i have a steady state problem (bouyancy dominated flow in a room), however the nature of the problem requires me of using transient simulation; i chose time step to be 10 seconds while the time domain was put to 5 min, i use k-e model. the residuals achieves the E-3 criteara for all the timestep. At 3 mins, the results are in VERY good agremment with my measurements, however if the simulation is kept running for 5 mins or 10 mins, with 10s time step. the results slowely goes away from the measurements; my understadning was that at some points, the results for a trasient solution wont change anymore

is it acceptable to consider the simualtion setip for a 3 min (timestep=10s) that gave VERY good agremment with my measurements as acceptable???

will increasinf the timestep do anything?

many thanks for your time

Your time step should be less than the critical time scale of your domain (at most equal).

my time-step is set to 10 seconds; iam not sure what u mean by critical time scale of your domain?? my transient runs from Ts=0 to Te=300 seconds for five minutes in total

thanks

(bouyancy dominated flow in a room) How did you select 10s as your time step? What is your reference length scale? and what is your reference velocity scale? without knowing these data one cannot decide what is the appropriate time scale (critical time scale) for your flow domain.

Explain you problem in a little more detail. What exactly is happening over time, and do you expect to reach a steady state? Why do you need a transient solution?

No, unfortunately you cannot simply stop at 3 min and then say "This is my result". The fact that your solution happens to match the experiment at one point could be completely random.

Increasing the time step won't do any good unless you are looking for a steady state (in that case it's not a time accurate solution). You should try to decrease your time step and see if the solution changes. If the time step is small enough, the solution should not change even if you further decrease the time step.

the problem is a 9-by-9 room with 25 occupants it uses a two displcament ventilation diffusers supplying at 117 L/s and 15.1 C; the problem is steady-state, however due to the fact that physics of the problem (the physics of buoyancy dominated flow) is transient by nature; So i think the correct way is for this steady-state case is to use an unsteady simulation (i.e. quasi-steady state). based on a reliable past work, i have chosen the timestep 10s, which i think is correct.

1) i can get convergence using strictly steady-state simulation by modifying the URFs, and at 1,200 iterations for (k-e model) the solution residuals pass the E-3 and E-7 for energy, but if the simulation is kept running for a while longer the continuity doesnt seem to be able to pass the E-4 and actually slowly rises; that leads me to think i must try transient simulation; and for the same steady-state simulation when i improve the mesh from 400,000 elements to ~800,000 elements (to check for grid independecne), there is no improvment and slight disimpovment

2) so i have tried to use transient with 10s timestep for a total of 10 minutes; @ 6 minutes the variables seems to get steady; but my numerical doesnt agree with measurements at the heights of 1.2m, 1.8, and 2.25m. i should mentiond that in either case the discrepency of my CFD and measurement is within 10%.

many thanks for your time

Looking for a transient solution makes sense only if you expect the flow to be unsteady even after a long time (for example, reaching a periodic state). I don't see why this should be the case, unless your analysis is so accurate (fine grid and time resolution), that you actually capture local flow instabilities (unstable shear layers...), in which case the solution will never become steady. However, if your transient computation yields a steady state, as you point out, this final solution ought to be identical to the one you get from the steady-state computation (if converged), simply because at steady state your time accurate equations reduce to the steady-state equations. How you get to that steady state is irrelevant for the solution. So, again: It only makes sense to run unsteady, if there is no steady state, even after a long time, or if you're actually interested in the initial transient behavior. That doesn't seem to be the case, here. The instability of your steady-state computations could be related to misbehaving boundary conditions or the turbulence model. I think that's more likely than the chance to encounter actual physical flow instabilities with such a coarse spatial and temporal resolution. Besides reaching a converged solution: How accurate this solution will be depends on a variety of factors. If it's a steady state, transient behavior does not factor in. Grid resolution, accuracy and adequacy of all boundary conditions, and the accuracy of the turbulence model will be important, regardless of how you get to that steady state (by transient or direct way).

OK, you have two inlets, each has a hydraulic diameter (reference length scale) and a definite mean velocity (reference velocity) from these you can get your reference time scale then compare that to your time step. Cheers

thank you for both of your comments. its greatly appreciated; though i have been over the BC many times; to tell u the truth the BC are not very complicated; they are only walls with specified surface temperature and the diffuser are modelled using Momentum method. my point is the BC are simple and i can think f anything being wrong with them;

running steady-state using pre-describe URF(0.3 for pressure and 0.7 momentum) gives oscillations at certain time and the continuity will never reach 10-3. then when i change the URF to 0.3 for pressure and 0.7 momentum, all my residuals converge nicely @ 10-3 and 10-7 for energy, though at some point the continuity's residual start to rise again!!