WIXLIB

Figure 2-7 fe-safe Result Contours2.3How to use the fe-safe extension2.3.1Specify the modelThe first step in setting up an fe-safe system is to specify an FEA solution file to base its analysis upon.Connect the fe-safe system downstream of a Model cell in another system. This will mean you will need tomake sure that the Solution cell is updated before performing the connection (since the FEA solution file willnot exist until the cell is up-to-date.)Pre-scanning of the FEA solution is not supported when using Workbench (see Limitations in section 0below). However, many settings regarding which FEA solution variables and other data are read can be madein the Analysis Settings item in the ANSYS Mechanical project tree. See section 0. Datasets are loaded for allextension workflows using full read settings configured in the Details of “Analysis Settings” panel (see moreabout selecting datasets to read in section 3.2).Note: On subsequent executions of the schematic, upstream systems will likely update the FEA solution file. If an fe-safesystem is connected to one of those upstream systems, it will refresh its datasets from the most recent FEA solution filethat was passed from upstream. It does not matter if the filename or location is different, the system will respect whateversolution file was most recently supplied. The caveat to this is that users must be sure that upstream systems will notchange the solution file in a way that will invalidate the fe-safe project you set up. (For example, if the number of steps ormaterial assignments are changed , or if a geometry selection is invalidated). If you think that an fe-safe project setup mayCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench9

have been “invalidated” by upstream changes, you should right-click the Project cell and select Reset to clear the projectconfiguration.2.3.2Configure the projectThis is a description of a basic workflow for the fe-safe extension.Right-click the Setup cell and select Edit to start setting up an fe-safe project. The Mechanical window willappear with the fe-safe system in the outline. The properties can be set up in any order.Project SetupFigure 2-8 fe-safe Basic Project SetupThe settings in the ANSYS Mechanical Details of “Project Setup” panel are provided to accelerateconfiguration of basic workflows that use simple load cases, and to tell fe-safe which regions of the model toanalyse. More details on each property can be found in section 3.3below.The only required property (highlighted in yellow) is the Fatigue Analysis Scope (for details, see section 3.3).All other properties are set to appropriate defaults.The default fatigue loading will create a single elastic-block (1 repeat) with a sequence of FEA solutions(dataset sequence) formed from all of the steps in the upstream system.Anything configured within this panel can be overridden in the Advanced Setup mode. If these properties donot give enough fine-grained control over a particular fatigue configuration, then Advanced Setup modeshould be selected by right-clicking on Project Setup in the outline.10fe-safe extension for ANSYS WorkbenchCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016

Advanced SetupFigure 2-9 fe-safe Advanced Project SetupThis mode is for any workflows that are not covered by the simplified controls in ANSYS Mechanical. WhenAdvanced Setup is first used, fe-safe will respect any settings that were configured in ANSYS Mechanical tosetup the fe-safe project. Subsequent changes whilst in component mode will take precedence when theanalysis is run.Selecting the Advanced Setup menu item opens the fe-safe GUI in a “component mode” and starts to openthe solution (e.g. file.rst) in fe-safe component mode. This is a special mode used for controlling the inputand output of files for fe-safe, from an external software component. The controls for Source and Resultsfiles/paths, and project directory that users expect to be able to set in a standalone version of fe-safe are notaccessible from the component, but instead are set by the configurations made in Workbench.Whilst in component mode, the workflow is mostly identical to the workflow in the standalone fe-safe product.Any kind of loading can be configured, the analysis groups can be configured individually, and any extraoutput contours that are enabled will be available to plot in ANSYS Mechanical.When the configuration is finished, close the fe-safe component mode GUI and return to ANSYS Mechanical.Notice that the properties are now read-only:Figure 2-10 Disabled PropertiesCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench11

This is to indicate that Advanced Setup now has control over the settings, However, these controls can beunlocked via the Unlock Properties menu item:Figure 2-11 Unlocking PropertiesBe aware that any further changes within these properties can potentially reset configuration in the AdvancedSetup. It is not a problem to change the scope of the analysis within ANSYS Mechanical from one namedselection to another; the effect will be that the now-redundant analysis group will be moved to the list ofUnused Groups in fe-safe.ExecutionTo run the fe-safe analysis, simply solve the schematic or the individual fe-safe system as shown in Figure2-12 (if in the Workbench GUI). From the ANSYS Mechanical window, use the Solve () action on theoutline for the fe-safe Solution cell.Figure 2-12 Update the ProjectAfter execution, the results contours will be available to plot under the Solution item in the fe-safe system inANSYS Mechanical. If results are missing, right-click on Solution to select the Worksheet: Result Summaryoption:12fe-safe extension for ANSYS WorkbenchCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016

