Hi experts,
Just had a quick question--I have been doing steady simulation but why do I get the following in the post-processing? I see that there're five frames with different plots. I have specified 500 timesteps in the input file.
Hi Prabin,
When you specify the number of time steps is 500.
But the default value for writting result interval in Field Ouput dialog is 100 by default.
It means that after each 100 steps, you get a single frame.
Best regards,
James
Hi Prabin, When you specify the number of time steps is 500. But the default value for writting result interval in Field Ouput dialog is 100 by default. It means that after each 100 steps, you get a single frame. Best regards, James
I would also suggest that if you're running 500 steps, and still not converging to a steady-state solution, maybe the flow is actually transient. You can try decreasing 'Steady update factor' in Solver Controls to 0.5 or 0.4 to see if that 'damps the wiggles' enough. But if not, maybe it really is transient - or you can determine yourself to accept the solution as steady-enough without switching to transient.
In addition to the output frequency issue method, the issue here is likely that there is no steady solution to this particular setup/settings.
Some physical phenomena do not have a steady state solution. Generally AcuSolve converges in 100 iterations for most problems. I have never used AcuSolve till 500 iterations for steady state. So it is running till 500 iterations, there is definitely something going on. Either bad mesh, incorrect settings, too fine convergence tolerance or its just transient by nature.
Please check the "Solution Ratios" in the Plot utility of HWCFD or AcuProbe. They might be around 0.1-0.05 values. Please post your .inp and .Log if possible. If not, bare minimum would be screenshots of residual ratios and solution ratios.
In addition to the output frequency issue method, the issue here is likely that there is no steady solution to this particular setup/settings. Some physical phenomena do not have a steady state solution. Generally AcuSolve converges in 100 iterations for most problems. I have never used AcuSolve till 500 iterations for steady state. So it is running till 500 iterations, there is definitely something going on. Either bad mesh, incorrect settings, too fine convergence tolerance or its just transient by nature. Please check the "Solution Ratios" in the Plot utility of HWCFD or AcuProbe. They might be around 0.1-0.05 values. Please post your .inp and .Log if possible. If not, bare minimum would be screenshots of residual ratios and solution ratios.
Thank you all for your responses.
This is just a series of tests that I have carried out starting with max_time_steps=100,200,300,500. I believe that the solution has already converged here but I am investigating whether I am able to meet the convergence tolerance of 0.0001 (I have specified convergence_tolerance = 0.0001 and max_time_steps = 500) for this problem. The flow is laminar. The solution and residual ratios plots are:-
I have run other simulations with exactly same parameters except max_time_steps = 300. I just wanted to investigate on the stability of the surface integrated heat flux (I want it to be correct upto at least 3-5 significant digits.) I have included the data for 500 timesteps for surface integrated heat flux as body_fitted_srf4.txt. I see variations in the value of surface integrated heat flux output at different timesteps although the solution is converged.
Moreover, I have also attached the log file and input file for your reference.
Thanks.
This is the solution and residual ratios for another problem. I see wiggles here not converged to a stabilized solution. Do you think this is fair enough to say converged?
This is not a converged solution.
Solution ratios of velocity are really high. That means that the velocity field is varying by 20-50% for each time step. So it seems that running a transient simulation is essential to know what is happening here.
Seems like the problem is inherently transient. Are you trying to simulate natural convection?
Thank you for your analysis. Yes, I have a convective heat transfer coefficient defined at the top surface of the domain. I will retry the simulation in a transient mode.
