Expression for physical timescale
From the help file under physical time scale chapter,
"It is often necessary to alter the physical time scale for buoyancy driven flows in order to achieve convergence." So max physical time scale will be : delta(tmax)=(dL/(B*g*deltaT))^0.5 here L is a length scale associated with the vertical temperature gradient; deltaT is the temperature variation in the fluid; B is the thermal expansivity of the fluid; g is the gravity So an expression for the physical time scale is needed. But for a 3D model with nonuniform mesh ,how to define the CEL of the physical time scale? how to define dL here? deltaT is radial or vertical temperature difference? 
The equation just gives a first guess estimate. If you could not be bothered working it out you can just make a guess (1s is a good starting point) and just go from there. Obviously a bit of trial and error and not very efficient but should be OK for most cases.
Often the time scale size makes little difference in steady state simulations. 
From the original sentence, "it's often necessary to alter the physical timescale", so I do not need to use a CEL language to alter it from time to time? just use a fixed number for example 1s?

Yes, just a fixed number. I change it while the simulation is running (using solver manager) so I can adjust the timestep easily and adjust it if it looks too big or small without having to restart.

so I guess you use "Edit Run in Progress" under "Tool" Menu.
During the running, I found RMS of U,V,WMom and Henergy is one order higher than MAX, for example rms=2.5e06 and max is 1.4e04, how shall I modify the physical timescale? 
1 Attachment(s)
the location of high residuals is not very far from the place I am interested in, so I guess this is a local problem. WHile from the attached graph, I do not have poor grid quality, so what kind of step can I do to fix this problem?

Do a sensitivity study. Do a simulation using your current convergence, and a second converged to maybe a factor of 10 better. Did values of interest to you change significantly? If not then your current convergence is probably OK.

Now my convergence criteria is 1e06, so your suggestion is getting to 1e05 and see the result?
I have done the grid independent study, the mesh is ok. And from the help file, it says"When you are having problems converging, you can check RMS and MAX residuals" I can converge to RMS 1e06, while my MAX residual is more than one order higher than RMS, so is this a local problem or we can just neglect it since its convergence Thank you 
Yes, you can also compare against a run with looser convergence. The aim is to see whether convergence makes any difference.

The temperature and velocity distribution shape are the same, only I got slightly higher temperature in lower convergence criteria. So do you have any comments on this. I can converge while still there is one order higher between RMS and MAX residual, does it matter? THe MAX residual show near the region of interest

I cannot comment on this  it is you to decide. Is the difference between the tight and loose convergence significant for the results you are interested in. Only you know what you are interested in.

All times are GMT 4. The time now is 08:30. 