Tutorials - Abaqus

ABAQUS

1. Introduction

This tutorial demonstrates how to run and view the results of an explicit crash simulation using the ABAQUS suite of FEA products on VPAC's HPC facility. Please not that model pre-processing is not discussed.

VPAC has an ABAQUS license with 100 "tokens". The number of tokens required for various combinations of ABAQUS features and core use is shown in the following table.

Capture

Note that any execution can effectively lock out others based on the numbers of cores and the specific ABAQUS feature set used. The tokens in concurrent use cannot exceed 19, and 5 are required for the most basic execution.

Note that a single 16 core execution will effectively lock out all other ABAQUS executions because there will not be 5 tokens available for even another single core job. Users needing higher core count executions for time-to-solution should use 24 cores (not 16) to minimise elapsed execution time, and thus enable other ABAQUS users to have tokens available at the earliest possible wall time.

If you do not have time critical requirements, please use 1, 2, 4, or at most 8 cores to enable 2 or 3 "low core count" simulations to be in concurrent execution, thus providing the best opportunity for all ABAQUS users to receive service.

NOTE: Because Abaqus is commercial software and only licensed for academic use VPAC users must email a request to help@vpac.org asking to be given access to the package. Unfortunately we can only offer assistance with Abaqus to people from VPAC member institutions. Please also note that VPAC has a limited number of licenses for Abaqus. Please see the license page for adding these to your PBS script.

The case study is a car door being propelled into a pole. This is analogous to the EURONCAP pole test, in which a car is propelled sideways into a rigid pole of diameter 254 mm at 29 km/h. While a crash event generally lasts for around 100 milliseconds, the time step of the case study has been reduced to 10 milliseconds to reduce the job time. A schematic of the assembly is shown in the following figure.

abaqus-001

Text inside [Square Brackets] indicates that there is a button to push in the GUI of the program being described. Menu command sequences are linked by ">" symbols.

3. Nomenclature
CAE Complete ABAQUS Environment
EURONCAP European New Car Assessment Programme
GUI Graphical User Interface
ODB Output Database

4. Job Submission

Serious compute loads must be launched via PBS Trifid. Copy the job files to your working directory using the following commands:

ssh username@trifid.vpac.org
cp -r /common/examples/abaqus/door .
cd door/
ls


The files copied to your working directory are shown below:

Door.cae ­ ABAQUS model database file Door.jnl ­ ABAQUS model database journal file Door.inp ­ ABAQUS input deck Door.odb ­ ABAQUS output database file pbs-abaqus ­ pbs job submission script

A sample PBS script for ABAQUS is shown below.

#!/bin/bash
#PBS -l nodes=2:ppn=2
#PBS -l walltime=0:05:00
#PBS -N AbaqusDoor
#PBS -W x=GRES:abaqus+14
# PBS -m ae
# Go to the directory from which you submitted the job
cd $PBS_O_WORKDIR
module load abaqus
#
# Run the job 'Door'
abaqus job=Door


Submit the job using the following command:
qsub pbs-abaqus The status of the job can be queried using the following command:

tail -­f door.sta

5. Post-Processing

Once the job has completed, all files, with the exception of the output database (.ODB) file can be deleted. By default, ABAQUS/CAE writes the results of the analysis to the ODB file. When you create a step, ABAQUS/CAE generates a default output request for the step, which in the case of this analysis is Energy Output.

You use the Field Output Requests Manager to request output of variables that should be written at relatively low frequencies to the output database from the entire model or from a large portion of the model. You use the History Output Requests Manager to request output of variables that should be written to the output database at a high frequency from a small portion of the model; for example, the displacement of a single node.

The results will be visualised using ABAQUS/CAE. It should be noted that ABAQUS/Viewer is a subset of ABAQUS/CAE that contains only the post-processing capabilities of the Visualization module. The procedure discussed in this tutorial also applies to ABAQUS/Viewer. Copy the files to your local machine and run the Abaqus CAE.

scp -r username@trifid.vpac.org:door .
abaqus cae


The following procedure is used to open the ODB file;

  1. Click [Open Database] in the Session Start window.
  2. The Open Database dialog will appear. Select Output Database from the File Filter dropdown menu.
  3. Select Door.odb and click [OK].
By default, ABAQUS/CAE will plot the undeformed shape with exterior edges visible.

