Are there any tips and tricks to aid convergence in periodic flow problems with specified mass flow rates in FLUENT?
If you are experiencing convergence difficulties while running a case with periodic boundaries and a specified mass flow rate, these are a few things you can try to improve the convergence behavior.
(1) Mesh Requirement: Mesh plays an important role in the case convergence. The mesh in the periodic faces should be exactly same. You should link the periodic edge or face mesh. The convergence will be better if the meshes near to the periodic faces are also exactly same. If you use the sizing function, make sure that the mesh is same in the nearby region also, otherwise use uniform mesh.
(2) URF: Start the simulation with smaller URF values. Pr- 0.2, dens- 0.5, body force- 0.5, mom- 0.3, all turbulent URF- 0.4. You can increase the URF gradually with convergence.
(3) Initial Pressure gradient: The following command sets the pressure gradient value to zero:
(rpsetvar 'periodic/pressure-derivative 0)
Include this command in Solve->Execute Commands and execute at every iteration. Enable this command for first 30-50 iterations. After 50 iterations, disable this and the calculated beta will be updated. This sometimes helps convergence.