| 1. | From the Post pull-down menu, select Free Body, then Displacements. |
The FBD Displacements tab displays in the tab area.
| 2. | Use the .op2/.odb file: field to specify the full path and filename of the results file containing the displacement output for the current model. |
| • | Clicking on the folder icon opens the standard file selection dialog window for browsing files. |
| • | Once an results file is selected, loadstep names and IDs with displacement output are saved with the rest of the HyperMesh database for use with all FBD utilities. If a new results file is required, or if the original results file changes, you must load the new results file into the database (overwriting the previously selected one). |
This lets you specify from which loadstep(s) to extract displacement information. Only loadsteps with displacement results from the currently selected results file display for selection. You can select multiple loadsteps by ctrl-clicking or shift-clicking. Filter buttons allow for additional selection control, including a name filter that uses standard HyperMesh filtering syntax. The loadstep display can be switched between ID and Name (ID).
The ID option lists the loadsteps as "SUB-CASE #". The Name (ID) option lists the loadstep as "SUBTITLE - LABEL(ID)". If no SUBTITLE exists, only the LABEL is used. See the OptiStruct online reference guide for more information regarding SUBTITLE and LABEL loadstep information cards.
The entity selection section allows you to select and/or create the appropriate entities required to execute the FBD Displacements utility. There are several options:
| • | The Element Set selector defines the elements that contain the nodes at which displacement data will be extracted. The Set Browser utility on the Tools menu can be used to create the necessary element sets. |
| • | The Node Set selector defines the nodes at which displacement data will be extracted. Only the nodes contained within the selected node set will be part of the extraction. If a node set is not selected, then all nodes within the element set are used. |
The Auto find interface nodes option automatically finds the nodes attached to elements that are not contained within the currently selected element set. This procedure selects the nodes interfacing with the remainder of the structure. You will be prompted to give the newly created node set a name. Additional nodes may be added to the node set once it is created by clicking the Node Set selector and picking additional nodes.
| • | The Show model checkbox is a graphical review option that, when checked, automatically displays the entire model in transparency mode and highlights the currently selected element and node sets. This functionality allows you to verify which element and node sets are currently selected. |
The Output options section contains various options to review and display results of FBD Displacement extractions.
| • | The Coordinate System selector determines the coordinate system used to display the nodal coordinates (x,y,z) in the summary table and .csv file output options. Displacement data (Ux, Uy,…) is always output in the system that the results are stored with in the results file format. Results coordinate system transformations are not performed on displacement data. |
The FBD Displacement utility extracts and applies the displacement and rotation results from the results file in the output coordinate system without any further coordinate system transformations. It is assumed that the output coordinate system assigned to each node in the HyperMesh database matches that used to run the analysis and generate the results file. Output coordinate systems are defined in HyperMesh by accessing the Systems panel. On the Setup menu, click Coordinate Systems, and toggle to the assign sub-panel, select the required nodes and a coordinate system, and click Set Analysis. In OptiStruct and Nastran this operation sets the CD field on the GRID card(s). See the OptiStruct online reference guide for more information regarding the GRID bulk data card. If the output coordinate systems for each node in the HyperMesh database does not match those used to run the analysis then the extracted values will be incorrect. Situations when this behavior could occur include modification of nodal output system within HyperMesh without rerunning the analysis and/or loading a results file that does not match the currently loaded model.
If a coordinate system is not specified, the HyperMesh "base" system is used by default.
| • | The Zero Tolerance entry defines the cut-off point below which a result quantity is considered zero. All calculations are done with float point precision and the zero tolerance value is only used for controlling the output of results to the various formats. The option helps to eliminate "relatively small" values from being output to the result formats. To maintain float precision the default is set to 1.0e-6, otherwise modify the value as desired. |
| • | The Create Load Collectors option will extract the specified displacement data and display it in organized load collectors within HyperMesh for graphical visualization within the model window5. A single load collector, for the current element and node set, is created for each loadstep. The load collector name format is FBDD_E(#)_N(#)_S(#)_Disp. For example, FBDD_E(1)_N(1)_S(1)_Disp would be created for element set 1, node set 1 and loadstep 1. The loads in this load collector are created with the SPC load type. This collector can be referenced as the SPC in the loadstep panel. |
The Create SPCD option will additionally create a load collector with the name "FBDD_E(#)_N(#)_S(#)_SPCD". Loads in this collector are created with the SPCD load type. This collector can be referenced as the LOAD in the loadstep panel.
The Color option allows you to choose a color for all created load collectors. This color can be modified later using either the HyperMesh interface or the FBD Results Manager utility.
| • | The Show summary table option outputs the results to a popup window for instant review. The table contains information about the loadsteps, element and node set(s), and detailed displacement data at each node. A sample window with partial output is shown below. |
| • | The Create .csv file option creates a .csv file that contains the same information as the summary table, but in a comma-separated file. You may select a new file or an existing file. If an existing file is selected there are several items to note: |
If the data you are extracting already exists in the file (based on element set, node set and loadstep IDs), the existing block will be overwritten with the new data. If it does not exist, it will be appended to the end of the file.
In any case, you will be warned that the file already exists and asked if you want to replace it. Selecting yes will not overwrite the file; it will append/replace the data.
