Initial shell curvature

Abaqus automatically calculates the surface normals at the nodes of every shell element to estimate the initial curvature of the shell. The surface normal at each node is determined using the algorithm discussed in Defining the Initial Geometry of Conventional Shell Elements.

With a coarse mesh as shown in Figure 1, Abaqus may determine several independent surface normals at the same node for adjoining elements. Physically, multiple normals at a single node mean that there is a fold line between the elements sharing the node. While it is possible that you intend to model such a structure, it is more likely that you intend to model a smoothly curved shell; Abaqus will try to smooth the shell by creating an averaged normal at a node.

Figure 1. Effect of mesh refinement on the nodal surface normals.

The basic smoothing algorithm used is as follows: if the normals at a node for each shell element attached to the node are within 20° of each other, the normals will be averaged. The averaged normal will be used at that node for all elements attached to the node. If Abaqus cannot smooth the shell, a warning message is issued in the data (.dat) file.

There are two methods that can be used to override the default algorithm. To introduce fold lines into a curved shell, either give the components of n as the 4th, 5th, and 6th data values following the nodal coordinates (this method requires manually editing the input file created by Abaqus/CAE in a text editor); or specify the normal direction directly with the NORMAL option (this option can be added using the Abaqus/CAE Keywords Editor; see Cross-section orientation). If both methods are used, the latter takes precedence. See Defining the Initial Geometry of Conventional Shell Elements for further details.