# Incorporating Transverse Normal Strain in the Homogenization of Corrugated Cardboards
## 2 Plate Element Incorporating Transverse Normal Strain
### Implementation in Abaqus  
Abaqus provides a user subroutine interface for advanced customization. Within Abaqus Standard, users can implement custom elements via the subroutine UEL. During analysis, Abaqus invokes UEL for each user element to retrieve elemental matrices (e.g., stiffness and mass matrices). The subroutine is written in Fortran (_for_ file extension), with function header and variable definitions detailed in the Abaqus documentation [16]. * Environment  
Compilation environment configuration is a prerequisite for UEL implementation, which can vary across Abaqus versions. This study employs Abaqus 2022, Visual Studio 2019, and Intel Visual Fortran 2020. By default, UEL subroutines compile with the Fortran 77 fixed format; free-format Fortran (adopted in this work) requires configuration file modifications (see Appendix B). * Programming guidelines  
Comprehensive UEL guidelines can be found in references [25; 26; 27]. Some critical variables warrant emphasis here:  
**AMATRX**: Represents the stiffness matrix (**K**) in static analyses. **U**: Solution vector of nodal displacement, corresponding to \(\mathbf{q}\) in Equation (5). **RHS**: The residual vector. For linear elastic analysis, **RHS** = \(-\)**AMATRX-U**. Programming templates and reusable subroutines are provided in reference [30]; several of them are utilized in this work. * Data flow  
The data flow is illustrated in Figure 3. For each user-defined element, the UEL subroutine is invoked by the solver to provide the element stiffness matrix and residual vector. Two keywords are necessary in the _.inp_ file:  
* User Element: defines the element in DOFs and nodal configuration. * Uel Property: passes parameters to UEL via the PROPS array. Figure 3: Data flow between main program and subroutine. Figure 2: Eight-node planar element. In the present work, six REAL-type numbers are passed in to specify the material's principal and normal vectors. Additional material properties and geometry parameters are read by UEL from a custom _.txt_ file in the working directory. * Activation of DOFs The nodal DOFs in Abaqus follow a convention that DOFs 1-6 represent three translational and three rotational components [16]. For the plate element developed in this paper, it is necessary to activate DOFs 1-5. Since users cannot define additional DOFs in Abaqus, existing DOFs must be repurposed with their original meanings overridden--a methodology aligned with established practices [25; 26; 27]. Specifically, DOFs 11 and 12 (originally designated for temperature) are reassigned to represent \(\psi\) and \(\zeta\). To accommodate these repurposed DOFs, the coupled temperature-displacement analysis mode is selected for the load step. The field variable NT is added to the output. Output values NT11 and NT12 correspond DOFs 11 and 12, respectively. * Element visualization The user element cannot be visualized like the native elements. The solution is to superimpose a native element S8R with negligible stiffness on the user element, where two elements share the same nodes--these are called dummy elements. This is done by first modeling with S8R, then modifying the _.inp_ file (see Appendix C). Loads and boundary conditions are applied according to specific problem requirements. Since DOFs 11 and 12 are assigned to DOFs \(\psi\) and \(\zeta\), their corresponding loads are applied via the keyword \"Cflux. The user element does not support the \"Surface keyword, but after using the dummy element, distributed loads can be applied directly to it. Uniformly distributed loads can alternatively be converted to nodal loads according to reference [30]. More complex distributed loads can be applied using the subroutine DLOAD, and custom boundary conditions can be defined using the subroutine DISP. These subroutines can be put in the same _.for_ file without blanking lines between codes. The source code of the UEL subroutines developed in this paper is available (see Data Availability Statement).