ODS Engineering

Initialising the domain

In a CFD model the initialisation of the calculation domain with some initial guess is an important step, particularly for larger and time-dependent simulations. If you think about it in physical terms this is quite understandable: if you have a large domain that has been initialised with an internal field of zero velocity then there will be a sudden "shock" within the calculation when air starts moving at the inlet. If the domain is small then the computer generally pushes through this small amount of air and the calculation progresses normally. However if the domain is very large then the forces required to move the tonnes of air will be too great and the calculation will generally fail. The user generally observes this as the calculation progressing for several timesteps and then suddenly stopping with error messages that include very large numbers like so:

Courant Number mean: 1166.08 max: 1.84785e+10
bounding epsilon, min: -5.72945e+14 max: 5.7353e+14 average: 1.30043e+09
DILUPBiCG:  Solving for k ...  Final residual = 6.45149e+10
bounding k, min: -4.34385e+26 max: 5.70886e+26 average: -5.18486e+20

This is typical of a simulation which has "diverged" as the computer has not been able to lock in to a sensible solution.

The solution to this is to be careful to ensure that you initialise your domain with a "sensible" solution to help the solver as much as possible. The following are suggestions to help achieve a well initialised domain:

If you are running a transient simulation (with pisoFoam for example) try running a steady-state solution first (with simpleFoam). When the steady-state solution is finished navigate to your CFD case directory and rename the "0" directory to "0.org". Then change the solver type back to pisoFoam and re-write the case files. Finally rename the final timestep directory to "0". Delete any processor directories and then re-run the case. This will use the results from the final iteration of the steady-state simulation as initial conditions for the transient solution
For initialising both transient and steady-state solutions try doing the same as above except with using the potentialFoam solver to intialise the domain.