Abaqus UEL Elasticity

This repository contains the Fortran source code for small strain isotropic linear elastic user element (UEL) subroutine and example input files for Abaqus/Standard. Standard displacement-based finite element formulation has been adopted in this subroutine. The purpose of the project is to make users familiar with developing the UEL subroutine in Abaqus/Standard using a standard textbook formulation. This source code contains necessary subroutines related to element operations and matrix algebra.

Warning

Abaqus UEL subroutine feature is intended for advanced users and requires the understanding of finite element formulations and substantial programming. Users are recommended to consult textbooks on finite element analyses, Fortran programming, and Abaqus user documentation before developing their UEL subroutines.

Obtaining the files

If you have git installed, you can clone the repository to your local machine using

git clone https://github.com/bibekananda-datta/Abaqus-UEL-Elasticity.git

You can also fork the repository and sync as updates are deployed, develop your code by creating a separate branch, and propose updates using the pull and merge features of GitHub.

Alternatively, you can download the files in a zip folder in this repository using the code drop-down menu on the top right corner. In this approach, you will not receive any bug fixes and updates.

Note

Compiling the source code requires the LAPACK library from the Intel oneMKL package. See below for the details.

Description of the repository

All the source codes are located in the src subdirectory and the Abaqus test cases are located in the tests subdirectory. The documentations are available in the docs subdirectory.

File name	Description
uel_mech.for	is the Fortran source code that implements the isotropic linear elastic user element. The main UEL subroutine performs all the initial checks but the main calculations are performed in a subsequent subroutine. The source code includes additional subroutines with Lagrangian interpolation functions for 4 types of 2D continuum elements (Tri3, Tri6, Quad4, and Quad8) and 4 types of 3D continuum elements (Tet4, Tet10, Hex8, Hex20) and Gaussian quadratures with reduced and full integration schemes. Body force and traction boundary conditions were not been included in this implementation, however, these can be applied by overlaying standard Abaqus elements on the user elements (to be discussed in the Modeling in Abaqus section). Since Abaqus/Viewer does not provide native support for visualizing user elements, an additional layer of elements with the same element connectivity has been created and results at the integration points of the elements are stored using the UVARM subroutine.
<some_module>.for	These are the utility files with different Fortran module that are included in the main source file using include <filename.ext> statement at the beginning of the main source code.
addElemMech.py	is a Python code in the tests directory that modifies a simple Abaqus input file and adds the overlaying dummy elements on the user elements. For complicated input files, this will not work properly and modification of this code will be required (optional).
<...>.inp	are the example input files prepared to be executed with the user element subroutine. Since the user-defined elements share the same topology as one of the Abaqus built-in elements, those models were built in Abaqus/CAE and then exported as input files. Later those input files were modified to include keywords and data to include user element definitions, properties, and overlaying dummy elements.
abaqus_v6.env	is the Abaqus environment file for Windows systems which adds the additional compiling option for the Intel oneMKL package. This needs to be in the same directory as the Abaqus jobs.
runAbq.ps1	is a PowerShell batch file in the tests directory that can execute the user subroutine and specified input file from the PowerShell terminal (optional).
elastic_elem.pdf	is a summary of the theory and algorithm used to implement the provided source code.
Abaqus_docs.pdf	is a collection of publicly available Abaqus documentation in PDF format related to the Abaqus UEL subroutine. The web versions of these documents are available at https://help.3ds.com.

Modeling in Abaqus

Since the implemented user elements have the same topology as the built-in Abaqus elements, users can build a primary model in Abaqus/CAE and then export the input (.inp) file. Once the input file is available, as described in the Abaqus documentation, the following information needs to be modified.

Element definition

The first modification is to introduce the definition of the user element being used in the analysis with the element name, coordinates, nodes, and the number of real and integer properties required for that element.

Properties

For isotropic linear elastic elements developed in this UEL, users need to specify the following properties:

• Young's modulus, $E$
• Poisson's ratio, $\nu$
• Number of integration points, nInt
• Number of post-processed variables, nPostVars

Dummy elements for visualization

To visualize the results, an additional set of built-in Abaqus elements with the same element connectivity as the user element has been created in the input file. These additional elements (so-called dummy elements) have negligible elastic properties and thus will not affect the results. If you are using a reduced integration element from the user subroutine, then use the analogous elements from Abaqus as the dummy elements.

Configuring Abaqus and executing the subroutine

To run user subroutines in Abaqus, you will need to install Intel Visual Studio and Intel oneAPI package and link them with Abaqus. Follow this blog tutorial if you have not done it before. Additionally, see this blog post to learn how to link and use the LAPACK library from the Intel oneMKL package to Abaqus user subroutines.

Navigate to the tests directory. Open the Abaqus command line terminal or cmd terminal or PowerShell terminal, you can execute the following command from the directory to execute the subroutine. Make sure to use the right directory for the main source code.

abaqus interactive double analysis job=<your_job_name> input=<input_file_name.inp> user=../src/uel_mech.for

Specify the variable names (inside < >) in the above command as needed. For additional information on executing user subroutines, check the Abaqus user manual.

If you use the PowerShell-based terminal, you can also execute the subroutine by running the runAbq.ps1 file. Make sure to check the input file name in the file.

./runAbq

Citation

If you use this repository (documentation or source code), please consider citing this from the following:

APA format:

Datta, B. (2024, April 28). An Abaqus user element (UEL) implementation of linear elastostatics. Zenodo. https://doi.org/10.5281/zenodo.11075088.

BibTeX:

@misc{dattaAbaqusUserElement2024,
  author       = {Datta, Bibekananda},
  title        = {{An Abaqus user element (UEL) implementation of linear elastostatics}},
  month        = apr,
  year         = 2024,
  publisher    = {Zenodo},
  doi          = {10.5281/zenodo.11075088},
  url          = {https://doi.org/10.5281/zenodo.11075088}
}