When you create a new part, you must specify the modeling space in which the part will reside. You can assign the following three types of modeling space:
Three-dimensional
Abaqus/CAE embeds the part in the X, Y, Z coordinate system. A three-dimensional part can contain any combination of solid, shell, wire, cut, round, and chamfer features. You model a three-dimensional part using three-dimensional solid, shell, beam, truss, or membrane elements.
Two-dimensional planar
Abaqus/CAE embeds the part in the X–Y plane. A two-dimensional planar part can contain a combination of only planar shell and wire features, and all cut features are defined as planar through cuts. You model a two-dimensional planar part using two-dimensional solid continuum elements, as well as truss or beam elements.
Axisymmetric
Abaqus/CAE embeds the part in the X–Y plane with the Y-axis indicating the axis of revolution. An axisymmetric part can contain a combination of only planar shell and wire features, and all cut features are defined as planar through cuts. You model an axisymmetric part using axisymmetric solid continuum elements or axisymmetric shell elements.
Abaqus/CAE uses the following methods to determine the modeling space of an imported part:
When you import a part from a file containing geometry stored in a third-party format, you can specify the part's modeling space, provided that Abaqus/CAE does not determine it must be three-dimensional.
When you import a mesh from an output database, Abaqus/CAE determines the modeling space of the new part from the information stored in the output database.
When you import a mesh from an input file, Abaqus/CAE determines the modeling space of the new part from the element type.
When you create a mesh part in the Mesh module, the modeling space of the mesh part is the same as the modeling space of the original part.
