3D Contact Tutorial

This tutorial gives a short introduction to the setup of a simple 3D contact problem. The goal of this tutorial is to give an overview of the general workflow in 4C and to show how to create a working .dat input file. It is neither intended to be an introduction to the theory of contact mechanics, nor demonstrate all possible optional settings for a given (contact) problem. It is assumed that 4C has been built on your machine according to the instructions and has passed the tests without error messages. For further information on how to build 4C and to test the build, please refer to the README.md.

Overview

  1. Problem description

  2. Create files

    1. Define Geometry

    2. Define Boundary Conditions

    3. Specify Simulation Settings

  3. Create .dat input file

  4. Run Simulation in 4C, Post-processing and visualization in Paraview

Problem description

In this tutorial we create two cubes sizes 1x1x1 and 0.5x0.5x0.5, with a time dependent Dirichlet boundary condition ( DBC) imposed on the right outer surface of the smaller cube. As a result, the smaller cube is pressed horizontally against the larger counterpart, which is clamped on the left outer surface. Mortar methodology is applied for the discretization of the contact constraints and the subdomains are coupled with dual Lagrange multipliers. The cubes are assumed to consist of two different materials, represented by a St.Venant-Kirchhoff material model with different values of the Young’s modulus and density for each cube.

Create files

To create a .dat input file for 4C we need three files:

  • .exo/.e file containing the geometry and mesh

  • .bc file containing information on the boundary conditions

  • .head file containing all relevant parameter settings for the simulation

Define Geometry

Information on the geometry and mesh are passed on to 4C as part of a binary EXODUS file (.e). This file can be generated using the pre-processing software Cubit. Before we can export an .exo file from Cubit (File -> Export -> Files of type: .e), we need to specify the geometry and meshing parameters in Cubit. This can be done using the GUI or read from a journal file (.jou) containing the specific Cubit commands. A tutorial on how to use the Cubit GUI can be found on the coreform webpage and can be useful to get to know some of the basic functionalities. The syntax of a Cubit command to a corresponding Input using the GUI can be seen in the Cubit terminal.

Remark: After learning the syntax of the basic Cubit commands, it may be more convenient to exclusively use journal files for an easy adaptation and reproduction of your geometry and/or use in e.g. python scripts for parameter studies etc.

In tutorial_contact_3d.jou it can be seen, that apart from the basic geometry definition and meshing, nodesets and element blocks are assigned to the corresponding nodes/lines/surfaces/volumes. The nodesets are used later on to assign the boundary conditions, whereas the element blocks are used to assign material properties. Additionally, the last line in the given journal file includes a terminal command to export the .exo/.e file from cubit.

The journal file can be called in Cubit from the Terminal with the command

/path/to/cubit/executable -nographics /path/to/tutorial_contact_3d.jou

This saves the .exo file in the current work directory.

Define Boundary Conditions

For the definition of the boundary conditions, it is convenient to use the prototype of the .bc file, as it provides syntax examples and a basic structure that automatically inserts the information on number of nodes in each block element/nodeset/etc. It also gives a list of all possible conditions that can be defined, as well as the element type names and the corresponding shapes. Depending on the type of the problem, undefined/empty/unnecessary lines can be deleted when using it as a template. Information on how to obtain prototypes for both the .bc file and the .head file is given in the README.md under the heading “Prepare and Run Simulations”. The terminal command to obtain both prototype files is:

<buildDir>/pre_exodus --exo=tutorial_contact_3d.e

In tutorial_contact_3d.bc it can be seen, that the first two blocks of text define the structure elements, which will later fill the system matrices. The other text blocks define conditions on parts of the system. The first line of each block assigns an (optional) name to the element block/nodeset and the shape of the element type is specified. The next part has already been filled in by pre_exodus. For our simple geometry and discretization it can easily be checked that the number of elements/nodes in the corresponding element blocks and nodesets is correct. Next, the Section of the .dat file under which this information will be listed is given. the structure element properties are listed under STRUCTURE, whereas the boundary/contact conditions will be listed under their corresponding section names. The parameters for assigning a material model to an element block with SOLID elements of shape HEX8 are:

description="MAT 1 KINEM nonlinear"

where we choose material model 1, set the kinematics to nonlinear and assume no enhanced assumed strain. Last, the element type/condition specific set of parameters is given and the name of the element type is specified. Hint: A list of possible options can be found in the .bc default file.

Remark: Apart from the separate listing of problem specific conditions, Dirichlet and Neumann BCs (as well as many other types of conditions) are also listed separately, depending on the geometric entity that they are imposed on, e.g. points, lines, surfaces or volumes.

The parameters for the definition of a DBC are:

description="NUMDOF 3 ONOFF 1 0 0 VAL -1.0 0.0 0.0 FUNCT 1 0 0"

where: NUMDOF = number of degrees of freedom per node, ONOFF = on which of the DOF is the condition imposed (Binary 1/0), VAL = scaling parameter, FUNCT = Assign a numbered function to a dof (here Function1, defined in .head file).

The master and slave surfaces for the definition of the contact mortar problem can be specified as:

description="1 Master"

Remark: It is common practice to choose the side with the finer discretization as the slave side.

Specify Simulation Settings

The prototype of the .head file contains an extensive list of possible parameter settings for running a simulation in 4C. It also gives information on the numerous abbreviations used in the input files. Hint: Use the search function of your editor to navigate the 13000 lines of text.

As we are setting up a structural contact problem, not all sections and parameters are required (e.g. sections concerning the simulation of fluids, etc. can be left out). If they are not specified explicitly in our input file, the parameters take on default values. Some sections that are required by all problem types include PROBLEM SIZE, PROBLEM TYPE, DISCRETIZATION, IO (Input/Output), at least one SOLVER section (for contact problems we need to specify two solvers: one for the state, where not contact is active, and one for the state with active contact) and a MATERIALS section. The time integration method DYNAMICTYPE (Generalized alpha method), time step size TIMESTEP and final time MAXTIME are also specified for structural dynamics. An important parameter is RESULTSEVERY, which specifies how often output is written and thus directly controls the size of the output file.

The contact specific parameters are given under --MORTAR COUPLING. Dual Lagrange multipliers are chosen for the coupling of the interface. Either the BruteForceEleBased algorithm, or the more efficient BinaryTree can be chosen as the contact search algorithm. In tutorial_contact_3d.head you will also find the definition of the FUNCTION that is used for the time dependent DBC.

Create input file

The final .dat input file for 4C can be created with the pre_exodus executable as described in the README.md. To manually create the .dat file the full command states:

<buildDir>/pre_exodus --exo=tutorial_contact_3d.e --head=tutorial_contact_3d.head --bc=tutorial_contact_3d.bc --dat=tutorial_contact_3d.dat

This saves the .dat file in the current work directory. The .dat file now contains all the information from the created files, plus a list of all nodes and structure elements.

Remark: The framework testing with ctest executes the command above automatically.

Run Simulation

Again, following the instructions from the README.md, the 4C executable can be invoked with the tutorial_contact_3d.dat input file. Since we chose the binary output option in our .head file (section IO), we also have to run a post processing tool before visualizing the results in Paraview.