Shell section behavior is defined in terms of the response of the shell section to stretching, bending, shear, and torsion. For more information, see “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide.
General shell stiffness sections allow you to specify shell section properties directly in terms of a stiffness matrix and thermal expansion response. These data completely define the shell section's mechanical response, so no material reference is needed as part of the section definition. General shell stiffness sections provide an efficient and flexible method for defining shell responses when you know the terms of the applicable stiffness and thermal stress matrices. For more information, see “Specifying the equivalent section properties directly for conventional shells” in “Using a general shell section to define the section behavior,” Section 29.6.6 of the Abaqus Analysis User's Guide.
General shell stiffness sections cannot be used with variable thickness shells or continuum shells. Like other pre-integrated shell sections, general shell stiffness sections are not integrated through their thickness and do not provide for heat transfer. In an Abaqus/Standard analysis, stresses and strains are not available for output from general shell stiffness sections.
The following sections describe how to create a general shell stiffness section:
“Specifying dependencies for general shell stiffness sections”
“Specifying advanced properties for general shell stiffness sections”
To create a general shell stiffness section:
From the main menu bar, select Section
Create.
A Create Section dialog box appears.
Tip:
You can also click Create in the Section Manager or select the create section tool 
in the Property module toolbox.
Enter a section name. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select Shell as the section Category and General shell stiffness as the section Type, and click Continue.
The general shell stiffness section editor appears.
On the Stiffness tabbed page, enter the symmetric half of the shell stiffness matrix in the data table. The first row contains matrix entries 
through 
, the second row contains matrix entries 
through 
, and so on; the last row contains matrix entry 
. See “Entering tabular data,” Section 3.2.7, for more information.
The Dependencies tabbed page allows you to define thermal stresses on the shell section. You can also apply temperature-dependent and field variable–dependent scaling factors to the shell stiffness matrix and thermal stresses. For detailed information on the equations used to define shell stiffness dependencies, refer to “Specifying the equivalent section properties directly for conventional shells” in “Using a general shell section to define the section behavior,” Section 29.6.6 of the Abaqus Analysis User's Guide.
To specify dependencies for general shell stiffness sections:
On the Dependencies tabbed page:
If you are defining a thermal expansion coefficient that is a function of temperature, toggle on Specify reference temperature and enter the reference temperature, 
, in the field provided.
To define thermal stresses on the shell section, toggle on Apply thermal stress and enter the stress components in the table provided: 
(Sigma11), 
(Sigma22), 
(Gamma12), 
(K11), 
(K22), and 
(K12).
To define scaling factors that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temp appears in the Scaling factors data table.
To define scaling factors that depend on field variables, click the arrows to the right of the Number of field variables to increase or decrease the number of field variables.
Field variable columns appear in the Scaling factors data table.
In the Scaling factors data table, enter the Scaling modulus (Y) for the stiffness matrix and the Thermal Expansion Coefficient (
) for the thermal stresses.
To specify advanced properties for general shell stiffness sections:
On the Advanced tabbed page:
Specify the Section Poisson's ratio to define the shell thickness behavior. Specifying the section Poisson's ratio causes the shell thickness to change as a function of membrane strains.
Toggle on Use analysis default to use the default value of 0.5, which will enforce incompressible behavior of the element for membrane strains.
Toggle on Specify value, and enter a value for the Poisson's ratio. This value must be between –1.0 and 0.5. A value of 0.0 will enforce constant shell thickness, and a negative value will result in an increase in the shell thickness in response to tensile membrane strains.
Toggle on Density, and enter a value for the mass per unit surface area of the shell. The mass of the shell is determined from this density.
For most shell sections Abaqus will calculate the transverse shear stiffness values required in the element formulation. If desired, toggle on Specify values from the Transverse Shear Stiffnesses options to include nondefault transverse shear stiffness effects in the section definition, and enter values for 
, the shear stiffness of the section in the first direction; 
, the coupling term in the shear stiffness of the section; and 
, the shear stiffness of the section in the second direction. If either value or is omitted or given as zero, the nonzero value will be used for both.
Click OK to save your changes and to close the general shell stiffness section editor.