence time distribution is also determined if the steady field of velocity is fixed, and no need to run the transient problem for concentration or particles adding to the INLET. The problem is how to do it?

There is a rather neat way to do this.

Solve an additional variable called (for instance) TIME. Define a source of TIME over the whole field, with a fixed-flux source with value unity. The resulting field (which you can plot with the Viewer or with Photon) shows you the residence-time distribution.

Effectively, you are solving a transport equation of the form

d(TIME)/dt + convection + diffusion = 1

David Glynn

Flowsolve

The procedure for calculating the residence time that you describe as 'pulse inlet traces' corresponds closely to the way residence times are measured in practice. First a steady-state solution is obtained for the hydrodynamics. Next, a transient calculation is carried out starting from the hydrodynamics solution and solving for a single scalar quantity, C1, which enters in a short pulse and is then convected out of the domain. Since only one equation is solved I found this method to take relatively little computer time even for large 3d cases. I recommend using the CGR solver wholefield for C1 with plenty of iterations, because then very few sweeps will be required per time step for convergence. A higher-order scheme is also beneficial for numerical accuracy.

There is another method termed 'time-since-injection' which solves a steady problem via the conservation equation DT/dt=1 where T is the time since injection. However, although this method is very efficient, it can produce very inaccurate results under certain conditions, e.g. when recirculation zones are present within the apparatus.

As I think you also suggest, the tracking of massless particles with GENTRA (Lagrangian particle tracking option) is another method; but this leads me to say that your idea of retrieving the residence time from the streamline computation in the pre-processor seems to be a good one, especially if the streamlines were colour contoured according to their flight time. The local velocity and the distance travelled is known, and so it ought to be possible to recover a measure of the time. How to do it? This depends on how the streamline algorithm has been coded in the VR Viewer and how the required information has been stored, if at all. The best that I can do is pass your suggestion on to CHAM's development team.

Dear David Glynn and Michael Malin, As for solving extra scalar variable with setting its constant source all over the field in order to obtain the field of residence time distribution, it really works!!! I followed the way you recommended and did it. But it doesn't seem to give accurate results for outlet, especially if the outlet area is rather small. It is practically impossible to draw the final curve of function of residence time distribution (e.g. in the outlet). This method if efficient when we want to estimate the field of residence time distribution all over the domain, but not for obtaining the final function of residence time distribution. I got my doubts, that GENTRA and streamline calculations would give accurate results. So, the best way is to use "pulse inlet tracers" e.g. a transient calculation starting from the hydrodynamics solution and solving for a single scalar quantity, C1, which enters in a short pulse and is then going out of the domain. Using CGR solver whole field for scalar and higher-order scheme appeared to be really beneficial for numerical accuracy. Thank you. I will be glad to receive more ideas on the problem. Roustam