My calculation took a very long time to get converged. The residual always fluctuate and reduce very slowly. How can I get a faster converged result? Should I change the time scale (now I use auto timescale)?

Maybe you need to refine your mesh at proper position of your domain.

Hi Twiti,

Try switching to a Physical Timescale. A good start would be 10x the Auto-timescale, which tends to be a little conservative. Another trick is to write a backup file and generate streamlines in Post. Use the calculator to calculate the lenght average time on the streamline, then use this value.

For more advice on timescale selection, search this forum or read the tech tip Monitoring and Improving Convergence on the CFX Community Site at http://www-waterloo.ansys.com/cfxcom...onvergence.htm.

Regards, Robin

more data for your reference, (copy from Solver_Models.pdf. page369 Later Problems)-- In many cases, global quantities will stabilise within 20 to 30 timesteps, but convergence will not be achieved until approximately 100 timesteps have completed. For most applications, convergence should be achieved (or well on its way) within 200 timesteps. If you have problems with convergence, you should find the source of the problem rather than taking the results as they are. There are many factors that may lead to poor convergence, including poor mesh quality, improper boundary condition selection and timestep selection to name a few. If you are unable to diagnose the source of your convergence difficulties, contact your technical support representative for advice....(pls see it more in pdf)

Hi,

you should probably give some more specifics on the flow and physics.

The auto time scale sets the time step for all transport equations to 1/3 of the global advection time scale. There are many characteristic time scales in a problem and the global time scale is perfect for simple flows like uniform flow in a cube. The length scale taken is the cube root of volume and the velocity scale as average velocity. When the local time scales and other physics deviate from this ideal then you have to do other things. Sometimes you have to use a larger time step, sometimes smaller.

When you add other physics you also introduce time scales of those processes....not all of which are solved active but are lagged from previous iterations.

The larger time step works well for "constant property flows" where none of the information is lagged.

What does your bouncing look like? How many is a lot of iterations?

Try several different physical time steps maybe advection time, 1/5, 1/20...etc and analyze!

Lots of possibilities............Bak_Flow

Thank you for you kind help, Kiddo, Robin and Bak_Flow. As Bak_Flow mentioned, my problem is the mixing of two stream with large different velocity, which may lead to two different time scale. May be I should try 1/2 of the smaller time scale as the Physical Time.

Hi,

do let us know what works for you!

Bak

I refined the mesh in some critical region and set a physical time scale about 1/3 of the cycle time which is a litter larger than auto-time scale. It seems that the convergence is faster, but still not as expected. I am trying another methods...

Hi Twiti,

Increase you timestep by another factor of ten and see what happens. Often you can get away with a very large timestep, at least to get you through the startup transients, then drop the timestep if the residuals fluctutate very rapidly.

Regards, Robin