When you generate a mesh using Ansys ICEM CFD or export a mesh from Ansys Meshing in the Polyflow
format, the mesh information is written to a .poly file. You
can read such a .poly file directly into Ansys Polydata or Ansys Polyman,
as described in Reading Files Directly and
Importing a Mesh File, respectively.
Ansys Meshing is a mesh generator, whereas Ansys ICEM CFD can generate both a geometry and a mesh. Both applications allow the generation of surface (boundary set) and volume (subdomain) topologies. Moreover, for 2D geometries you can define 1D internal and external PMeshes, while for 3D geometries you can define 2D external PMeshes and 1D and 2D internal PMeshes. Note that the PMeshes cannot be defined on the border. See PMeshes for details about PMeshes.
You do not need to generate midsegment or midface nodes in the mesh generator in order to use these interpolation schemes in Ansys Polyflow. Midside nodes will be added by Ansys Polyflow automatically, as needed.
In general, you must carefully check the mesh in order to avoid thin regions in which only one element exists between opposite walls. If such situation occurs, all velocity nodes of such elements have fixed (and generally) null values (that is, a fixed wall condition): no fluid will cross these elements, leading to artificial obstacles in the flow.
Note the following with regard to meshes generated by the CutCell method in Ansys Meshing:
You must not combine (for example, using Ansys Polyfuse) a mesh that was generated by the CutCell method with another type of mesh, if you intend to use it in an Ansys Polyflow simulation; Ansys Polyflow requires that the mesh you read in consists of a domain in which either every part or no part is a CutCell mesh. Consequently, you cannot use an unaltered CutCell mesh with moving boundaries (for example, in a free jet region outside of an extrusion die), as the remeshing algorithms require a sliceable mesh, which is typically a swept mesh. To overcome this limitation, you can use Polydata to convert a portion of your CutCell mesh into a sliceable mesh, as described in Generating a Sliceable Free Jet Mesh.
CutCell meshes should not be used when PMeshes are also created, as the compatibility is not guaranteed.
For CutCell meshes, the interpolation for the velocity field is limited: for a pure CutCell mesh, it must be the linear element; for a portion of a CutCell mesh that has been converted into a sliceable mesh, it can be either the linear element or the mini-element.
Note that the non-conformal elements created by the CutCell method do not support the mini-element interpolation. When this interpolation is chosen, it is applied only on the conformal elements created in the free jet defined in Polydata (see Generating a Sliceable Free Jet Mesh). A linear interpolation is used for all other elements.
The following tasks are not supported for CutCell meshes:
MIXING task
Volume Of Fluid problem(s)
The following sub-tasks are not supported for CutCell meshes:
Differential viscoelastic isothermal flow problem
Differential viscoelastic non-isothermal flow problem
Integral viscoelastic isothermal flow problem
Integral viscoelastic non-isothermal flow problem
Film model : Gen. Newtonian isothermal
Film model : Gen. Newtonian non-isothermal
Film model : Viscoelastic isothermal
Film model : Viscoelastic non-isothermal
Shell model : Gen. Newtonian isothermal
Shell model : Gen. Newtonian non-isothermal
Shell model : Viscoelastic isothermal
Shell model : Viscoelastic non-isothermal
Isothermal crystallisation
Non-isothermal crystallisation
Residual stresses and deformations (Narayanaswamy)
Internal radiation
The adaptive meshing technique is not supported for CutCell meshes.
When reading a CutCell mesh and data file that was created prior to version 16.0, you will receive a warning message if Ansys Polydata detects an incompatibility with the ordering of the subdomains and boundaries, along with instructions on how to remedy the problem. In such cases, the easiest remedy (which will not require modifications to the simulation setup) is to rename the Named Selections in Ansys Meshing, so that when Polydata reorders the new names alphabetically, they will now correspond to the original order in the data file.