what is the meaning of physical time scale in steady state simulations and how do i set it for ADDITIONAL VARIABLES.Is physial time scale * no of iterations the real time for steady state to be achieved.or can it be varied indepentant of any physics to suit convergence.

Physical time scale is a pseudo time step, definitely not the real time. You may backup the results file to have a view of the development of fluid flow when you are running a steady state simulation, but it doesn't give you the real time information. Comparing with the solutions of a transient state and a steady state, there is a relationship between the real time information of the transient flow and the under-relaxation factor of the steady state, which might be the way that the 'physical time scale' is worked out. I would rather treat a physical time scale as an under-relaxation factor. But this under-relaxation factor can be much bigger than 1.0 for fully-implicit solver. The larger it is, the quicker for the solver to solve the physical problem if there is no convergence problem ahead. If you have no idea about the physical time scale of your problem, you can try the 'auto timestep' if there is the option. I am sure that experts here will correct me if I am not right on the point. Regards Yingchun

Hallo Everyone!

I´ve got another question about timescaling. I have a model with a fluid and a solid domain and I want to solve heat transfer (no hydrdynamic equations). I found out that I get a correct solution when I set physical timescaling with 0.5 s per time step for the solid and automatic timescaling for the fluid. I get an incorrect solution when I set both to auto timescaling. Has somebody got an explanation for this? Any comments appreciated!

Thanks in advance. Alexandra

Hi,

are you interested in a time accurate transient evolution of the problem? If one is interested in the transient behaviour all of the equations must march at the same time step.

If one is only interested in the steady state solution, the time step is effectively a relaxation parameter. The "warped time" evolution will differ when different time steps are set for different cells, however, the steady state solution should be the same.

When you set auto-timestep the code will calculate characteristic time scales for the solid and fluid domains. They are going to be different.

What is the problem you are solving, what is the analytical solution?

Regards,

Bak_Flow

Hi!

I'm sorry I forgot to say that I'm doing a steady state simulation. My problem is rather simple, it's just a test case. I have a fluid with a thermal conductivity and a solid with a different thermal conductivity. The solution should be two linear domains of temperature distribution. But the are not linear at all when I use auto timescale for solid and fluid. Alexandra

Hi Alexandra,

When you choose auto-timescale for both, the solver probably hasn't converged. If this is not the case, you may want to add a conservation criteria of .001 or smaller. It is possible that the heat transfer through the solid is so slow that the residuals converge before a steady state is acheived.

Generally, I wouldn't use autotimestep for the solid. You can usually come up with a better estimate of the timestep yourself based on the maximum thickness (L) using the equation:

L^2/alpha

where alpha is the thermal diffusivity. In fact, the equations are so stable in the solid that you can often get away with an even larger timestep.

Regards, Robin

dear users,

actualy i am to simulate pure diffusion of oil in a solvent which is quiescent.so no hydrodynamic eqns.only transport eqn for additional variable oil conc is set for .the diffusive time scale is very high something like 500 s.am i correct in setting so because often the time scales are of order 0.1 etc. soubhik