While many dynamic mesh problems are transient, you can use dynamic meshes for steady-state applications as well. Some examples of steady-state applications include: checking the valve application after reaching a steady-state valve position; or after a fluid-structure interface application has reached a steady-state solution.
There are no differences in the meshing aspect between steady-state cases and transient cases. Furthermore, setting up a steady-state simulation is similar to setting up a transient case, described in Using Dynamic Meshes. However, there are a few differences that you should note:
A CG_MOTION UDF is needed
to specify the motion of the boundary: a transient profile used in
transient cases cannot be used in steady-state cases.
The dtime passed to the CG_MOTION UDF is 1 by default: if a displacement of
1 mm is needed to move the boundary, you can specify the velocity
to be 1e-3 m/s.
Dynamic mesh parameters can be different since an interpolation error is no longer a concern.
If you have enabled local remeshing for your steady-state application, you can instruct ANSYS Fluent to perform additional remeshing after the boundary has moved. This additional remeshing is based on skewness criteria, and can further increase the quality of your mesh. See Dynamic Mesh Update Methods for further details.
The mesh must be manually updated through journal files or execute commands. To update the mesh, you can use the Mesh Motion Dialog Box.
Solution →
Run Calculation → Update Dynamic Mesh...
Alternatively, you can use the following text command:
solve → mesh-motion
which can also be used as an execute command in the Execute Commands Dialog Box:
Note: When you are solving a problem using the six DOF solver, you may need to modify the pseudo time step size in order for the solver to converge. It is also recommended that you ensure that the steady-state solution is reasonably well converged before performing the steady-state dynamic mesh update.
Solution → Calculation Activities → Execute Commands
New...
You can display dynamic mesh statistics (such as minimum and maximum volumes and maximum cell and face skewness) by clicking the button in the Mesh Motion Dialog Box (Figure 10.94: The Mesh Motion Dialog Box for Steady-State Dynamic Meshes).
Important: The following options are not available for steady-state applications:
In-Cylinder
Implicit Update
Also, the Dynamic Mesh Events dialog box is not available for steady-state applications.
Consider a rescue drop case shown in Figure 10.95: Initial Object Position. The object can be moved in any position in the steady-state solver, after which steady-state analyses can be performed at different object positions.
The dynamic mesh parameters setup is identical for the steady-state
and transient cases, which is described in Setting Dynamic Mesh Modeling Parameters. When setting up the dynamic
zones, the procedures are similar to those described in Specifying the Motion of Dynamic Zones, except that the UDF selected
from the Motion UDF/Profile drop-down list is
different. In steady-state cases the dtime passed to the UDF is by default 1. So, in this example, the object
will move 50 mm each time the following UDF is executed:
#include "udf.h"
DEFINE_CG_MOTION(pod,dt,vel,omega,time,dtime)
{
NV_S(vel,=,0);
NV_S(omega,=,0);
vel[1] = -50e-3;
}
The resulting mesh is shown in Figure 10.97: Final Object Position After 40 Executions.