**** Entered By: akpaul @ 07/18/2005 03:45 PM ****
Q. How can you preload a structural model prior to doing an FSI analysis with CFX?
Here's the situation: Client wants to twist a structural model which will create stored energy independent of CFX. He then wants to release the structural model and have it swing back to its original state while being damped by a fluid modeled with CFX in a transient analysis. He needs to have the CFX mesh morphed to the shape of the deformed structural model prior to the first step so it is ready to start damping the transient response. Is this possible? He does not want to have to run a long transient initially just to set up the structural preload in his model.
A.
The best way to setup a FSI case with pre-loading using the MFX solver, is to run two simulations as given below:
1)Pre-Load Step: A regular FSI simulation is executed, but no forces are received from CFX. Instead, a force boundary condition is applied in ANSYS. The solid model mesh moves, and deformations are transferred to CFX. Hence you will only define one FSI interface in the Ansys input file - one that sends 'Displacements' to the corresponding boundary condition in CFX.
Note that the CFD domain feels this motion and establishes a flow field. However, You can set an expert parameter in the CFX def file, 'SolveFluid = f' (Solve Turbulence = f' etc..) to stop the solver from computing a solution for the momentum and turbulence equations. In which case, CFX will only solve for the mesh deformation, which will reduce the time and computational effort required. This simulation is run until the desired preload is realized.
2) Fully Coupled FSI/Damping run. - This essentially is a FSI restart. Make sure all the run files from pre-load step are available in the working directory. In the input file add the second FSI interface - the one that transfers forces from CFX to Ansys. Also remove the pre-loading pressure. For CFX the 'Initial Values File' w
|
**** Entered By: akpaul @ 07/18/2005 03:45 PM **** Q. How can you preload a structural model prior to doing an FSI analysis with CFX? Here's the situation: Client wants to twist a structural model which will create stored energy independent of CFX. He then wants to release the structural model and have it swing back to its original state while being damped by a fluid modeled with CFX in a transient analysis. He needs to have the CFX mesh morphed to the shape of the deformed structural model prior to the first step so it is ready to start damping the transient response. Is this possible? He does not want to have to run a long transient initially just to set up the structural preload in his model. A. The best way to setup a FSI case with pre-loading using the MFX solver, is to run two simulations as given below: 1)Pre-Load Step: A regular FSI simulation is executed, but no forces are received from CFX. Instead, a force boundary condition is applied in ANSYS. The solid model mesh moves, and deformations are transferred to CFX. Hence you will only define one FSI interface in the Ansys input file - one that sends 'Displacements' to the corresponding boundary condition in CFX. Note that the CFD domain feels this motion and establishes a flow field. However, You can set an expert parameter in the CFX def file, 'SolveFluid = f' (Solve Turbulence = f' etc..) to stop the solver from computing a solution for the momentum and turbulence equations. In which case, CFX will only solve for the mesh deformation, which will reduce the time and computational effort required. This simulation is run until the desired preload is realized. 2) Fully Coupled FSI/Damping run. - This essentially is a FSI restart. Make sure all the run files from pre-load step are available in the working directory. In the input file add the second FSI interface - the one that transfers forces from CFX to Ansys. Also remove the pre-loading pressure. For CFX the `Initial Values File` will be the *.res file from the earlier run. Note: Edit the RES file (Tool>Edit Definition File from SOLVER MANAGER) to set the Solve Fluids expert param (and others) to 't'. This will result in the flow equations being solved. POSSIBLE ISSUES : Will have to work within the limits of the CFX mesh morphing routines to deform the fluid mesh - which currently has no re-meshing/re-zoning capability. |
||
|