Exporting ANSYS data

You can use options in the Export Simulation dialog box to control how the software writes out the ANSYS .inp file from your data.

Model Orientation

You can use the Model Orientation options to export the model in a coordinate system that is different from the one used in the original Simulation file. This allows you to re-orient the model on export to a specified coordinate system.

You can export the model:

• In the Absolute coordinate system.

• In an existing coordinate system under the CSYS node in the Simulation Navigator.

When you export the model, the software transforms both the model’s origin and orientation. It transforms all objects in the model to the new coordinate system, including the location of nodes, loads, boundary conditions, and material orientation vectors.

For ANSYS models, the software transforms the model to the new coordinate system by adding the coordinate system that you specify using the Model Orientation option, to the top of the coordinate system hierarchy.

For example, consider an ANSYS FEM file that has three coordinate systems defined, all at the same level in the coordinate system hierarchy.

If you select Absolute from the Use Coordinate System list, the software uses the LOCAL command to write out the data for csys1, csys2, and csys3 when you export the model:

If you select csys3 from the Use Coordinate System list, the software uses the LOCAL command to write out the data for csys3. It uses the CLOCAL command to write out the data for csys1 and csys2:

If you later reimport this ANSYS input file:

• The coordinate systems are re-numbered. In ANSYS, coordinate system ID values of 1-10 are reserved for internal use. Therefore, on export, this software adds an offset value of 10 to all coordinate system IDs that have a value of 10 or less.

• csys3 is renumbered as csys13 and becomes the parent coordinate system of csys1 and csys2 which are renumbered as csys11 and csys12.

Model orientation details

When you use the Model Orientation option to transform your model:

• Node coordinates refer to the selected coordinate system instead of the absolute coordinate system. In ANSYS, the NBLOCK command does not support reference coordinate systems. Therefore, this software writes out the nodes using the N command, regardless of the options you selected in the Formatting Options group in the Export Simulation dialog box.

• The software modifies material coordinate systems to refer to the selected coordinate system, unless the material coordinate system is a parent coordinate system in the hierarchy. In this case, the software modifies the material coordinate system to refer to the absolute coordinate system.

• The software modifies nodes that do not have an assigned displacement coordinate system to refer to the selected coordinate system as their displacement coordinate system. It adds the ANSYS NROTAT,ALL command in the input file before other NROTAT commands that are specific to each node. The NROTAT,ALL command resolves the orientation for many loads and boundary conditions, including applied forces.Note: Pressure loads that are created using the Components or Components-Spatial option do not use nodal displacement coordinate systems for orientation. Instead, the software creates a material orientation vector on export to orient them. Because material orientation vectors refer to the selected coordinate system, no change occurs with the Model Orientation option as the actual orientation is correct.

• The Acceleration and Gravity commands do not use coordinate systems that refer to nodes. Therefore, the software transforms their X, Y, and Z components to the selected coordinate system.

Current limitations

• For axisymmetric models, the software does not validate whether the coordinate system you select using the Model Orientation option is correct. You must ensure that the parent coordinate system is in-plane. For example, if you selected csys3 from the Use Coordinate System list, you must ensure that the Z-axis of csys3 is parallel to the Z-axis of the absolute coordinate system.

• If your FEM file contains a coordinate system hierarchy, the coordinate system you select from the Use Coordinate System list must be at the top level of that hierarchy. That is, it must be the parent coordinate system. If the user-defined CSYS is a child, the exporter will write it out as the parent. This data altering may lead to incorrect orientation.

• In general, you should not use a nodal reference coordinate system to re-orient your model on export. This can lead to issues, if that reference coordinate system becomes a child of a user-defined coordinate system.Note: Although this software allows a model to have multiple nodal reference coordinate systems, ANSYS only allows one nodal reference coordinate system for the entire model.

Exporting selected data

You can use both the Subset Export and the Output Options to control the precise data that this software writes out to the ANSYS .inp file.

• Use the Subset Export option to control whether you export your entire model, or just portions of it. For example, you can select the Selected groups option to export only the contents of specific groups.

• Use the Output Options to control which types of ANSYS commands to export.

Where do I find it?

Application	Pre/Post
Menu	File→Export→Simulation

Learn more

Importing ANSYS structural and thermal elements

Mesh validity checking during import (ANSYS)

Look up more details

ANSYS file formats supported for import

ANSYS commands supported for import and export

Working with ANSYS compressed results files

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Exporting ANSYS data, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });