Contents     Functions              PDF Index

abaqus

• read[*.fil, *.inp, *.mtx, *.dat]
• Build[model,case,contact]
• Resolve
• write
• JobOpt
• conv
• splitcelas
• uniquematpro
• AssembleUserElements
• odb2sdt
• odb2sdt.py reference
• Examples

Purpose Interface between ABAQUS and SDT (part of FEMLink) Warning this function requires MATLAB 7.1 or later.

Syntax

  abaqus('read FileName');
  abaqus('job');

read[*.fil, *.inp, *.mtx, *.dat]

By itself the read command imports the model from a .inp ASCII input or .fil binary output file. Support for .dat read is very partial, but provides a framework for users to parse desired tokens.

Models created by an *Assembly command using several instances and/or additional nodes or elements are treated with superelements. Each part instance (called by *Instance…*end instance) becomes then a specific superelement in the SDT model. A packaged call allows to get a full model back

model=abaqus('read Job-1.inp');
model=abaqus('ResolveModel',model);
% both calls at once:
model=abaqus('read-resolve Job-1.inp');

The ResolveModel command has a limited robustness in the general case due to the difficulty to handle heterogeneous Stack data while renumbering parts of a model. Most cases should be properly handled. One can use command read-resolve to perform both operations at once.

When reading deformations, sdtdef('OutOfCoreBufferSize') is used to determine whether the vectors are left in the file or not. When left, def.def is a v_handle object that lets you access deformations with standard indexing commands. Use def.def=def.def(:,:) to load all. If a modal basis is read, it is stored in the model stack, as curve,Mode. If static steps are present all associated deformation are concatenated in order of occurrence in the model stack as curve,step(1).

Command option -wd allows to save the model generated in a directory different from the one in which the abaqus files are saved.

You can request the output of element matrices which will then be read into an upcom model. To do so, you need to define an element set. To read matrices, you have to provide some information before running the job in order to select which matrices you want to write and read. In the .inp input file you may enter the following line

*ELSET, ELSET=ALL ELT FOR SDT
THIN SHELL1 , THIN SHELL1_1 

(second line contains all the ABAQUS defined sets) just before the *STEP line and

*ELEMENT MATRIX OUTPUT, ELSET=ALL ELT FOR SDT, STIFFNESS=YES
*ELEMENT MATRIX OUTPUT, ELSET=ALL ELT FOR SDT, MASS=YES

just after the *STEP line.

Note that this information are automatically generated using the following command abaqus('elementmatrices model.inp'); .

Running the Abaqus job generates outputs specified by the user, with *OUTPUT commands in the Abaqus job input file. Current default use generates an odb file, using commands of the type *NODE OUTPUT. The odb format however requires the use of Abaqus libraries to be read.

Imports are thus handled in SDT using the .fil output binary file. This file is readable without Abaqus, and its reading has been optimized in FEMLink. This type of output is generated using commands of the type *NODE FILE. A sample command to obtain nodal deformation a the end of a step is then

** general command to .fil and ask for nodal deformation field
*OUTPUT, FIELD
*NODE FILE
 U

All nodal variable keywords should be expressed on separated lines. This must be repeated in all steps of interest in an ABAQUS computation file input .inp.

Most common and general nodal variables keywords of interest are the following (this is not applicable to all ABAQUS procedures)

• U, V, A respectively for nodal displacement, velocity and acceleration output
• RF,CF, VF, TF respectively for nodal reaction forces, constrained forces, viscous forces, and total forces output
• GU, GV, GA respectively for generalized displacement, velocity ad acceleration (when reduction is involved)

Since not all information (materials, set names, ...) can be found in the .fil, you may want to combine two reads into an upcom model

abaqus('read file.inp', 'buildup file.fil');.

Abaqus features a matrix sparse output starting from version 6.7-1. Their generation is performed in a dedicated step as follows

*STEP
*MATRIX GENERATE, STIFFNESS, MASS
*END STEP

The output is one ASCII file .mtx by matrix requested, which can be read by abaqus.

Reading a .dat file should be avoided in general as the ASCII storage format and variation between ABAQUS versions makes it unpractical. There are however cases where such reading is the easiest way; A framework adapted to such parsing is provided with support to read complex mode shapes (that cannot be stoed in the .fil file).

One can call data=abaqus('Read',fdat,li); with fdat a .dat file and li an optionnal Nx2 cell array providing a list of tokens to detect and and associated callback. The supported tokens are used if li is omitted, it is separately accessible with li=abaqus('DatList'); if users wish to combine supported features with customized ones.

