[Chander]

I am simulating steady state turbulent conjugate heat transfer problem in CFX. I am facing some convergence problems (residuals stabilize before reaching convergence criteria). I have gone through the FAQ regarding this available under CFD wiki ( http://www.cfd-online.com/Wiki/Ansys...gence_criteria) and tried to play with the time-step being used by the CFX solver.

Now I observe the following
1) With Automatic Timestep calculation, I am able to get convergence for my simulations if I reduce the Timescale factor to 0.1. So whatever automatic time-step is calculated by solver, I multiply it with 0.1.

2) I tried to get an idea of the physical time-step by plotting streamlines and observing the time variable on the streamlines (as outlined in the CFD wiki link above). However, the flow is very complex consisting of 3-dimensional vortices and the physical time estimate from streamlines is very large. And choosing a time-step based on a fraction (1/3 to 1/5) of this physical time leads to a large time-step and solver failure

3) Choosing the local timescale factor of 4 leads to very slow convergence.

I have asked similar question before on this forum. However, I have come back as I am not sure what I am doing is right.

My question is:
a) Is it fine to get convergence by such large reduction (1/10) in the automatically calculated time step? I have repeatedly checked my mesh and set-up and I have not been able to find any problem with that. I have also checked that I am not resolving any transient behavior in my simulation because the period of oscillation of residual changes with change in time-step.

b) The transient formulation being used in CFX for steady state simulation is fully implicit (correct me if I am wrong). Then why does the convergence behavior depend on choice of time-step? Isn't a fully implicit discretization unconditionally stable?

c) moreover, why should attainment of steady state depend on choice of time-step? Theoretically one can use as large a time-step as desired.

[Chander]

Anyone please...

[Florent]

what is your configuration?

[ghorrocks]

a) You can use any time step you like to get convergence. A larger timestep will usually get there quicker, that is why it is recommended.

b) Yes, CFX is fully implicit (although there are some physics models which are not, such as surface tension and particle tracking, but that is another matter). The importance of time step size is that is what CFX uses to stabilise the equations. A SIMPLE based solver uses under relaxation factors. CFX uses time step size.

c) Just as for under relaxation (URF) on SIMPLE based solvers, you want to use the largest URF which converges reliably. Then you often reduce it a bit for safety. Likewise in CFX you use the largest timestep which converges. As you approach convergence the equations often become more stable, meaning that you can increase the timestep size.

This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.

[Chander]

Originally Posted by ghorrocks

This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.

Thanks Glen again for the detailed reply. It clarified a lot.
I have one query here. In my simulations, I find that convergence stalls and when I reduce the timestep, it goes towards convergence. But when I reach near convergence I have to keep the time step small until the convergence is reached.
This is because in one of the simulations I tried the following:
1. I first got a solution with reduced time-step.
2. Then used this as initial condition with a larger time-step. The residuals actually went up and stabilized at the higher level (inside the red circle)! Does this point to some error in problem setup?

[ARohit]

[QUOTE=ghorrocks;305513]a) You can use any time step you like to get convergence. A larger timestep will usually get there quicker, that is why it is recommended.

b) Yes, CFX is fully implicit (although there are some physics models which are not, such as surface tension and particle tracking, but that is another matter). The importance of time step size is that is what CFX uses to stabilise the equations. A SIMPLE based solver uses under relaxation factors. CFX uses time step size.

c) Just as for under relaxation (URF) on SIMPLE based solvers, you want to use the largest URF which converges reliably. Then you often reduce it a bit for safety. Likewise in CFX you use the largest timestep which converges. As you approach convergence the equations often become more stable, meaning that you can increase the timestep size.

This means it is very common to start a CFX steady state run with a small timestep and run that for a few iterations to set the flow up, but then start increasing the time step size as the flow settles down. As you approach convergence you can often be running time steps 100 or 1000 times larger than you started with. Use the "Edit run in progress" feature of the sovler manager and you can do this without stopping and restarting the run.[/ Sir, I am also having the convergence problem. I have attached image here. When i reduced time step, residuals actually went up. why? ]