This feature enables you to import data from one or more text files and apply it in a Mechanical application analysis. Data can be imported into a static structural, transient structural 1 , steady-state thermal, transient thermal or thermal-electric analysis.
To import data from an external file:
In the Project Schematic, add any number of files to an External Data system and specify the necessary details.
When multiple files are added to the same External Data system, each file is given a unique identifier (that is, File1, File2, and so on). These identifiers are used in conjunction with the data identifiers (Pressure1, Thickness1, and so on) to identify and apply the dataset(s) within Mechanical.
If your files contain data for the same nodal coordinates, or if only one of your files contains the nodal information, you can choose the Master option in the External Data system to designate a master file. This option notifies the mapping utility that the group of files, defined in the External Data system, share the same nodal information. The nodal information is therefore processed and stored only from the master file. This greatly reduces the memory usage by only allocating space for the nodes once, not once per file. It can also result in much faster import times as only one mapping operation will be required.
Mechanical APDL .cdb files can be added as a master mesh in the External Data system; for details, see Importing a CDB File as Input in the Workbench User's Guide.
To transfer data to Mechanical, create a link between the Setup cell of the External Data system and that of an applicable downstream system.
To transfer shell thickness data to Mechanical, either:
Drag the Setup cell of the External Data and drop it onto the Model cell of a Mechanical system to create the link.
Right-click the Setup cell of the
External Data system and select
Transfer Data to New >
mechanical_system. This creates a
link to the Model cell of a new
Static Structural system
and a connection to the
Setup cell. Remove the unwanted connection
to the Setup cell.
To transfer load data to Mechanical, drag the Setup cell of the External Data system and drop it onto the Setup cell of an applicable Mechanical system.
Alternatively, you can right-click the Setup cell
of the External Data system and select
Transfer Data to New >
mechanical_system. This creates a link to the
Setup cell of a new Static
Structural system and a connection to
the Model cell. Remove the unwanted connection to
the Model cell.
When an External Data System is connected to a system using the Samcef or ABAQUS solver, the following quantities cannot be used: Body Force Density, Stress, Strain, Heat Flux, and the Emag Condition.
When an External Data System is connected to a system using the ABAQUS solver, the ABAQUS system does not support the import of Forces.
Attach geometry to the analysis system, and then double-click Setup to open the Mechanical window.
If your simulation has a shell thickness defined from an External Data system, an Imported Thickness folder is added under the Geometry folder.
Select appropriate geometry in the Details view, and then click .
Select appropriate options in the Details view. You can modify the mapping settings to achieve the desired mapping accuracy.
You can specify a thickness value for the unmapped target nodes using the Unmapped Data Value property. By default, a zero thickness value is assigned to the unmapped nodes.
Important: For the ANSYS solver, the thickness value at each node must be greater than zero.
Right-click the Imported Thickness, and then click Import Thickness to import the thickness. When the thickness has been imported successfully, a contour plot will be displayed in the Geometry window and any mesh display will be based upon the mapped thickness of the elements.
If your simulation has load data defined from an External data system, an Imported Load folder is added under the Environment folder.
To add an imported load, click the Imported Load folder to make the Environment toolbar available, or right-click the Imported Load folder and select the appropriate load from the context menu.
Select appropriate geometry in the Details view, and then click Apply.
In a 3D structural analysis, if the Imported Body Temperature load is scoped to one or more surface bodies, the Shell Face option in the details view enables you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information.
When mapping data to surface bodies, you can control the effective offset and thickness value at each target node, and consequently the location used during mapping, by using the Shell Thickness Factor property.
By default, the thickness value at each target node is ignored when data is mapped.
You can choose to enter a positive or negative value for the Shell Thickness Factor. This value is multiplied by each target node’s physical thickness and is used along with the node’s offset to determine the top and bottom location of each target node. A positive value for the Shell Thickness Factor uses the top location of each node during mapping, while a negative value uses the bottom location of each node. For example:
A value of 0.0 means that the physical thickness and offset of the surface body nodes will be ignored; all target nodes are mapped at default surface body locations.

A value of 1.0 means that the thickness used for a target node will be equal to the physical thickness value specified for that node. The top location of the node will be used during the mapping process.

A value of -2.0 means that the thickness used for a target node will be equal to twice the physical thickness value specified for that node. The bottom location of the node will be used during the mapping process.

The Viewer will look similar to the following for a value of –1.0. The colored dots represent the location and corresponding values of the source nodes. In this case, each target node will be projected using its physical thickness value to its bottom location and then mapped.