If a token is detected in the file, a callback will be fired as out1=feval(cbk1,fid,evt,cbk2:end); with cbk the callback cell array provided in the second column of li, fid the valid opened file object set a the starting position of the currently detected token, evt a structure with fields .p0 the starting position of the scanned text buffer (not the current position to be recovered by pcur=ftell(fid);, .p1 the file length, .bufs a buffer size to be exploited. The callback command must rethrow a structure whose field will be incremently added to the global output structure.

Build[model,case,contact]

Thise set of high level commands aims at transforming a raw imported model into a functional model in SDT. It exploits in particular the lower level abaqus Resolve commands.

• BuildCase step istep
  model=abaqus('BuildCase step1',model); This command prepares the model case loading corresponding to a given step index istep. Raw model reading imports indiferently all boundary conditions and loading into the Case Stack. The loading sequence is stored in the stack entry info,BSHist and is exploited by BuildCase to generate the loading relative to a given step. One can ask for the last step by using token steplast instead of step istep. Command options
  • all restores all case entries in the Case Stack.
  • -noResolve asks not to perform the abaqus Resolve call if this was previously performed.
• BuildModel step istep
  model=abaqus('BuildModel step1',model); This command generates the model global state at a given step specified by step index istep. In addition to the BuildCase functionalities, this function looks for a static response result corresponding to the given set to define a curve,q0 entry, thus declaring a static state in the SDT model. One can ask for the last step by using token steplast instead of step istep. Command options
  • -noResolve asks not to perform the abaqus Resolve call if this was previously performed.
  • -contactCAM link to a call to the BuildContact command with forwarding of additionnal command options given in CAM. This feature is only accessible with a valid SDT-Contact module license.
  • -getStatic to only resolve the static state. The output is then the static state. It is possible to specifiy in intial set of static deformations in an additional argument. q0=abaqus('buildModel-steplast-getStatic',model,...
    stack_get(mo1,'curve','step(1)','get')).
• BuildContact step istep
  model=abaqus('BuildContact step1',model); This command packages the generation of SDT contact elements and laws based on the ABAQUS definition. This feature is only accessible with a valid SDT-Contact module license. The import generates contact elements based on master surfaces with penalized contact laws. Hard contact laws are thus automatically penalized with a calibrated stiffness density. Support for the *CONTACT PAIR, *MOTION, *CLEARANCE, *CHANGEFRICTION commands is provided and integrates *SURFACE BEHAVIOR and *FRICTION law inputs.

  The step definition is mostly usefull for *MOTION and *CHANGE FRICTION commands.One can ask for the last step by using token steplast instead of step istep. Command options

  • -module has to be used for users with no access to the SDT-NL tools outside SDT-Contact.
  • Command option -useRes asks to initialize contact states based on static force resultants on surface rather than by observing gaps on the static deformation field. This can be usefull to alleviate contact state import discrepancies due to different contact implementations between ABAQUS and SDT.
  • -optim is used to remove curves from the model that are not usefull for further anlysis after the BuildContact step is performed.
  • -tgStickNoMotion can be used to define tangential sticking property for contact with friction and no motion.
  • -moRot is used to specify the local definition of contacts : tangent and normal directions
    • -moRot”cyl” defines a cylindrical contact (for example the sliding contact of a drum brake)

Resolve

This set of commands transforms a raw model import by abaqus read into en exploitable SDT model. This is for example useful when the ABAQUS model has been generated with *PART and *INSTANCE. In such case, the representation of an ABAQUS model becomes very far from an SDT model. The raw reading obtained by read will thus interpret parts as superelements, and leave the instance data, and some internal information not translated. Some other advanced definitions need special care and are thus handled in this section.

Some adaptations, performed by ResolveModel are thus needed. In particular, renumbering can occur, however all sets definitions are maintained.

• ResolveModel
  This command will create the elements conforming to the instance information. Commands ResolveSet, ResolveMass, AssembleUserElements, ResolveCase and ResolveShellC will also be called, to generate a fully exploitable SDT model.
• ResolveSet
  This command transforms each ABAQUS implicitly defined sets into explicit SDT sets. This is very useful if some sets have been defined in ABAQUS using internal part numerotations. This command is also usefull to distinguich sets of different types but with initially the same name. This behavior is not available in SDT and special care is taken not to mixup set names and types. Called by ResolveModel.
• ResolveCase
  This command aims at resolving all implicitly defined case entries in the model, including *MODEL CHANGE, and some connector calls. This also handles the multiple slave resolution in the manner of ABAQUS, and should thus be performed before assembling models if multiple slave error occur.
• ResolveMass
  This command handles the model stack entry info,UnResolvedMasses that may have been created during the read call, and assigns mass values missing in mass elements. This is necessary when masses have been defined in an ABAQUS part, such that the attribution of the mass amplitude by *MASS is not directly retrievable. Called by ResolveModel.
• ResolveShellC
  Continuum shell elements (SC8R and SC6R) have no direct counterparts in SDT. A base resolution just ignores the shell declaration and declare these elements as solids with reduced integration (this may not work for stacked layers of continuum shells). The following command options are available
  • -shellSE will generate a superelement embedding shells in SDT format from the neutral fiber of the continuum shells, within the 3D topology. In that way a behavior equivalent to ABAQUS is expected.
  • -order2 in combination with -shellSE uses second ordr shells instead of first order ones.