Figure 2-13 Results SummaryAll of the result contours that were found in the fe-safe results file (*.FER) file should be listed under ListAvailable Solution Quantities.Figure 2-14 ANSYS Solution QuantitiesTo plot any of these results, right-click and choose Create User Defined Result.Figure 2-15 Creating a viewable resultThese results should now appear under the Solution item and can be evaluated like any other ANSYSMechanical result.2.3.3ParameterisationParameterisation is not supported in the current release of the fe-safe extension.Copyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench13

2.3.4File ManagementThe fe-safe project directory can be set manually when starting a regular instance of fe-safe. When using thefe-safe extension for the Workbench environment, this directory resides in the project directory for the sameWorkbench project, alongside the other systems. These fe-safe working files in the project directory will besaved when the Workbench project is saved or archived (and reloaded when the schematic is loaded). Thedirectory structure logic is identical to other ANSYS Workbench systems with respect to design points. Thenaming convention for fe-safe files within the working directory is for an “SYS” prefix, possibly followed by “-1”,“-2” etc depending on how many instances of the fe-safe system were dropped into the schematic.Identifying the fe-safe working files and their location (if required) in the Workbench project directory can beaccomplished by selecting the View Files menu selection from the Workbench interface as shown below inFigure 2-16.Figure 2-16 Files Table14fe-safe extension for ANSYS WorkbenchCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016

2.3.5Resetting the cellIf required, you can reset the fe-safe project to its initial state using the Reset Project menu item. This deletesthe underlying fe-safe project directory, forcing fe-safe to create a new project and re-read the FEA solutionfrom scratch.Figure 2-17 Resetting the project2.3.6LimitationsPre-scanning of the FEA solution is not supported when using Workbench, as fe-safe has no way at presentto replay the pre-scan choices when the solution is refreshed by subsequent runs. The steps in the FEAsolution are loaded in full every time it is updated by Workbench.PSD-based loading from Harmonic Analyses are not possible at the current release.Nodal groups are not supported and fe-safe only reads the element-nodal (corner) data from the FEAsolution.Plug-in modules (fe-safe/Rubber, or user-defined plugin algorithms defined using Custom Module Frameworkor CMF for fe-safe cannot be used at this release.The Engineering Data cell provides its material data as a MatML file (an XML extension designed to supportstandardised material data). Presently fe-safe has no interpreter for MatML so cannot receive its material datafrom this cell, although in this release there is an option for matching material names with a fe-safe materialdatabase file.At this release, fe-safe does not support concurrent execution. Measures have been put in place to stop fe-safe being invoked concurrently within a Workbench schematic; however you should take care not to design aschematic where this could occur.Copyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench15

16fe-safe extension for ANSYS WorkbenchCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016

3Interface ReferenceNote that only those interface elements of particular importance for using fe-safe with Workbench aredescribed here.3.1fe-safe client application GUI vs component GUIWhen Advanced Setup is selected, fe-safe opens up in component mode. The look of this is essentiallyidentical to standalone fe-safe, with some minor differences. These are shown in Figure 3-1.Figure 3-1fe-safe stand-alone GUI (left) and Workbench component GUI (right)The differences are mostly located in the Fatigue from FEA window. In component mode, the buttons forchoosing the source file and output file have been removed (they have been moved to the Workbench projectschematic). Also, the Analyse! button has been removed, since the purpose of the Workbench extension is torun fe-safe from inside the Workbench project environment.3.2fe-safe Model Reading propertiesAs noted in 2.3.1 above, pre-scanning is not available in the component mode, and the default full readsettings for Ansys RST files in fe-safe can be configured using the Details of “Analysis Settings” panelaccessible from of the fe-safe Analysis Settings in Mechanical. These settings are used to control what modeldata and FEA solutions from the RST/RTH file are read by fe-safe as shown below:Figure 3-2 RST full read optionsCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench17

