Using ABAQUS

Contents

• Introduction
• Input Files
• The abaqus.env File
  • Example abaqus.env File
• Running ABAQUS Jobs
  • Example Input File
• Geometry Models
• Nodes and Elements Stored in Files
• More Information

Introduction

ABAQUS is a powerful finite element software package. It is used in many different engineering fields throughout the world. ABAQUS performs static and/or dynamic analysis and simulation on structures. It can deal with bodies with various loads, temperatures, contacts, impacts, and other environmental conditions. ABAQUS is developed and supported by Hibbitt, Karlsson & Sorensen, Inc. (HKS). ABAQUS includes four functional components:

• Analysis Modules
• Preprocessing Module
• Postprocessing Module
• Utilities

More details about the first three components are documented in ABAQUS Products. The utilities are additional programs included in the ABAQUS release and are described below. They are invoked through the ABAQUS execution procedure.

• ABAQUS abares - Translates ABAQUS restart files for post processing on other computers.
• ABAQUS append - Joins separate result files into a single file.
• ABAQUS ascfil - Translates ABAQUS result files between ASCII and binary formats. This is useful for moving result files between different computer types.
• ABAQUS fetch - Extracts example input files from the libraries included with the release.
• ABAQUS make - Compiles and links user-written postprocessing programs for ABAQUS.
• ABAQUS plot - Creates ABAQUS plot files for various hard copy devices.

ABAQUS is written in Fortran and it runs as a batch application. The input file to ABAQUS is an ASCII file which is composed and edited based on engineering knowledge and rules of ABAQUS input files.

Back to Top

Input Files

The ABAQUS input file is an ASCII file with an extension of .inp. This file helps users communicate with the ABAQUS analysis modules and it must be created first. As a general finite element package, ABAQUS has multiple built-in libraries. The four main libraries are:

• Element Library
• Material Library
• Loading Library
• Procedure Library

Each library implements many keywords with their required and optional parameters and data lines. These keywords and parameters are readable both by ABAQUS and by the user. In comparison with most computer languages, the construction of the ABAQUS input file is simple. The key is to select the correct keywords and parameters to configure the models and the analysis procedures. There are two kinds of input lines used in an input file: keyword lines and data lines. Figure 1 is an illustration of the composition of a ABAQUS input file. The original code is cited from ABAQUS/Standard User's Manual, Volume I

Figure 1

As shown in Figure 1, there are two parts to an input file: the model input and the history input. Very often the history input may consist of more than one paragraph which starts with *step and ends with *end step. The complexity of the job determines the total number of input lines but the basic order of definitions and construction in an input file is almost always the same.

Back to Top

The abaqus.env File

The abaqus.env is an environmental file available to users for use in configuring micro-environments for running different jobs. When a user runs a certain job on ABAQUS, he/she may need to control various aspects of an ABAQUS job's execution. Variables called environmental variables are used to control the job's execution. These variables are assigned default values by the ABAQUS Site but the user can modify the environment file, abaqus.env, to run different jobs. For example, a user may:

• Change memory-related parameters to improve the performance of the job.
• Control where and how scratch files are written.
• Provide his/her own default values for some parameters to make operations easier.

Also many other aspects of a job's execution can be configured via the abaqus.env.

When a job is submitted, ABAQUS will first search for the environmental file(s) in the following order:

1. The ABAQUS site subdirectory where abaqus.env defined by ABAQUS must exist.
2. The user's home directory where abaqus.env is optional and will affect all ABAQUS jobs submitted from user's account.
3. The current working directory where abaqus.env is optional and will affect all ABAQUS jobs submitted from the current working directory.

If an environment variable is defined more than once in more than one environment file, the last definition encountered will be used. Only the start_cmd and end_cmd are exceptions to this rule.

The following command line can be used to diagnose problems caused by possibly faulty environment file parameters:

  abaqus info=environment

Example of an Environment File

  queue_name="aba_short hold"
  after_prefix="-a"
  queue_prefix="-q"
  aba_short="qsub -me -q batch -lM 64mw -lT 10000 %A %T -eo -o %L %S"
  hold="echo Job %S not submitted"
  post_geometry="800x500+12+34"
  post_buffer="12000000"
  post_memory="12000000"
  cpus=1

More details about the ABAQUS environment variables and their default values can be obtained from the "Using the ABAQUS environment file" section in the ABAQUS/Post Manual.

Back to Top

Running ABAQUS Jobs

The input file in Figure 1 will serve as a simple start for a new ABAQUS user. This file provides the input lines for the static analysis of a simple beam and can be named beam.inp. The command to run the job is:

  abaqus job=beam

or

  abaqus
  Under the prompt of Identifier, enter the name of
  input file, beam without the .inp extension.

If you have run this job before, ABAQUS will prompt Old job files exist. Overwrite? (y/n) and stop for your answer.

