Obtaining an Initial Flow Field

Run the simulation in a quasi-steady state to obtain an initial flow field. The solution from this initialization step is used as the initial condition for the co-simulation.

To solve for a steady-state flow about a rigid plate, freeze the co-simulation and mesh morpher solvers. The number of inner iterations per time-step are increased to allow a flow field to develop within a single time-step. Then, run the simulation for one time-step. As you are only searching for a steady-state solution, you do not need to be time-accurate. Therefore, use a large time-step of 1.5 s and a 1st-order temporal discretization setting.
  1. Select the Solvers > Implicit Unsteady node and set Time Step to 1.5 s.
  2. Multi-select the Solvers > Abaqus Co-Simulation and Solvers > Mesh Morpher nodes.
  3. Activate Solver Frozen.


  4. Select the Stopping Criteria > Maximum Inner Iterations node and set Maximum Inner Iterations to 400.
As the quasi-steady simulation only runs for one step, disable the maximum physical time and maximum steps stopping criteria:
  1. Multi-select the Stopping Criteria > Maximum Physical Time and Stopping Criteria > Maximum Steps nodes.
  2. Deactivate Enabled.
  3. From the menu, select Solution > Step.
  4. When the initial step is complete, refresh Scalar Scene 1.
  5. Save the simulation.
Reset the time to zero by clearing the solution history. Do not clear the solution fields, as this would cause you to lose the initial solution:
  1. From the menu, select Solution > Clear Solution.
  2. In the Clear Solution dialog, deactivate Fields and Reset Mesh, then click OK.