Yes, the dynamic mesh feature can be used in steady state applications to perform a parametric study of different object/boundary positions in the fluid flow. Typical applications include check valves, steady state FSI etc, often to calculate the object equilibrium positions. The primary advantage of using steady state dynamic mesh feature is that it will eliminate the repeated time-intensive mesh generation process for the series of intended runs. When creating the base mesh the user should have the same topological and meshing considerations as for a transient run. Set up is similar to a transient case set up. First define the dynamic mesh parameters, Define -> Dynamic Mesh -> Parameters (note that In-Cylinder and Six DOF Solver are incompatible with steady state solver). A DEFINE_CG_MOTION or DEFINE_GRID_MOTION user function is required to move the object (note that motion profiles are incompatible with steady state solver). The mesh will have to be manually updated using Solve -> Mesh Motion feature (or using the TUI command /Solve/mesh-motion). However, this process can be automated for a series of object positions using journal files and/or execute commands. It is important to remember that a default time step of 1 s will be used to update the mesh and so the user will have to set an appropriate velocity in user functions to achieve the desired object movement.