You have started a simulation of physical processes in Flow Vision by yourself, but the calculation always breaks down. Or the calculation runs, but the results do not correspond to physics. Is it familiar to you? Here is the quintessence of the experience from technical support and the training department staff. It`s a guide on what to do if your calculation breaks down.
how to understand that calculation breaks down?
You can monitor the calculation status by:
- Monitoring window. Here check up the time step, number of calculated cells, iterations of equations.
- Fields of main parametrs (velocity, pressure, temperature and others). They are layers in PostProcessor on a plane or in volume.
- Integral values of the parameters. They are calculated as characteristics on the plane or supergroup.
You shouldn't ignore such signs:
- Too large or too small explicit time step.
Time step smaller than 10-6 is considered as very small. The tasks with high speeds and fine mesh are exceptions. The FlowVision solver stops calculation by default, when an explicit time step of calculation reaches 10-10 value.
- Abnormally large or low values of temperature, pressure, Mach number or another parameters in computation domain.
For example, a temperature of 0 K never encounteres in calculations for general industrial tasks. Also the Mach number rarely exceeds the value of 10. You can control values and find a point of an anomalous value in computational space using the characteristics of the variable in the entire volume.
- The equations (pressure, velocity, enthalpy) run through zero or several hundred iterations.
- Algebraic residuals are close to 1. The first time steps of the calculation are exceptions.
- The number of calculation cells is 0.
what to do if this has happened?
- Check up the geometry. Specifically
- dimensions of the geometric model. Maybe you have saved it in mm or inches while exporting. Remember, that FlowVision works with geometric dimensions only in meters.
- check up the geometric model for self-intersections. You can't run the calculation with self-intersections, even if the task is correct. Anyway, after some time the decision will fall apart.
- precision of CAD geometry model . The coarse grid of the CAD geometric model surface affects the solution precision.
- Check up the physical statement of the task.
Estimate the result that may be reached on the base of your initial data. The most unsolvable calculations are those that come up with from nowhere without sense of physics.
- Check up reference values of pressure and temperature.
Keep in mind that all other pressures and temperatures (for boundary and initial conditions, modifiers, layers and characteristics) are set relative to reference values. The only exceptions are the properties of substances and limiters. Here all values are set in absolute values.
- Check up if all the necessary properties of the substances are set.
Even if a substance takes from the standard FlowVision database, it does not mean that all substance`s parameters are set in range which is needed for your task.
- Check up all physical processes in the phase.
It is not correct to simulate flow with speeds highly than 0.5M without taking temperature in account. Unreasonable ignoring of this equations leads to non physical results.
- Check up the initial data.
The closer the initial data is to the required one, the sooner the solution will converge. As a result, the solver will have the less maneuvers to break down. The lack of initial data is fatal for the task in some cases. For example, it happens that the task of supersonic flow falls apart near streamlined bodies (most often in shadow zones) due to high initial velocities in the border cells. To avoid this, set the braking parameters near the surface as the initial data.
- Check up the settings of boundary conditions.
Sometimes engineer sets only the type of BC, but forgets to change the BC parameters. Or the BC is set correct but it is not attached to the geometric model. Also you should consider that there are restrictions on the application of some types of BCs for different types of flows. Read more about this features of the application of each BC in the documentation: Theory > Boundary conditions for each physical process.
- Check up the initial conditions.
Have you set the IC for the correct objects in each subregion? The sequence of initial conditions in project`s tree is also important. Note: the initial conditions are inserted according to the list in the project tree from top to bottom and overwrite each other.
Check up the mesh.
Maybe you have been creating it for a long time in the Initial grid editor and have forgotten to click the "Apply" button. Or the computational domain has very coarse mesh. So the place of disturbances is poorly resolved by the grid. If you forget to change the criterion for small cells from absolute to relative, the computational mesh will consist of 0 cells.
- One of the most common causes of computation`s collapse is a time step.
If your calculation have collapsed, set the time step CFL = 1. Also it is important to limit the maximum time step. Because of absence of initial conditions during the first computation step, the time step will be equal to 1 s by default. Some irreversible changes may happen in calculation during this time step. You may set very small maximum time step, for example, about 10-8 for supersonic flows with shock waves. And then, after a few iterations, raise it.
- The absence of calculation limiters make influence on calculation parameters for supersonic flows.
Limiters eliminate high values of parameters caused by the features of numerical methods. If the value of parameter exceeds a limit value then it is decreased artificially.
- Check up if there are small bad cells in the subregion.
To do this, create a layer "number of cells" in PostProcessor. If there are such cells, it means that you need to change the criterion for the small cells or change the mesh.
if nothing helps you