a positive net change in the number of wet nodes does not occur as a result of the time step, even though the inlet flow rate is not zero

This is an indication that Equation 21–1 has not been integrated over a period of time that is long enough to allow new nodes of the domain to reach the threshold, and so a larger time step needs to be applied. In this case, the time step index is not incremented, is increased by 50%, and the calculations are run again to compute the field. This process can be repeated up to 10 times for a particular time step, after which point the simulation is terminated.

the ordinary flow calculation returns an error (for example, divergence is detected for a nonlinear problem)

In this case, the time step index is not incremented and the flow calculation is attempted again using a smaller value of . If no new wet nodes result and the calculation still diverges, the algorithm will eventually stop.

the calculations for a time step yields a positive net change in the number of wet nodes

This represents a successful outcome, and so the time step index is incremented. Having computed a new wet node flag vector (which yielded a new volume of fluid in the domain) as a result of the inlet flow rate , a new value for is calculated for the next time step as follows:

(21–2)

where is a parameter you can set to control the accuracy of the scheme. Recommended values of are on the order of 0.2–0.5. Note that an extremely low value of can reduce the time step to such a degree that no new nodes become wet; consequently, the time step will be increased as described previously, and you then run the risk of engaging in an oscillatory "forward/backwards" marching scheme that calculates several useless iterations without improved accuracy. An inherent limitation of the VOF model is that it cannot process changes that are smaller than the element size.

Note that if the inlet flow rate for the time step was 0, Equation 21–2 is ignored and is set to the value you defined for the initial time step.

the time step index is incremented beyond the maximum number

In this case, the simulation is terminated. The maximum number of time steps is used to stop simulations that have values for that are too low, and consequently run too long. Because of the Courant-type limitation described previously, you should expect a complete filling simulation to take several hundreds time steps and set the maximum accordingly. By default, the maximum number of time steps is set to 200.

is set to a value lower than the minimum

The simulation is terminated when falls below the minimum.

the total outlet flow rate (integrated over all outlets) is 99% of the nonzero total inlet flow rate (that is, the flow in the cavity is established, but almost all of the fluid is leaving the domain)

By default, Ansys Polyflow stops the simulation in such circumstances, even if the cavity has not been completely filled. In most cases, it is considered normal to terminate a VOF simulation when the flow exits the domain. The value of 99% is hardcoded in Ansys Polyflow; while this value can be revised in the data file, it is recommended that you do not change it. This constraint is disabled for simulations in which there are no defined inlets, thereby allowing you to model the emptying of the cavity. You can also ignore this constraint by clicking the Disable ‘Stop When Full’ criterion menu item in the VOF iterative parameters menu, as described in step 8.(a)viii. in Problem Setup.

the fluid fraction variable exceeds the threshold value (for example, 0.5 when tracking a single fluid) throughout the entire domain

As stated previously, the fluid is determined to be present wherever is above the threshold value. Exceeding this value throughout the domain indicates that the volume of fluid has completely filled the cavity, and so the simulation is stopped by default. You can ignore this constraint by clicking the Disable ‘Stop When Full’ criterion menu item in the VOF iterative parameters menu, as described in step 8.(a)viii. in Problem Setup.