Select appropriate options in the Details view. You can modify the mapper settings to achieve the desired mapping accuracy. Mapping can be validated by using Mapping Validation the objects.
For pressure loads, you can apply the load in the direction normal to the face or by specifying a direction. Setting Define By to Components enables you to define the direction by specifying the x, y, and z magnitude components of the load. The z component is not applicable for 2-D analyses. For pressure loads in Harmonic Response, you can apply both real and imaginary components of the loads.
In a 3D analysis, if the Triangulation mapping algorithm is used, the Transfer Type mapping option defaults to Surface when an Imported Temperature or Imported Body Temperature load scoping is only on shell bodies. If the scoping is on shell bodies and other geometry types, the Transfer Type mapping option will default to Volumetric. In such cases, to obtain a more accurate mapping, you should create a separate imported load for geometry selections on shell bodies, and use the Surface option for Transfer Type. See Transfer Type under Mapping Settings for additional information.
For Imported Pressure loads, you can apply the load onto centroids or corner nodes using the Applied to property in the Details view. See Imported Pressure for additional information.
For imported force loads, both conservative and profile preserving algorithms are available using the Mapping property. See Imported Force and Mapping Settings for additional information.
For each load step, if an Imported Displacement and other support/displacement constraints are applied on common geometry selections, you can choose to override the specified constraints by using the Override Constraints option in the details of the Imported Displacement object. By default, the specified constraints are respected and imported displacements are applied only to the free degrees of freedom of a node.
For Vector 2 and Tensor 3 loads, the Coordinate System property can be used to associate the component identifiers, defined in the worksheet, to a particular coordinate system. This option is useful when the source data is defined, or needs to be defined, with respect to a coordinate system that is not aligned with the Global coordinate system. If a cylindrical coordinate system is chosen, the data is interpreted to be in the radial, tangential, and axial directions. By default, the Source coordinate system is used.
Note: The Source Coordinate System drop-down option is an internal coordinate system used by Mechanical and is not visible in the tree. It represents the coordinate system that was used to define source points in the upstream External Data system. If there are no Rigid Transformations (Theta XY/YZ/ZX) defined in the upstream External Data system, the Source Coordinate System is the same as the Global Coordinate System.
Under Data View, select the desired data Identifier, for the imported load. The data identifier (File Identifier: Data Identifier) strings are specified in the upstream External Data system. You can also change the Analysis Time/Frequency and specify Scale and Offset values for the imported loads.

For Vector 2 and Tensor 3 loads, if the Define By property is set to Components you should select data identifiers that represent the x/radial, y/tangential, and z/axial magnitude components of the load. For Vector 2 and Tensor 3 , the components are applied in the Coordinate System specified in the Details view. The z component is not applicable for 2-D analyses. For Imported Displacement load, you can choose to keep a component free, or fixed (displacement = 0.0) by selecting the Free or Fixed option from the list of data identifiers. For all other loads, you can choose to ignore a component if you do not have data for that direction by selecting the Ignore identifier from the drop-down list.
For Imported Pressure/Imported Velocity in Harmonic response, you should select data identifiers for both real and imaginary components. You can also specify Scale and Offset for both real and imaginary components.

For Imported Convections, you should select data identifiers for film coefficient and ambient temperature. You can also specify Scale and Offset values for both film coefficient and ambient temperature.

Right-click in the Data View and select Add row to specify additional data for a different analysis time/frequency.
Change any of the columns in the Data View tab as needed:
Magnitude \ Film Coefficient \ Ambient Temperature
Select the appropriate data identifier that represents the load values to be applied from the drop-down list.
X Component
Select the appropriate data identifier that represents the x component of the load values to be applied from the drop-down list.
Y Component
Select the appropriate data identifier that represents the y component of the load values to be applied from the drop-down list.
Z Component
Select the appropriate data identifier that represents the z component of the load values to be applied from the drop-down list.
Note: If you do not have data for a direction you can choose to ignore that component by selecting Ignore from the appropriate drop-down box. Select the Fixed option from the drop-down list to make the component constant with a value of zero or the Free option for the component to be without any constraints.
If multiple files have been used in the upstream External Data system, the data identifiers for component-based vector or convection loads must come from the same file or from files that have a master file association. For example, you can select File1:PressureX, File1:PressureY, and File1:PressureZ, but you cannot select File1:PressureX, File2:PressureY, File3.PressureZ (assuming that File1, File2, and File3 do not have a master file association).
XX, YY, ZZ, XY, YZ, and ZX Component
Select the appropriate data identifiers to represent the components of the symmetric tensor to be applied from the drop-down list.
Analysis Time/Frequency
Choose the analysis time at which the load will be applied.
Scale
The amount by which the imported load values are scaled before applying them.
Offset
An offset that is added to the imported load values before applying them.
In the project tree, right-click the Imported Load, and then click Import Load to import the load.
When the load has been imported successfully, a contour or vector plot will be displayed in the Geometry window.
For Vector 2 loads, contours plots of the magnitude (Total) or X/Y/Z component can be viewed by changing the Data option in the details pane. Defaults to a vector plot (All).
For Tensor 3 loads, contours plots of the Equivalent (von-Mises) or XX, YY, ZZ, XY, YZ and ZX components can be viewed by changing the Data option in the details pane. Defaults to a Vector Principal plot.
For Imported Convections loads, contours plots of film coefficient or ambient temperature can be viewed by changing the Data option in the details pane.
For complex load types, e.g. Pressure/Velocity in Harmonic Response, the real/imaginary component of the data can be viewed by changing the Complex Data Component option in the details pane.
Note: The range of data displayed in the graphics window can be controlled using the Legend controls options. See Imported Boundary Conditions for additional information.
If multiple rows are defined in the Data View, imported values at different time steps can be displayed by changing the Active Row option in the details pane.
To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivate at this step! See Activation/Deactivation of Loads for additional rules when multiple load objects of the same type exist on common geometry selections.
For Vector 2 and Tensor 3 loads, when the Define By property is set to Components, any rotation transformations (Theta XY/YZ/ZX) specified in the External Data system will be appropriately applied to the mapped data if the Coordinate System is specified as Source Coordinate System. If any other coordinate system is specified then the components are applied in the specified Coordinate System. Rotations, resulting from using a cylindrical projection coordinate system, for 2D to 3D mapping are also appropriately applied to the mapped data. Rotations, resulting from analytical transformations specified in the External Data system, do not get applied to the mapped data.
For Imported Displacements, selecting the Free identifier for a source component will result in the corresponding target component being left unconstrained and free to deform in that direction, whereas Fixed identifier results in a value of zero being applied. For other load types, a value of zero is applied on selecting the Ignore component.
1 - The rigid dynamics solver is not supported.
2 - Imported Displacement, Imported Force, Imported Pressure and Imported Velocity.