write

abaqus('write Name.inp',model); writes and ABAQUS input file.

abaqus('BwMTX',model); writes all matrices stored in model.K in the abaqus sparse output format. Each matrix file is named after the model.file entry and model.Klab. For a model stored in model.mat containing a matrix 'k', the file output will be named model_k.mat.

BwMat ; BwMp ; BwSet ; Bwbas ; BwStepEig are implemented.

JobOpt

JobOpt = abaqus('JobOpt',Opt); This command returns a filled JobOpt structure to be run by sdtjob. Opt is a structure containing at least the field Job as the job name or file. InList and OutList must be filled. Further options concern the fields Input when the input file is different from the job name, RunOptions to append the usual option to the Abaqus command, RemoveFile to remove files from the remote directory when needed.

conv

This command lists conversion tables for elements, topologies, face topologies. You can redefine (enhance) these tables by setting preferences of the form sd_pref('set','FEMLink','abaqus.list',value), but please also request enhancements so that the quality of our translators is improved.

splitcelas

model=abaqus('SplitCelas',model) splits all SDT celas elements to one dimension celas elements that can be handled by Abaqus. This command can change the EltId so it must be used when meshing the model.

uniquematpro

Merges duplicated pl/il instances.

AssembleUserElements

Returns a matrix and its corresponding DOF, from the assembly of all USER ELEMENT instances in an ABAQUS model. This command is exploited in abaqus Resolve calls.

[K,dof] = abaqus('AssembleUserElements',model);

Command option -inModel directly sets a SDT functional superelement named usere in the model. In this case, element matrices are removed from the stack. They can be kept with command option -keep.

Command option -disjsplit splits the assembled SE into disjoint SE regarding DOF connectivit, resulting SE are named uei with i a 6 digit fixed index.

model=abaqus('AssembleUserElements-inModel',model);

odb2sdt

Utility functions to transfer Abaqus .odb file data into a format similar to MATLAB 6 binary .mat file and readable by sdthdf. The changes in the format are introduced to support datasets larger than 2GB.

Abaqus outputs are commonly written in .odb files, using a non documented format. The only way to access its data is to use Abaqus CAE or Abaqus Python. These utility functions are to be used with Abaqus Python to extract data from the output database for further use outside Abaqus. The modules used are

• odbAccess. Abaqus access libraries.
• abaqusConstants. Common output values dictionary, such as 'U', 'UR'
• Numeric. Module for array handling utilities.
• struct. Module to pack data into binary strings.

For the moment, only nodal data transfer is completely implemented. More information can be found on Python at http://www.python.org. Note that def is a reserved word in Python for the function definition command; remember not to use it in another way!

The following script is a quick example of what can be done with these functions. It can be launched directly if written in a .py file readODB.py for example, by abaqus python readODB.py

from odb2sdt import *   # import read functions

jobName='my_abaqus_job'
odb=openOdb(jobName + '.odb')
allNodal2mat(odb)

This second script will only write the DOF set in a .mat binary file

from odb2sdt import *   # import read functions

jobName='my_abaqus_job'

odb=openOdb(jobName + '.odb')       #open the database
stepName=odb.steps.keys()[0]        #get the name of the first step
fieldItem=['U']                     #I want the 'U' displacement field

# get the fieldOutputs instances list from the first frame:
fieldOutputs=odb.steps.__getitem__(stepName).getFrame(0).fieldOuputs

f=matFile(jobName + '_dof.mat')              # Initialize the file
dof2mat(f,fieldOutputs,fieldItem,stepName)   # write the DOF array to it
f.close()

Once a file_allNodal.mat file has been generated, it is possible to load the deformation structure fields using

def=abaqus('read file_allNodal.mat')

def output is here a cell array containing all def structures found in the allNodal.mat file. Only simple cases of .odb outputs are supported. The rest of the data is not automatically read, it can nevertheless be attained using

r1=sdthdf('open',file_allNodal.mat);

where r1 is a cell array containing all the fields contained in the allNodal.mat file.

odb2sdt.py reference

The following lists the main subfunctions in odb2sdt.py

The following are lower level calls, and alternative calls, with output in the workspace.

Examples

See also

FEMLink