Abaqus2Matlab is a Matlab toolbox which is used to retrieve the results of an Abaqus analysis in an easy to handle form. It is developed by George Papazafeiropoulos (email@example.com) in an effort to facilitate the process of coupling between Abaqus and Matlab. It is written in MATLAB programming language and is available as source code distributed under a BSD-style license (see License.txt which is included in the toolbox folder).
Abaqus2Matlab is an effective tool with the following features:
2.1. It provides linking between Abaqus and Matlab. Abaqus analysis can be conducted through Matlab, without interacting with Abaqus/CAE interface, or even Abaqus/Command.
2.2. It transfers efficiently results from Abaqus to Matlab, in an error-proof way, since every contained external function is verified by its application in reading the results of a corresponding Abaqus analysis. The results of the verification of each function are presented in this toolbox in the form of html files.
2.3. It provides the requested results in a form that enables the user to easily manipulate the data for further postprocessing.
2.4. It can read 24 different kinds of nodal results (results at nodes), 35 different kinds of elemental results (results at the element integration points or results regarding whole elements) and 3 different kinds of analysis results (e.g. node definitions, element connectivity, eigenfrequencies and eigenvalues, etc.)
2.5. A complete documentation package is provided along with the source code in this toolbox.
2.6. It covers most types of Abaqus analyses and results. A sufficient number of functions is included in the toolbox to capture the most usually requested Abaqus results.
All files and folders of Abaqus2Matlab toolbox have to be setup in the current folder of Matlab, which must be the folder of the toolbox. This folder should be placed in the Abaqus working directory, although this is not mandatory. In any case, the files generated in Abaqus runs will be placed one level up (outside) from the toolbox folder.
3.1. Find the directory containing this file
S = mfilename('fullpath'); namelength=numel('Documentation'); S=S(1:end-1-namelength);
3.2. Setup all files and folders inside the directory where Abaqus2Matlab toolbox is found
addpath(genpath(S)); cd(S); savepath
The source code files and folders used in this toolbox are the following:
4.1. A function named Fil2str that converts the contents of the results file into a one-row string to be further used in Matlab. This conversion is necessary because the results file is written as a sequential file, i.e. all words in the results file are of the same length (all rows in the file have the same length). Details
4.2. A folder named OutputAnalysis which contains the functions for the processing of the analysis results (e.g. node definitions, element connectivity, eigenfrequencies and eigenvalues, etc). See Analysis result types to find which record key and which function is associated with each of the possible analysis result type and List of functions used for any file output request
4.3. A folder named OutputNodes which contains the functions for the processing of the nodal results. See Node result types to find which record key, which output variable identifier and which function is associated with each of the possible nodal result types and List of functions used for any node file output request
4.4. A folder named OutputElements which contains the functions for the processing of the element results (results at the element integration points or results regarding whole elements). See Element result types to find which record key, which output variable identifier and which function is associated with each of the possible element result types and List of functions used for any element file output request.
4.5. This script (Documentation.m).
All the functions provided with this toolbox and associated with obtaining analysis, element or node results are verified to ensure that they work correctly and they are not error-prone. In the verification process a suitable Abaqus input file, in which the option for the extraction of the desired results in an ascii results file (.fil) is specified, is run by Abaqus, after being copied from the AbaqusInputFiles folder outside the folder of this toolbox (no matter where it is placed), which must be the Abaqus working directory. After the Abaqus analysis terminates and the results file is created in the Abaqus working directory, it is processed appropriately by Matlab to obtain the requested results. Finally, the results are presented and checked with regard to their class and size. See here for a complete list of the functions verified and the verification results for each function. The verification source codes are contained in the folder named Verification.
The verification of this toolbox was made using Abaqus 6.13.
Except for the source code files and folders used in this toolbox other supplementary files and folders are provided, which are the following:
6.1. A folder named AbaqusInputFiles which contains the input files which are run by Abaqus. These Abaqus files can be run by opening Abaqus/Command and typing < < abaqus job=X > > where X is the name of the Abaqus input file without the extension (*.inp). Each Abaqus input file is named with a number, let it be Y, which is the record key of the output variable identifier. The Abaqus input file Y.inp is run by Abaqus and produces results which are obtained after Abaqus completes the analysis by the function RecY.m. The Abaqus input files can be opened in any simple text editor, to view the various options specified in them.