Checkboxes corresponding to Read Geometry and Detect Surface are enabled by default to complete surfacedetection in fe-safe as described in the fe-safe user guide. If you are using a 3D shell model, this is notnecessary but not detrimental either.FEA solutions of elemental-nodal strain, force, and temperature can be added to the Dataset Read Options byengaging checkboxes for those options, and subsequently used in the fe-safe extension. Stress is read bydefault since most FEA Fatigue analysis are based on elastic material with plasticity correction during theanalysis process in fe-safe.Note that it is the responsibility of the engineer to read strains only when elastic-plastic material propertieshave been applied to the body selected for FEA Fatigue analysis in fe-safe. Similarly, forces are only requiredin the case of welded joint fatigue using Verity in fe-safe (loading them is not detrimental to analysis).Temperatures will only have an impact if a material with temperature variability is selected for FEA Fatigueanalysis (loading them is not detrimental to analysis). As with all FEA interfacing, loading unnecessarydatasets may take more time.3.3fe-safe Project Setup propertiesThe properties below are configured as part of the Details of “Analysis Settings” panel in the Mechanicalwindow.3.3.1Material PropertiesAt the present release, the materials supplied by default with ANSYS Engineering Data do not have all thematerial properties that fe-safe requires for a fatigue analysis. Conversely the material databases that aresupplied with fe-safe are not compatible with ANSYS. Accordingly, for fe-safe to find the material data itneeds, a material database file (*.dbase) must be the source of the data. There are two methods availablewith the fe-safe extension for specifying the material data:Figure 3-3 Comparison of Material Properties defined with Advanced Setup (above)versus Match with Engineering data (below)18fe-safe extension for ANSYS WorkbenchCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016

Define within fe-safe Advanced SetupThis is the default option. It requires that the Advanced Setup mode be used to open up the fe-safe GUI andassign materials to analysis groups, as in a normal fe-safe workflow. Any .dbase file that is opened in fe-safecan be used; if this step is omitted then fe-safe will report an error to the Workbench log when the system issolved.Match with Engineering DataWith this option, fe-safe will attempt to match the materials from Engineering Data to a given fe-safe materialsdatabase, based on the material name.The fe-safe material *.dbase file must be specified in the Material Database Location field (this is a filebrowser field).fe-safe will look at each body in the model to discover which material has been assigned:Figure 3-4 Determining the material for a given bodyCopyright 2016 Dassault Systemes Simulia Corp.Issue: 4.0 Date: 31/08/2016fe-safe extension for ANSYS Workbench19

In this case, “Structural Steel” is associated with the body “Solid 1”. Then when the analysis groups arecreated, fe-safe will expect to find a “Structural Steel” material in the database (the name match is casesensitive and punctuation-sensitive), and it will assign fatigue properties with the same name to the group infe-safe created for that body. If the fatigue analysis is based on named selections, fe-safe will create ananalysis group for each named selection and apply the material associated with that named selections. If anamed selection spans several materials, analysis groups will be created for each.To use this approach effectively, a *.dbase file must be maintained with materials that match those availablein Engineering Data. It is only recommended for organisations with a standardised library of materials.3.3.2Fatigue Analysis ScopeThis is where the scope of the analysis can be restricted to regions of the model. Under Scoping Method thereare three options:Geometry SelectionFigure 3-5 Scoping a fatigue analysis to GeometryWith this mode, either bodies or faces can be selected. fe-safe will create an analysis group for the chosenentity. Click on the yellow field, use the body/element pickers in ANSYS Mechanical to choose the entity, thenclick Apply.Named SelectionFigure 3-6 Scoping a fatigue analysis to a Named SelectionWith this mode, either bodies or faces can be selected. fe-safe will create an analysis group for the chosennamed selection. The drop-down box displays any

Experienced users of ANSYS Workbench new to the fe-safe extension for ANSYS Workbench Read Chapter 4, Chapter 2, then work through the tutorial to familiarise yourself with the fe-safe extension for ANSYS Workbench. Once you have done this, follow the procedure described in Chapter 2 with your own data, referring to Chapter 0 as necessary.