Auto Timescale is a fluid timescale control option that uses an internally calculated physical time scale based on the boundary conditions, flow conditions, physics, and domain geometry. Information on how the CFX-Solver calculates the Auto Timescale is available in Automatic Time Scale Calculation in the CFX-Solver Theory Guide

Auto Timescale is the default timescale control setting. However, be aware that the Auto Timescale calculated by the solver is often conservative. This is usually robust, but faster convergence is often possible using a more aggressive setting. This can be done by:

It is also worth noting that, in some instances, the internal time scale calculation fails to find an appropriate velocity or length scale on which to base the time scale. For example, a buoyancy-driven flow problem can be specified using a Subdomain heat source in a cavity. If no velocity field or temperature difference is specified, a very large time scale (several orders of magnitude) can result. If this is the case, then you should try either:

SOLVER CONTROL:
  CONVERGENCE CONTROL:
     Maximum Number of Iterations = 300
     Timescale Control = Auto Timescale
     Timescale Factor = 1.5
     Number of Timescale Updates = 12
     Timescale Update Frequency = 7
     Maximum Timescale = 5 [s]
     Timescale Ramping Factor = 1.3
  END
END

The Local Timescale Factor option enables different time scales to be used in different regions of the calculation domain. The value you enter is a multiplier of a local element-based time scale. Smaller time scales are applied to regions of the flow where the local time scale is very short (such as fast flow), and larger time scales to those regions where the time scale is locally large (such as slow flow). The default value is 5. Any value 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 timescales may locally result for small elements or large aspect ratio elements, which may in turn reduce the overall convergence rate. For this reason, it is best used on meshes of uniform element size and moderate aspect ratios.

The Physical Timescale option enables a fixed time scale to be used for the selected equations over the entire flow domain.

In general, there are two situations in which you would use a physical time scale:

For advection dominated flows, the physical time scale should be some fraction of a length scale divided by a velocity scale. A good approximation is the Dynamical Time for the flow. This is the time taken for a point in the flow to make its way through the fluid domain. For many simulations, a reasonable time estimate is easy to make based on the length of the fluid domain , and the mean velocity , for example:

(16–1)

For external flow, should be based upon a characteristic geometric length (for example, chord length).

If the domain contains largely varying velocity and length scales, you should try to estimate an average value. If you get divergence, check in the CFX-Solver Output file that your time scale is not larger than the Advection Time Scale value given in the Average Scale Information at the end of the run. A "small" time scale can be considered to be less than 1/3 the smallest length / velocity scale in the simulation. Values higher than this can be considered a "large" time scale.

It is often necessary to alter the physical time scale for buoyancy driven flows in order to achieve convergence. The maximum physical time scale may be estimated using the following relationship:

(16–2)

where:

Physical time scales that are too large are characterized by bouncy convergence or results that do not converge. Time scales that are too small are characterized by very slow, steady convergence.

Depending on your initial guess, a significantly smaller time scale may be required for the first few iterations of a problem.

A judicious physical time scale value usually gives faster convergence than specifying a Local Timescale Factor value.

If you use an expression for the physical time scale, it must evaluate to a constant value. CEL variables are available to control the time scale depending on the iteration. For details, see Timestep, Timestep Interval, and Iteration Number Variables in the CFX Reference Guide.

When using the Auto Timescale option for the Solid Timescale Control, a Solid Timescale Factor is used. The default value is 1. How this value is used to calculate a solid time scale is described in Solid Time Scale Estimate in the CFX-Solver Theory Guide.