I wish to perform a simulation and create a mesh of an eccentric rotor.

    • arv2995

      I am performing a simulation of a rotor and stator arrangement of a centrifugal compressor. I have created the meshes in Turbogrid where the centre of line of axis lie on (0,0,0). Now I want to do a simulation wherein the rotor has a certain eccentricity say e.

      How do I create a mesh in Turbogrid or make changes in Design modeler so that I keep the volume of mesh same, but just that the eccentricity is represented in this mesh.

    • rfblumen
      Ansys Employee
      If the eccentricity is small (10-20% of the tip clearance), one approach is the following:
      -Generate the mesh in TurboGrid about the global rotation axis (assume z-axis), as usual.
      -In CFX-Pre, replicate the blade passage to a full wheel under Geometry Transform. Then, translate the geometry in the y-direction by an amount that reflects the desired eccentricity (call it dy).
      -Create a new coordinate system (Coord 1) based on the y offset value of dy.
      -Under the domain settings, use Coord 1.3 for the rotational axis. Set Mesh Deformation from None to Regions of Motion Specified. Set mesh motion of the inlet, outlet and blade tip interfaces to "Unspecified". Set the mesh motion of the shroud to Specified Displacement. set the displacement to (0,-dy,0). Set the shroud as a rotating wall with rotation opposite to the impeller angular velocity and rotating about the global z axis.

      For larger eccentricity values, the above workflow may lead to negative volumes due to excessive mesh deformation. In that case, an alternate approach would be the following:
      -In BladeEditor, under the FlowPath feature, create an intermediate layer in the tip gap just off the blade tip. Create a new FlowPath using the intermediate layer as the new "shroud" and export the geometry to TurboGrid using the new FlowPath. Also in BladeEditor, create an annular solid extending from the hub to the shroud using the revolve feature. Create a 3D surface from the intermediate layer, then offset this 3D surface in the y-direction by dy. Use the 3D surface to cut the annular solid. The solid at the higher radius represents the tip clearance from the intermediate layer to the shroud and has a non-uniform thickness in the circumferential direction.
      -In Ansys meshing, create a mesh for the annular solid
      -In CFX-Pre, replicate the blade passage to a full wheel under Geometry Transform. Then, translate the geometry in the y-direction by an amount that reflects the desired eccentricity (dy). Read in the annular body mesh. Put all bodies into the rotating domain. Connect the rotor domain "shroud" with the inner surface of the annular domain using a GGI interface. As before, specify the rotor to rotate about the local offset z-axis. Have the shroud counterrotate about the global z-axis. Not that with this approach, no mesh deformation is used.
    • arv2995
      Thank you very much for your reply-
      My eccentricity values are very less hence the method 1 is the one that I am currently using.
      After following your instructions I have some errors in the Error window,that say.
      The parameter "Wall Velocity Relative To" should exist in the object "/FLOW:Flow Analysis 1/DOMAIN:B_ABC/BOUNDARY:WallABC/BOUNDARY CONDITIONS/MASS AND MOMENTUM" but is not present.
      There must be an object of type "MESH MOTION" in the object "/FLOW:Flow Analysis 1/DOMAIN:ABC/BOUNDARY:InterfacePQR/BOUNDARY CONDITIONS" but it does not exist.
      I have the same error for the Blades of the rotor,main as well as splitter blades. Also for the various other interfaces that I have defined in my model I am getting the same error. Also for the Hub it is giving me the same error. What mesh definition(Mesh motion setting) should I give for these blades and interfaces to resolve these errors?
      Could you please explain what you meant by Coord 1.3?
      Kindly help me with this problem.

Viewing 2 reply threads
  • You must be logged in to reply to this topic.