A reference representation is an alternative representation of a part or a subset (one or more cells) of a part that is not used in the analysis. The reference representation retains the original solid model geometry, and, like reference geometry in the Sketcher, you can use entities from the reference representation as tools to construct a simpler version of the part. The reference representation is most commonly used to construct a midsurface model. When used with the offset face tool to create faces for the midsurface model, the offset calculations between the reference representation and the new faces also allow Abaqus/CAE to automatically compute shell thicknesses and element offsets in the midsurface model.

Abaqus/CAE creates a reference representation when you assign a midsurface property to one or more cells in a solid part. The selected cells are removed from the active representation of the part and added to the reference representation. The reference representation appears by default in the Part module and is colored translucent brown. You cannot change the color of the reference representation, but you can toggle it on or off in all modules using the Show Reference Representation tool located with the visible object tools in the main toolbar. You can also toggle translucency of the reference representation on or off using the display options (for more information, see “Controlling edge visibility,” Section 76.3.

You can use the reference representation with the shape creation tools or with the tools in the Geometry Edit toolset to help construct new geometric entities in the active representation. For example, you can offset faces in the reference representation or you can select a planar face from the reference representation as the sketch plane to create a new shell face using the extrude method. You can use the geometry in the reference representation to define partitions—select an edge and a vertex from the reference representation as the point and normal to partition a cell—or create datum entities. You can also use reference representation geometry to position entities and define constraints in the Assembly module.

You cannot edit the geometry within the reference representation, and you cannot assign analysis attributes such as loads, boundary conditions, and interactions to it. When you create a reference representation, any analysis attributes that were applied to the solid cells before you created the reference representation will now be associated with an empty region. You can edit the empty regions to associate the analysis attributes with geometry—solid geometry or shell geometry that you create for the midsurface model—that is part of the active representation. Alternatively, you can suppress or delete the analysis attributes. If you do not make any changes to the affected analysis attributes, Abaqus/CAE will display a warning message when you submit the job in the Job module.