Example Input File, beam.inp

  *heading
  cantilever beam
  *node, nset=ends
  1, 0.
  6, 100.
  *ngen
  1, 6
  *element, type=b21
  1, 1, 2
  *elgen, elset=beam
  1, 5
  *beam section,
  section=rectangular,
  elset=beam, material=steel
  1., 2.
  *material, name=steel
  *elastic
  30.e6
  *boundary
  6, encastre
  *step, perturbation
  *static
  *cload
  1, 2, -20000.
  *el print, position=averaged at nodes,
  summary=yes
  s11, e11
  sf
  *node file, nset=ends
  u, cf, rf
  *restart, write
  *end step

On running this job, several files will be generated. Among them, will be three files with the extensions .log, .dat and .msg respectively. These files are important and useful for testing and checking input files.

• .log: Log file -- it records the summary information about the job execution.
• .dat: Printed output file -- it records all information about your input model together with error information.
• .msg: Message file -- it mainly reports the information and errors that occurred while executing the history input.

These are three tools besides the ABAQUS/Post that help check and correct the input file. They are all ASCII files and can be viewed with the cat and more commands.

Back to Top

Geometry Models

A geometric model code should include the node and node set definitions, and the element and element set definitions (see Figure 1).

The commonly used keywords for creating nodes and elements and defining node sets and element sets are:

• keywords for node and node set definitions are:
  *node, *ngen, *nfill, *nset, *ncopy, *nmap
• keywords for element and element set definitions are:
  *element, *elgen, *elset, *elcopy

Figure 2 is used to explain how to use the above keywords to define geometric model in an input file. It is a two dimensional domain and the design of its nodes and elements are shown in Figure 3.

Figure 2

Figure 3

The geometry model in Figure 3 can be coded using the following example of an input file:

Geometry Example File

  *HEADING
  An example of 2-D geometry model
  *NODE   
  35,0.,0.,0.     
  37,1.0,0.,0.
  38,1.5,0.,0. 
  40,3.5,0.,0.
  435,0.,2.0,0.
  437,1.0,2.0,0.
  438,1.5,2.0,0.    
  440,3.5,2.0,0.    
  635,0.,4.0,0.       
  637,1.0,4.0,0.   
  638,1.5,4.0,0. 
  640,3.5,4.0,0. 
  *NGEN,NSET=X11  
  35,37   
  *NGEN,NSET=X12  
  38,40   
  *NGEN,NSET=X13
  435,437 
  *NGEN,NSET=X14
  438,440
  *NGEN,NSET=X15  
  635,637       
  *NGEN,NSET=X16  
  638,640       
  *NFILL,NSET=BLOCK1
  X11,X13,4,100
  *NFILL,NSET=BLOCK2
  X12,X14,2,200
  *NFILL,NSET=BLOCK3
  X13,X15,2,100
  *NFILL,NSET=BLOCK4
  X14,X16,2,100
  *NGEN,NSET=RIGHT
  40,240,200
  440,640,100
  *NSET,NSET=TOP
  X15,X16
  *NSET,NSET=NALL
  BLOCK1,BLOCK2,BLOCK3,BLOCK4
  *ELEMENT,TYPE=DC2D4    
  35,35,36,136,135
  *ELGEN,ELSET=EBLOCK1
  35,2,1,1,4,100,100     
  *ELEMENT,TYPE=DC2D4     
  38,38,39,239,238
  *ELGEN,ELSET=EBLOCK2      
  38,2,1,1,2,200,200     
  *ELEMENT,TYPE=DC2D4     
  435,435,436,536,535
  *ELGEN,ELSET=EBLOCK3     
  435,3,1,1,2,100,100
  *ELEMENT,TYPE=DC2D4     
  438,438,439,539,538     
  *ELGEN,ELSET=EBLOCK4      
  438,2,1,1,2,100,100
  *ELEMENT,TYPE=DC2D3     
  37,37,38,137
  *ELGEN,ELSET=EBLOCK5     
  37,1,1,1,2,200,200
  *ELEMENT,TYPE=DC2D3     
  137,137,238,237
  *ELGEN,ELSET=EBLOCK6     
  137,1,1,1,2,200,200
  *ELEMENT,TYPE=DC2D3
  138,137,38,238
  *ELGEN,ELSET=EBLOCK7
  138,1,1,1,2,200,200
  *ELSET,ELSET=ALLBLOCK
  EBLOCK1,EBLOCK2,EBLOCK3
  EBLOCK4,EBLOCK5,EBLOCK6,EBLOCK7
  *SOLID SECTION,ELSET=ALLBLOCK,MATERIAL=SILT
  *MATERIAL,NAME=SILT     
  *CONDUCTIVITY   
  1.2,-40.
  1.2,31.2
  .9,32.  
  .9,80.  
  *DENSITY
  105.    
  *SPECIFIC HEAT  
  .27,-40.
  .27,31.2
  .37,32. 
  .37,80. 
  *LATENT HEAT    
  28.8,31.2,32.   
  *INITIAL CONDITIONS,TYPE=TEMPERATURE    
  NALL,24.8       
  *RESTART,WRITE  
  *STEP,INC=100   
  TEMPERATURE ANALYSIS 
  *HEAT TRANSFER
  1.,50.
  *BOUNDARY
  35,11, ,37.8
  36,11, ,37.8
  37,11, ,37.8
  235,11, ,37.4
  135,11, ,37.4
  TOP,11, ,24.8
  RIGHT,11, ,24.8
  *PRINT,FREQUENCE=1
  *NODE PRINT,FREQUENCE=1 
  NT      
  *NODE FILE,FREQUENCE=1
  NT      
  *CONTOUR
  TEMP    
  *END STEP       

