Hi all,

I am trying to solve a case with a large volume with 1 to 10 kg gas inside. The inlet flow is approximately 1e-5 kg/s. The outlet flow and thus the total hold-up is determined by the pressure near the outlet. However, the outlet is located in a region with Mach >1.

The problem is that I need large timesteps to get a decent mass balance and to predict the total gas holdup. On the other hand I need small timesteps as the physics near the outlet geometry require small timesteps.

Any suggestion or workaround? Maybe the solution is not a CFD-solution.

Astrid

Hi Astrid,

Do you need the large domain? Sounds like you can make a reasonable approximation of total pressure close to the outlet.

As for the timestep, try running with a local timestep factor of ~10 until you get the residuals down, then continue with a small timestep.

Robin

Hi Robin,

- Yes, I need the large domain. The pressure distribution in the volume and thus the hold up determine everything. I can make a reasonable approximation. The problem is that I was asked to give a better approximation, using CFD.

- I will try the local time step factor. As it is not possible to specify a time scale in combination with the local time step factor, I was wondering how the minimum and/or miximum is determined by CFX5.5. Is the minimum the usual auto time scale and the maximum 10 times larger? Or just the other way around?

Astrid

Robin,

can you give an answer on my second question in my previous posting?

Astrid

Hi Astrid,

Direct from the documentation (a handy thing, wouldn't you say):

Local Timestep Factor

This option allows different timestep sizes to be used in different regions of the calculation domain. The value you enter is a multiplier of a local element-based timescale. Smaller timesteps are applied to regions of the flow where the local time scale is very short (e.g. fast flow), and larger timesteps to those regions where the timescales are locally large (e.g. slow flow). The default value is 5.0. A values less than this can be considered a small timestep.

This option is very useful when there are widely varying velocity scales in the simulation, for example, jet flow into a plenum chamber. The main disadvantage of this method is that very small time steps will be applied to small elements, potentially reducing the overall convergence rate. For this reason it is best used on meshes of uniform cell size.

The element-based timescale is literally the time it takes the fluid to cross that element (for advection at least). In terms of advection, the local timescale factor is effectively the CFL number. The code will also consider the diffusion and conduction timescale when making the calculation, using the largest of these. This insures that if you have a conducting solid, or the rate of diffusion is much greater than advection, the appropriate timescale will be used.

Just a reminder though, converging with the local timescale selected will not give you proper results. You can use this to the solution moving along, but you must switch back to a physical or automatic timescale and run it to a final converged solution.

Regards, Robin

Thanks Robin. Of course I read the manual but I was not really satisfied with the answer. Your last reminder is usefull!

Astrid