Free Courses Fluids Structures Electronics 3D Design Optics Photonics Materials Installation Python Optimization Safety & Cybersecurity Embedded Software MBSE Digital Mission Engineering STEM NVH Student Teams Indo Kursus Partner Courses My Courses

[FAQ]

When loading a mesh from Ansys Meshing into Fluent it can occur that the following warning message is printed many times: Warning: materials in neighbor cell threads (6 and 7) of interior zone 1 are of different types (aluminum and air). This problem MUST be fixed before solving The reason for this can be a conflicting definition of material type (fluid, solid) in Ansys Meshing For example the issue will become visible with the following settings: 1. no material assignment in geometry 2. body name includes the text “fluid” 3. Named Selection (NS) is defined on the same body, but without the text “fluid” 4. Default setting of “Auto Zone Type Assignment = On” is set in Ansys Meshing (AM) In this scenario the material type is undefined by the geometry. So it gets automatically defined in AM. As the body name includes “fluid” the body will be defined as fluid type. However, as the NS does not include “fluid” the material type gets overridden as solid. Due to this overriding no “Interior Wall” is defined between the fluid and neighbor solid bodies. This results in the warnings in Fluent. The solution is one of the following: 1. define the material type in geometry and deactivate “Auto Zone Type Assignment” 2. define the material type in AM on the body and deactivate “Auto Zone Type Assignment” 3. use “fluid” in the body name and do not define Named Selections on the body (i.e. only on faces of the body but not on the volume) 4. do not change the default body names and use “fluid” in the Named Selection on the body Or check the following: If the “Auto Zone Type Assignment” is active (default) and a body is defined as fluid (by type or name) than a specified NS on the body must also have the text “fluid” in its name. The “Auto Zone Type Assignment” can be set in the options of Ansys Meshing in File > Options > Meshing > Export > Ansys Fluent > Auto Zone Type Assignment