The above code is a sample input file for a heat transfer problem, in which the 2-D element TYPEs are selected as DC2D4 & DC2D3. Its testing result is shown in Figure 4 below. By highlighting each line, you can copy it into your own input file and try it on ABAQUS.

Figure 4: The 2-D Model Plot by ABAQUS/Post.

Back to Top

Nodes and Elements Stored in Files

For a complicated problem in finite element analysis, the meshed domain may consist of many thousands of elements and nodes. Due to the potential complexity of a problem, the design of its domain, elements and nodes can be obtained from other more convenient graphic packages. Then the node numbers, node coordinates, and node members forming each element can be transformed into the data files with formats defined by keywords *node and *element. As an example, the Input file example in the previous section is modified for this section. To show their applications in geometry models, the keywords of *ncopy and *elcopy are used here even though the *elcopy can be omitted. And also the 3-D element TYPEs (DC3D8 & DC3D6) are used here instead of the 2-Ds.

  Input file: beam1.inp                     Data file: gm3dnd.txt
                                           
  *HEADING                                   35,0.,0.,0. 
  An example of 3-D geometry                 37,1.0,0.,0.
   model (modified)                          38,1.5,0.,0.   
  *NODE,INPUT=gm3dnd.txt                     40,3.5,0.,0.     
  *NGEN,NSET=X11                             435,0.,2.0,0. 
  35,37                                      437,1.0,2.0,0.
  *NGEN,NSET=X12                             438,1.5,2.0,0.
  38,40                                      440,3.5,2.0,0. 
  *NGEN,NSET=X13                             635,0.,4.0,0.
  435,437                                    637,1.0,4.0,0.
  *NGEN,NSET=X14                             638,1.5,4.0,0.
  438,440                                    640,3.5,4.0,0.
  *NGEN,NSET=X15  
  635,637       
  *NGEN,NSET=X16  
  638,640       
  *NSET,NSET=NFRONT
  BLOCK1,BLOCK2,BLOCK3,BLOCK4
  *NCOPY, OLD SET=NFRONT,
  NEW SET=NBACK,
  CHANGE NUMBER=4000,
  REFLECT=MIRROR
  0.0,0.0,-2.0,1.0,0.0,-2.0
  0.0,1.0,-2.0
  *NFILL,NSET=NALL
  NFRONT,NBACK,4,1000
  *ELEMENT,TYPE=DC3D8,
  INPUT=gm3del1.txt                         Data file: gm3del1.txt
  *ELGEN,ELSET=EBLOCK1
  35,2,1,1,4,100,100,2,1000,1000      35,35,36,136,135,1035,1036,1136,1135 
  *ELGEN,ELSET=EBLOCK2                38,38,39,239,238,1038,1039,1239,1238
  38,2,1,1,2,200,200,2,1000,1000      435,435,436,536,535,1435,1436,1536,1535
  *ELGEN,ELSET=EBLOCK3                438,438,439,539,538,1438,1439,1539,1538
  435,3,1,1,2,100,100,2,1000,1000
  *ELGEN,ELSET=EBLOCK4      
  438,2,1,1,2,100,100,2,1000,1000
  *ELEMENT,TYPE=DC3D6,
  INPUT=gm3del2.txt                       Data file: gm3del2.txt 
  *ELGEN,ELSET=EBLOCK5
  37,1,1,1,2,200,200,2,1000,1000        37,37,38,137,1037,1038,1137 
  *ELGEN,ELSET=EBLOCK6                  137,137,238,237,1137,1238,1237
  137,1,1,1,2,200,200,2,1000,1000       138,137,38,238,1137,1038,1238 
  *ELGEN,ELSET=EBLOCK7
  138,1,1,1,2,200,200,2,1000,1000
  *ELSET,ELSET=FIRSTHALF
  EBLOCK1,EBLOCK2,EBLOCK3
  EBLOCK4,EBLOCK5,EBLOCK6,EBLOCK7
  *ELCOPY,OLD SET=FIRSTHALF,
  NEW SET=SECONDHALF,ELEMENT SHIFT=2000,
  SHIFT NODES=2000
  *ELSET,ELSET=ALLBLOCK
  FIRSTHALF,SECONDHALF
  ...
  ...
  ...

Figure 5: The 3-D Model Plot by ABAQUS/Post

Back to Top

More Information

• For help contact User Support

Arctic Region Supercomputing Center
PO Box 756020, Fairbanks, AK 99775 | voice: 907-450-8600 | email:

home | search | about | support | news | science | resources