Gå till innehåll

Forsiden / Blogg / Blogg / ANSYS Tutorial: CFX Re-Meshing  

+47 67 57 21 00

+46 21 470 35 50

Kontaktformulär

ANSYS Tutorial: CFX Re-Meshing

ANSYS CFX Tutorial: In ANSYS CFX 12.1 it is possible to apply automatic re-meshing using ANSYS ICEM CFD for cases with large mesh deformation. This article explains the key steps to make it work.

Introduction

In many CFD cases where for example fluid structure interaction (FSI) is used, large deformation is very common. Generally, CFD solvers allow for a mesh deformation to adapt to this deformation. However, if the deformation is too large it might be hard to deform the current mesh without destroying the mesh or at least distort the elements too much.

The method to overcome this problem is to apply a re-mesh step when the current mesh quality becomes too low. This can be done in ANSYS CFX 12.1 using the meshing capabilities in ANSYS ICEM CFD.

Creating input mesh

This part needs to be done in ANSYS ICEM CFD as we will use it for the re-meshing process. In this example, I will let a rectangular box move downwards in a square channel.


Figure 1 shows the geometry that is originally created in ANSYS DesignModeler. First we need to create parts for the boundaries we want to use in our CFD simulation. The box in the centre is target for a downward motion. It is given the name BOX. As in any mesh session in ICEM CFD, you must apply your required sizing necessary for the simulation.

Figure 1

Thereafter, bring up the Replay Manager in ICEM CFD and perform the desired meshing steps. Save these commands to a replay (.rpl) file for later use in ANSYS CFX. Also, export the created mesh to ANSYS CFX format and save the project and remember the location of the ICEM CFD files (.tin and .rpl).

Set up the ANSYS CFX case.

General setup.

In this simple case, the BOX will move downwards with time.

  • Define the fluid flow in the domain with the desired physics and allow for mesh deformation.
  • Set the mesh stiffness to increase in small volumes. This will preserve the small prismas close to the solid walls as much as possible and the main deformation will be absorbed further away from the body.

Boundary details

  • At the top and bottom surfaces, opening conditions is applied so that fluid can enter or leave the domain as needed.

The fundamental part in this case is to allow for mesh deformation and monitor the quality of the mesh. As the quality becomes too low a re-mesh call is made. The motion of the walls is here described with an expression.

  • Create an expression that describe the motion of the solid. In this case a linear motion is used which increases with time. The expression is named to "motion". The reason for using Time This Run is that I will otherwise get large jumps when the solver restarts after a re-mesh. Alternatively, the variable mesh reinitialisation time can be used.
  • Create the remaining boundaries except the moving wall as usual and set the mesh motion to unspecified. This will allow for the nodes on the surface to move if needed.

The wall boundary on the BOX is somewhat different compared to the other boundaries. Here, the motion expression should be set as the z-axis displacement. Since the box should move downwards a minus sign is added.

Interupt control setup.

The next step is to set up a stop control that will monitor the mesh quality and stop the solver.

  • The first step is to create a logical expression that monitors the orthogonality in the mesh. The expression is given the name remeshingcond. This expression will be 1 if the orthogonality becomes lower than 5 degrees and 0 if not.
  • Add the expression as in interrupt control under the solver control tab.
  • Specify a configuration to allow for special events in the simulation. For example a configuration can allow for a sequence of simulations or a re-mesh.

Re-mesh control setup.

Before the re-meshing is defined two output monitors needs to be defined. The reason for this is that the re-meshing feature uses output monitors as input to ANSYS ICEM CFD.

  • The first output control is a Geometry Scale factor. This will scale the ANSYS CFX output to match the model in ICEM CFD. Here, the geometry scale is set to 1mm as the ICEM model is done in mm. If the model is created in the same dimensions this is not needed.
  • The second output monitor is WALL Displacement z. This output monitor tracks the average of the total centroid displacement of the moving boundary. This variable is added in version 12 and tracks the centroid of a surface from the start of the simulation. Thus, the monitor will give us the total motion of the body from the first time step of the simulation.

With these two output controls defined we can now specify our re-meshing.

  • Create a new re-mesh with the option ICEM CFD Replay.
  • The re-mesh should be activated by our previously created interrupt condition.
  • The domain that should be meshed is here BODY. Body corresponds to the volume in ICEM CFD.
  • The geometry file should be the .tin file created during the meshing.
  • The replay is the file that stores the meshing steps done during meshing.

The next step is to create an ICEM CFD Part Map. This couples the boundary in ANSYS CFX to corresponding boundary in ICEM CFD. In this case, we only need to create one part map since we only have one moving boundary.

Finally, two scalar parameters needs to be created. The name of these scalar parameters are sensitive as they are identified by the re-meshing scripts included in the ANSYS CFX installation.

  • The first one is named DISPLACEMENT Z BOX and should use the WALL Displacement z monitor previously defined.
  • The second scalar parameter should be named ICEM CFD Geometry Scale and should be set to the corresponding monitor point.

This is what should be needed to perform this type of analysis. The animation at the top show the motion of the box through the domain. Basically, the script that run the motion of any part in ICEM CFD can be modified to allow for any deformation. If YOU want to do this and need advice or help. Give us a call!

Do you want to learn more?

EDR provides a training course that covers basic ANSYS CFX operations, as well as other interesting topics.

Or contact our ANSYS Support to ask for hints!