7.1. Abaqus2Matlab GUI

Contents

About the Abaqus2Matlab GUI

Summary of implementation steps of the Abaqus2Matlab GUI

Detailed outline of implementation steps of the Abaqus2Matlab GUI

Various additional Abaqus2Matlab GUI options

About the Abaqus2Matlab GUI

Abaqus2Matlab GUI is a complete environment that provides a simple, consistent interface which helps the user perform the analysis of an Abaqus input file as well as its postprocessing in Matlab. The Abaqus2Matlab GUI is very intuitive and allows the user to begin working without a great deal of preparation. However, it is recommended that the (new) user reads carefully the Abaqus2Matlab Analysis User's Guide first, in order to use the Abaqus2Matlab GUI in the best way.

The Abaqus2Matlab GUI can be started by simply clicking the relative icon on the APPS tab of the Matlab main window. If Abaqus2Matlab is not listed in the apps, then it is most likely that it has not been installed. You can install Abaqus2Matlab application by following the instructions described in the 8.Installation section.

Summary of implementation steps of the Abaqus2Matlab GUI

In summary, Abaqus2Matlab GUI can perform the following tasks:

[1] Install the Abaqus2Matlab library permanently.

[2] Load an Abaqus input file into Abaqus2Matlab

[3] Modify the contents of the data in the input file that are loaded in the memory.

[4] Save the modified data of the initially loaded input file into another Abaqus input file in a subfolder of the directory from which the initial input file was loaded, named A2M_GUI_Output.

[5] Generate the appropriate Matlab script which runs the Abaqus input file saved at the previous step and postprocesses the Abaqus results, according to the options specified by the user at the second step of this section.

[6] Run the generated Matlab script

Detailed outline of implementation steps of the Abaqus2Matlab GUI

Here the steps summarized in the previous section are explained in detail. In order to facilitate the user to perform operations at the Abaqus2Matlab GUI correctly, each section is followed by a representative figure showing graphically the steps described.

[1] Installing library permanently is needed in order to enable Abaqus2Matlab scripting without the need for the GUI to be opened. This updates the Matlab paths (recorded at the pathdef.m file) with the directory in which Abaqus2Matlab is installed. Go to the Tools tab, then select Install Library Permanently. A Matlab script is opened in the Matlab Editor named Abaqus2MatlabSetUp.m, and a message appears in the command window stating "Please RUN the Abaqus2MatlabSetUp.m script in order to add the Abaqus2Matlab functions to Matlab". After this, go to the Abaqus2MatlabSetUp.m file in the editor, then run it by selecting the Run button (green arrow) or pressing F5. The above steps are indicated in the following figure:

[2] The loading of an Abaqus input file in Abaqus2Matlab is described in the following:

[2.1] In order to load the contents of an Abaqus input file into Abaqus2Matlab, the user has to click the LOAD INPUT button at the upper right section of the GUI window, and in the browsing window that opens, select the Abaqus input file to be loaded, then press "Open". The Abaqus input file has the extension *.inp and is always in ASCII format. It is either created by pressing the "Write input" button at the Job manager window at the Job module of Abaqus/CAE, or manually edited by a text editor (editing the input file is recommended for users with good knowledge of the Abaqus Keywords and of how the various options are arranged in it).

[2.2] During loading of an input file in the Abaqus2Matlab GUI, extensive checks are made regarding its content. If incorrect definitions are present in the input file, then descriptive errors are issued at the Matlab command window. In case of issues that may have spurious effects on the Abaqus analysis of the loaded input file, appropriate warning messages are issued. Indicative but not exclusive checks that are performed during reading of the input file are described in the following:

[2.2.1] Not equal *PART and *END PART option specifications in the input file, or the existence of a *PART option specified after its corresponding *END PART option.

[2.2.2] Definition of a *PART option without the NAME parameter.

[2.2.3] Not equal *INSTANCE and *END INSTANCE option specifications in the input file, or the existence of a *INSTANCE option specified after its corresponding *END INSTANCE option.

[2.2.4] Definition of a *INSTANCE option in which none of the NAME or INSTANCE parameters are specified.

[2.2.5] More than one *ASSEMBLY or *END ASSEMBLY definitions, or the specification of one of them without specification of the other.

[2.2.6] No *STEP option specified in the input file.

[2.2.7] Not equal *STEP and *END STEP option specifications in the input file, or the existence of a *STEP option specified after its corresponding *END STEP option.

[2.2.8] Abaqus/Standard and Abaqus/Explicit definitions in the same Abaqus input file.

[2.2.9] Specification of the *FILE FORMAT or *FILE OUTPUT option more than once in the input file.

[2.2.10] At least one results file / output data base file output request outside a step definition.

[2.2.11] Both *FILE FORMAT and *FILE OUTPUT options specified in the same input file.

[3] In section [3.1] the information that appears on the GUI and is loaded automatically from Abaqus2Matlab is explained. The procedure for modification of the data loaded from the input file in Abaqus2Matlab by the user according to his/her needs is described in section [3.2]:

[3.1] After loading of the input file, Abaqus2Matlab determines the following:

[3.1.1] The type of analysis that is performed if the input file is run in Abaqus (Abaqus/Standard or Abaqus/Explicit).

[3.1.2] The steps that are defined in the input file. The steps are shown under the Step: drop-down list.