6.2. A folder named help which contains all the source files which are published in the documentation, and do not include any verification examples. Such source files include the record key tables, function lists, etc.
6.3. A folder named html which contains all the html files of the documentation of this toolbox, including all the html files produced by publishing the verification examples of this toolbox. All the verification examples contained in the folder Verification and the editing files of the external functions and the Abaqus input files contained in the folder help are published by Matlab in this folder and are accessible through the documentation.
Follow the instructions below to watch step by step an example verification procedure of the toolbox:
7.1. Ensure that Abaqus license server has started successfully.
7.2. Place the folder of the toolbox in the Abaqus working directory (usually C:\Temp)
7.3. Open the file named < < Documentation.m > > in Matlab and run it (press F5)
7.4. Type in the command window of Matlab the name of the file to be executed (it will be one of the verification files in the Verification folder) without its extension. The name of the file is of the form VerifyX, where X is the name of the Abaqus input file (X.inp) which is run by Abaqus to produce the corresponding results file X.fil in the Abaqus working directory. The information contained in X.fil is processed by the external Matlab function RecX.m, to give the requested output. For example by typing Verify8 in the command window of Matlab, the file 8.inp is run by Abaqus, after the analysis the file 8.fil is created in the Abaqus working directory, and the function Rec8.m obtains the requested results.
7.5. After the source code in the file VerifyX.m has run, the results of the Abaqus results file X.fil will appear in the command window. The results of the run can be viewed in the documentation which accompanies this toolbox. A complete list of the verification results for all Abaqus results postprocessing functions can be found here.
Follow the instructions below to run and use the toolbox:
8.1. Ensure that Abaqus license server has started successfully.
8.2. Place the folder of the toolbox in the Abaqus working directory (usually C:\Temp). Usually, this step is not necessary, since Abaqus can run from any directory. This action is suggested, however, to avoid confusion with the large number of files which are created in each Abaqus run.
8.3. Open the file named < < Documentation.m > > in Matlab and run it (press F5)
8.5. To extract an arbitrary Abaqus analysis result from an Abaqus results file, initially the record key and the output variable identifier have to be specified. These can be obtained from Analysis result types for an analysis-type output, Element result types for an element-type output, and from Node result types for a node-type output.
8.6. To view the instructions for use of each function, type < < doc RecX > > or < < help RecX > > (where X is the record key found in step 8.5 above) in the Matlab command window. the first option shows the function manual in a matlab browser, whereas the second option shows the function manual in the matlab command window. In the manual of each function the necessary options to be included in the Abaqus input file are shown.
8.8. Run the Abaqus input file in Abaqus, either by opening Abaqus/Command and typing < < abaqus job=X > >, then enter, or by typing in the Matlab command window < < !abaqus job=X > >, then enter. After the analysis terminates, the results file X.fil is automatically generated. This file is then read by Matlab to extract the requested results.
8.9. Place the file X.fil in the same directory with function Fil2str. Type in the Matlab command window < < Rec= Fil2str ('X.fil') > >. The variable Rec is a one-row string containing the information contained in the X.fil file.
8.10. Type in the Matlab command window < < out=RecX(Rec) > >. The variable out contains the requested results, extracted from the X.fil results file. It will be generally a double or cell array. For more information about the identity and/or physical meaning of each element contained in this array, one can refer to the manual of the function RecX.m (mentioned in section 8.6 above) or section 5.1.2 (Results file output format) of the Abaqus Analysis User's Guide
Abaqus2Matlab - www.abaqus2matlab.com Copyright (c) 2016 by George Papazafeiropoulos
If using this toolbox for research or industrial purposes, please cite: G. Papazafeiropoulos, M. Muniz-Calvente, E. Martinez-Paneda. Abaqus2Matlab: a suitable tool for finite element post-processing (submitted)