For clarity (if the mesh density is high) it may be necessary to make feature edges visible. The following procedure is used:

  1. Click [Common Plot Options] in the Toolbox Area.
  2. In the Basic Tab, check Feature edges in the Visible Edges section.
  3. Click [OK]. The door assembly undeformed shape plot is shown in the following figure. Both exterior edges and feature edges are shown.

abaqus-004
5.1. Deformed Shapes

The following procedure can be used to plot the crash models deformed shape:

  1. Click [Plot Deformed Shape] in the Toolbox area. By default, the final step is displayed. It should be noted that the Deformation Scale Factor is 1 by default in explicit analyses.
  2. Click [Animate: Time History] to animate the crash event. The frame rate can be adjusted by clicking [Animation Options] and moving the slider in the Player tab to the desired speed.
The door assembly deformed shape plot is shown in its final increment in the following figure.

abaqus-006

The following procedure can be used to plot contours over the deformed shape:

  1. Click [Plot Contours on Deformed Shape] in the Toolbox area.
  2. If the user intends to compare a number of different configurations of the same model, the minimum stress/strain value should be set to the same value for each configuration. Click [Contour Plot Options], select the limits tab and check Specify and set the value to 0. In analyses were non-linear geometry is considered, the user can also specify a maximum strain/stress to help gauge the location(s) of any plastic regions.
  3. The output variable can be modified by clicking Result > Field Output. By default Mises stresses are plotted. A number of invariants are available for each output. Note that the field output variable can also be modified in the Probe Values dialog.
The door assembly contour on deformed shape plot is shown in the following figure.

abaqus-007

The stresses and strains of individual elements can be probed as follows:

  1. Click Tools > Query and select Probe Values. Click [Apply]. The Probe Values dialog will appear.
  2. Check the appropriate output variable in the Probe Value section and click on an element of choice. The probed values of each element selected can then be written to a text file.
It should be noted that default probe location is the integration point of the element. Hence, for this example, one value will be stored to the Selected Probe Values table since the element is a reduced integration shell of type S4R. It should also be noted that the stresses and strains shown in the contour plot are an average of the actual stress that is calculated at the integration point.

The following procedure can be used to save image animation:

  1. Plot a deformed shape or contour on deformed shape using the procedure described above.
  2. Animate the results event using the procured described above.
  3. Click Animate > Save As. Accept the default file format (AVI) if you plan to use the animation in a PowerPoint presentation. However, it should be noted that QuickTime format offers better compression and image quality.
  4. Specify a file name and location and click [OK].
  5. It should be noted that viewport annotations can be toggled off for clarity. Click Viewport > Viewport Annotation Options and uncheck any information that is not required.

5.2. XY Data Plotting

History output can be used to plot XY Data. In this example, all energy output variables (whole model) were written to the ODB file. The user can save a numerous output variables for node/element sets that are present in a model.

The following procedure can be used to plot XY Data:

  1. Click [Create XY Data], accept the default selection (ODB history output) and click [Continue].
  2. Select Internal Energy and Kinetic Energy and click [Plot]. All XY data can be exported to Excel in .CSV format.
A sample XY plot is shown in the following figure showing kinetic energy and internal energy versus time.

abaqus-010

It should be noted that it may be necessary to "operate" on XY Data to create certain plots that are not time dependent (Force-displacement etc). The following procedure will demonstrate this process:

  1. Click [Create XY Data], accept the default selection (ODB history output) and click [Continue].
  2. Select data set 1 and click [Save As]. Give the data an appropriate name.
  3. Repeat step 2 for data set 2. Click [Dismiss].
  4. Click [Create XY Data] and select Operate on XY Data.
  5. From the Operators section, select combine(X,X). Double click the x-axis data, and then double click the y-axis data. Click [Save As] followed by [Plot Expression].

Top of Page