[3.1.3] The node sets and element sets that are defined in the input file. These sets appear in the NODE SETS and ELEMENT SETS lists respectively. Two types of node or element sets can be defined in an input file:

- Node or element sets that are defined at the part level (within *PART definitions). These are inherited by instances and are referenced at the step level (where output requests are specified) as INSTANCE_NAME.SET_NAME, where INSTANCE_NAME is the name of the instance referring to the part in which the SET_NAME is specified.

- Node or element sets that are defined directly at the instance or assembly levels and are referenced at the step level (where output requests are specified) simply with their names.

[3.1.4] The various output requests that are present in the input file. The Abaqus2Matlab GUI can be used to modify the requests pertaining to the results (fil) file according to the user's needs, in order to obtain from the input file the desired results during postprocessing after the Abaqus analysis. It is noted here that the requests associated with the field or history output written in the odb file cannot be modified by the Abaqus2Matlab GUI. If such modification is necessary, then the user has to make it by loading the input file in Abaqus/CAE and making there the appropriate changes at the Step module.

[3.2] The user has to make the following selections which pertain to the results which are to be extracted from the Abaqus analysis in the results (fil) file:

[3.2.1] Erase from the output requests that are shown in the bottom window of the GUI the ones that are not relevant to the user's needs, except for the following options:

- *FILE FORMAT

- *FILE OUTPUT

and the output requests related to the odb file.

[3.2.2] Select the step at which the specified output will be requested, by clicking on the Step: drop-down list and selecting one of the steps available in the input file.

[3.2.3] Select the desired results (fil) file output options to be printed in the new Abaqus input file as follows:

[3.2.3.1] If node-type output requests that have not already been defined in the input file are needed, then select from the NODE SETS listbox the node set for which the output is required, then select from the variable drop-down list (under the NODE SETS listbox) the required output variable identifier. For each node-type output request, press the ENTER SELECTION button to insert it into the bottom window of the GUI containing the output options which will be written into the new Abaqus input file.

[3.2.3.2] If element-type output requests that have not already been defined in the input file are needed, then select from the ELEMENT SETS listbox the element set for which the output is required, then select from the variable drop-down list (under the ELEMENT SETS listbox) the required output variable identifier. For each element-type output request, press the ENTER SELECTION button to insert it into the bottom window of the GUI containing the output options which will be written into the new Abaqus input file.

[4] At this stage the user has to check the options that appear in the bottom window of the GUI, and that are going to be printed in the new input file. After this, press the WRITE TO INPUT button to create a new Abaqus input file in which all the information from the initially loaded input file modified according to the selections made in the GUI by the user are stored. It is important to note that all previous information related to the output requests that is included in the initial input file is going to be deleted. Only the information that is in the text box at the bottom of the GUI is going to be printed in the new file. The new input file is saved in a new folder named A2M_GUI_Output which is created inside the directory from which the initial input file was loaded.

[5] Press the GENERATE POST-PROCESSING SCRIPT button to generate a Matlab script which serves for performing the Abaqus analysis of the new input file generated from the Abaqus2Matlab GUI, and for performing the required post-processing operations at the odb and/or fil files that are generated after the Abaqus analysis terminates. The generated Matlab script is saved in the same directory in which the new input file is saved. Finally, run the generated Matlab script either by pressing F5 or by pressing the Run button under the EDITOR tab of the Matlab editor in which the generated script is opened. All the files that will be generated during and after the Abaqus analysis will be placed in the A2M_GUI_Output folder.

Various additional Abaqus2Matlab GUI options

Abaqus2Matlab GUI offers a variety of tools to the user in order to be acquainted with the software and to use it more efficiently:

Viewing the open source codes included in the application: By clicking on the Tools menu, a drop down list appears which offers the options of editing the open source codes of the odb file postprocessing functions, the fil file postprocessing functions, as well as the mtx file postprocessing functions.

Opening Matlab script templates for editing and running postprocessing tasks adjusted to the user's needs. By clicking on the Tools menu and selecting Templates at the drop-down list that appears, a list of all available templates in Abaqus2Matlab application is shown. By selecting the template which relates to the desired postprocessing job, the template opens in Matlab editor for editing and/or execution.

Execution of various postprocessing examples in order for the user to comprehend the way Abaqus2Matlab works as well as its capabilities and limitations. By clicking on the Examples menu, a list of the examples available in Abaqus2Matlab appears, and by selecting one of them, the main code of the example is opened in the Matlab editor (named as Main_CODE by convention), and the folder in which the necessary files for running the examples are placed is opened.

At the Help menu, the user can open the documentation of the Abaqus2Matlab application and the license file. The documentation is available in chm (compiled html) format, as well as in pdf format. The information contained in the chm and pdf files is identical; the pdf file can be used for printing the documentation or part of it whereas the chm file can be used for easily viewing the documentation.

_________________________________________________________________________
Abaqus2Matlab - www.abaqus2matlab.com
Copyright (c) 2017 by George Papazafeiropoulos

If using this application for research or industrial purposes, please cite:
G. Papazafeiropoulos, M. Muniz-Calvente, E. Martinez-Paneda.
Abaqus2Matlab: a suitable tool for finite element post-processing.
Advances in Engineering Software. Vol 105. March 2017. Pages 9-16. (2017)
DOI:10.1016/j.advengsoft.2017.01.006



Created with an evaluation copy of HelpSmith.
To remove this notice, you should purchase the full version of the product.

We support Ukraine and condemn war. Push Russian government to act against war. Be brave, vocal and show your support to Ukraine. Follow the latest news HERE