Mechanical enables you to export specifically supported analysis data to one or more of the following file types.
Text (delimiter-separated)
Standard Tessellation Language (STL)
ANSYS Viewer File (AVZ)
Part Manager Database (.pmdb)
Refer to the topics below for the type of data you wish to export based upon the desired export file format.
General steps to export
Select an object in the tree.
Click the Worksheet to give it focus (if applicable).
Right-click the selected object in the tree or within the Tabular Data window, select , and then select a file type as required.
Specify a file name and save the file. Based on the object type, the application may automatically open Excel, assuming you have the application.
Note: You must right-mouse click the selected object in the tree to use this feature. On Windows platforms, if you have the Microsoft Office 2002 (or later) installed, you may see an option if you right-mouse click in the Worksheet. This is not the Mechanical application feature but rather an option generated by Microsoft Internet Explorer.
You can export a variety of analysis data to a tab-delimited text file. This file format enables you to view the data in a text editor as well as Microsoft Excel.
Mechanical supports exporting data from the following object types (without access to worksheet data):
| Contour Results |
| Node-Based Named Selections |
| Element-Based Named Selections |
| Imported Loads |
Data from the following additional objects can be exported but requires worksheet data to be active:
| Connections | Convergence | Geometry |
| Contact Group | Coordinate Systems | Mesh |
| Contact Initial Information | Fatigue Sensitivities | Solution |
| Contact Tool | Frequency Response | Thermal Condition |
Note: Note the following with regards to how data is presented in text file format:
Exported result values equal the values the application used to create the results contour (color) displays.
For results, the exported file provides columns of information.
The column headings in the file combine results names and result unit types.
The node ID column and, if applicable, the element ID column, are NOT necessarily sorted.
For unaveraged element- or node-based contact results or elemental-based contact result results, the element IDs in the exported file correspond to the solid elements with which the contact elements share a face.
The following objects enable you to export object information in STL file format, either as Binary (default) or ASCII. File size is the primary difference between the file formats. The binary format generates smaller files, however; it does not include information for the bodies of your model. The ASCII format preserves all body information during export. Using the Options dialog box, under the Export category, you can change the default setting for exporting in STL format.
When a model contains multiple bodies, Mechanical uses a nonstandard file format for the ASCII representation. In this case, the application separates the bodies.
Files saved in the STL format can be viewed in appropriate STL supported applications, such as SpaceClaim. Currently for the Mesh object and results-based objects, files exported in the ASCII format enable you to render individual parts of your model in SpaceClaim. Files in the binary format do not support this display capability.
The exported file is written using the CAD application's unit system.
When you select Top/Bottom as the Shell setting in the Details view for a surface body and export the result contours (such as stresses and strains), the export file contains two results for every node on a shell element. The first result is for the bottom face and the second result is for the top face.
For result contours that are scoped to more than one body, and that share nodes by more than one body, the export file will contain multiple result listings for each shared node. Furthermore, if the result type is a degree of freedom result, such as temperature and displacement results, then the result values for a given shared node are identical (and redundant). In addition, if the result type is an element nodal result, like stress or strain, then the result values for a given shared node can be different because the solver can compute different element nodal result values for a node shared by different bodies.
Mechanical enables you to export your mesh and/or a result object as an AVZ (.avz) file. The export operation creates a 3D model representation that you can display in the ANSYS Viewer (installation required). The ANSYS Viewer is a WebGL based 3D image viewer that you can use to visualize the exported mesh and results of your analysis without opening the Mechanical application. For results, you can inspect result values at specific locations by hovering the mouse over a point on your model. For result objects and as desired, you can automatically launch the ANSYS Viewer by changing the default setting under the Export preference of the dialog.
Note: Exporting results that include a customized legend may present legend/contour display inconsistencies in the viewer.
You can export the geometry (entirely or as parts) to a binary Part Manager Database (.pmdb) file by:
Right-clicking on the Geometry object and then selecting >. The application writes the entire geometry to the .pmdb file. This option also writes any Named Selections created in Mechanical into the .pmdb file.
Or...
Right-clicking one or more bodies/parts, and then select >. The application writes the selected parts to the .pmdb file. If a selected body is part of a multi-body part, then the entire part is written to the file.
Or...
Right-clicking one or more bodies in the Graphics window and then selecting >. The application writes the selected parts to the .pmdb file.
Exporting the Geometry as a .pmdb file facilitates future geometry import into SpaceClaim, DesignModeler, as well as re-importing the file back into Mechanical.
When exporting a geometry to a .pmdb file, the application exports all bodies, including suppressed bodies, to the file without maintaining their suppression status. Therefore, when you re-import the geometry, all of the bodies are unsuppressed. However, the application does export whether or not a you have hidden bodies. This means that suppressed bodies, which are typically hidden, appear hidden when you re-import the geometry. As a result, your geometry may have bodies that are hidden, because they were suppressed on export, but that are no longer suppressed.
The application does not export supplemental model data created after the geometry was imported. This includes coordinate systems, work points, spot welds, or materials that you manually added during your Mechanical session.
When defined, .pmdb files include geometry cross sections for line bodies in the exported file. Subsequent SpaceClaim and Mechanical sessions import the line body cross section data accordingly. However, DesignModeler does not support importing line body cross section data and as needed, requires you to redefine the cross sections if imported into DesignModeler.
The Export the Mechanical application settings in the Options dialog box enables you to:
| Automatically Open Excel (Yes by default) |
| Include Node Numbers (Yes by default) |
| Include Node Location (No by default) |