Understanding midsurface modeling

Context:

The midsurface modeling process relies on an accurate solid model as the starting point. Midsurface modeling is best suited to thin solids or thin-walled solids where wall thickness is constant or where reasonable approximations of the wall thickness at each point can be made easily. You can apply midsurface modeling to any solid cell within a model; you need not apply it to the entire model. If you apply midsurface modeling to only a portion of a solid model, Abaqus/CAE automatically creates shell-to-solid coupling constraints to couple the motion of the midsurface shell edges to that of the remaining solid model faces. Shell-to-solid coupling constraints will not be created if the angle between the shell surface and the solid face deviates significantly from 90°.

Besides reduced expense, you might use a midsurface model in place of a solid model to better account for bending response in thin sections of the model. Shell elements are designed to manage bending loads within the thickness of a single element, whereas a single solid element will have little or no resistance to bending.

Creating a midsurface model in Abaqus/CAE is a manual process. The procedure presented below provides an overview of the general steps involved. The tasks within each step may vary depending on the complexity and completeness of the original solid model and the analysis requirements. Some steps, such as Step 4 below, may not be required or may be completed in a different order from what is presented here.

Assign midsurface regions on the solid part. Use the Assign Midsurface Region tool to select one or more cells from the solid part to begin creating a midsurface model. For more information, see Assigning a midsurface region.
Abaqus/CAE removes the selected cells from the active representation and creates a reference representation containing the selected cells.
Create new shell faces to replace the solid geometry that you moved to the reference representation.
You can use tools in the Geometry Edit toolset or the shell feature creation tools to add shell features to the midsurface model. For more information, see The Geometry Edit toolset and Adding a shell feature, respectively. The offset faces tool in the Geometry Edit toolset is the most common face creation method for midsurface models. The offset process creates new faces based on selected geometry and automatically assigns a shell thickness based on the offset parameters.
Assign thicknesses to the new shell features.
The Assign Thickness and Offset tool allows you to assign shell thicknesses to the new midsurface geometry (for more information, see Assigning thicknesses and offsets). The tool allows you to assign thicknesses to individual faces, and you can also use it to edit thicknesses that Abaqus/CAE assigned automatically for faces created using the offset process. You must still assign a section to the new faces in the Property module. During the section assignment process you can make a final decision whether to use the thickness defined with the section properties or to use the definition from the geometry. You can toggle the shell thickness display in all part and assembly-based modules to see the thickness in the viewport (for more information, see Visualizing shell thicknesses).
Revise any analysis attributes that were associated with the solid geometry that was used to create the reference representation.
Analysis attributes such as loads, boundary conditions, or interactions cannot be applied to geometry in the reference representation. Any attributes that were associated with the solid geometry before it was moved to the reference representation will be associated with an empty region if the geometry is no longer part of the active representation. For more information, see Understanding the reference representation.