By linking ANSYS Workbench systems with Mechanical analysis systems, you can import results from one analysis and apply them as boundary conditions in a downstream (target) system.
For example, Mechanical enables you to import data from:
Mechanical analysis systems as Imported Loads or through Submodeling.
External Data systems as Imported Loads .
Fluent CFD analyses using the System Coupling feature.
HFSS, Maxwell, or Q3D Extractor applications as Imported Loads .
Additional information on Thermal-Stress, Fluid-Structure Interaction (FSI), Ansoft - Mechanical Data Transfer, Icepak to Mechanical Data Transfer, Submodeling, and External Data Import can be found in the Special Analysis Topics section.
Note: Convergence is not supported for environments with imported loads.
This section outlines the systems that you can link for importing boundary conditions as well as the supported boundary conditions, and it presents the steps to import and apply imported boundary conditions. Select a link below to navigate to a desired topic.
Note: You can work with imported loads only when you perform an analysis with data transfer.
The following table lists the systems that interact with one another using data transfer. The associated imported boundary conditions (as a data type) are show in parenthesis.
| Source Analysis/System (Transfer Data Type) | Target Analysis |
|---|---|
| CFD (Convection) | Steady State Thermal, Transient Thermal, Thermal-Electric |
| CFD (Pressure) | Static Structural, Transient Structural 1 |
| CFD (Temperature) | Steady State Thermal, Transient Thermal, Thermal-Electric, Static Structural, Transient Structural 1 |
| System Coupling (Heat Flow, Convection, Temperature) | Steady State Thermal |
| Electric (Joule Heat) | Steady State Thermal, Transient Thermal |
| Electromagnetic (Force Density) | Static Structural, Transient Structural 1 |
| Electromagnetic (Power Loss Density) | Steady State Thermal, Transient Thermal |
| Electromagnetic (Force and Moment) | Harmonic Response 2 |
| External Files (Displacement, Force, Temperature, Stress, Strain, Body Force Density) | Static Structural, Transient Structural 1 |
| External Files (Temperature, Convection, Heat Flux, Heat Generation) | Steady State Thermal, Transient Thermal, Thermal-Electric |
| External Files (Pressure) | Static Structural, Transient Structural 1 , Harmonic Response |
| External Files (Velocity) | Acoustic Analysis 3 |
| Harmonic Response (Velocity) | Acoustic Analysis 3 |
| Polyflow (Temperature) | Steady State Thermal, Transient Thermal, Thermal-Electric, Static Structural, Transient Structural 1 |
| Static Structural, Transient Structural (Displacement, Temperature, Force 4 , and Moment 4 ) | Static Structural, Transient Structural 1 |
| Steady-State Thermal, Transient Thermal (Temperature) | Static Structural, Transient Structural 1 , Electric |
| Thermal-Electric (Temperature) | Static Structural, Transient Structural 1 |
1: Rigid dynamics solver is not supported.
2: See the Importing Data into a Harmonic Analysis section for the specific steps to perform the analysis.
3: An acoustic analysis is performed via ACT. For information on creating optimization extensions, see the ANSYS ACT Developer's Guide.
4: Supported for Beam to Shell or Solid submodeling only.
Mechanical supports the boundary conditions listed below. The availability of a boundary condition in an analysis is dependent upon the types of systems that you have joined.
To import loads for an analysis:
On the Workbench Project page, add the desired analysis that supports data transfer. Link the Solution cell of the upstream onto the Setup cell of the downstream system. As required, you can also link the Engineering Data and Geometry cells between the systems.

As needed, attach geometry to the downstream analysis system and then double-click Setup to open the Mechanical window. An Imported Load folder is added under the environment folder, by default.
To add an imported load, click the Imported Load folder to make the Environment toolbar available or right-click the folder and select the appropriate load from the context menu.
Note: An Imported Load can also be created from duplicating an existing imported load. Perform a right-click an Imported Load to display the context menu, select duplicate to add an identical Imported Load to your model.
On the Environment toolbar, click Imported Loads, and then select an appropriate load.
Select the appropriate geometry, using the geometry selection or geometry-based Named Selection option and then click .
The following Imported Loads can also be scoped to node-based Named Selections.
Imported Body Temperatures (from External Data, for Submodeling [ not supported], or for Thermal-Stress)
Imported Displacements (from External Data or for Submodeling)
Imported Forces (from External Data)
Imported Temperatures (from External Data or for Submodeling)
Imported Velocities (from External Data)
Imported Initial Stress and Imported Initial Strain (from External Data), when the Apply To property is set to Corner Nodes
Set the appropriate options in the Details view.
The Data View can be used to control the load data that is imported. Each data transfer incorporates some or all of the column types shown below.

Source Time/Frequency: Time at which the load will be imported.
Source Time Step: Time Step at which the load will be imported.
Analysis Time/Frequency: Time at which the load will be applied when the analysis is solved.
Scale: The amount by which the imported load values are scaled before they are sent to the solver. The scale value is applied to the imported load values in the solver unit system.
For Imported Temperature and Imported Body Temperature loads:
The values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value.
Offset: An offset that is added to the imported load values before they are sent to the solver. The offset value is applied to the imported load values in the solver unit system.
Specific transfer details can be found in the Special Analysis Topics section.
If you are using the ANSYS solver, loads can be applied using tables, or can be applied at each analysis time/frequency specified in the imported load using the Tabular Loading property. When sending as tables, the loads can either be ramped or step changed (stepped) between the specified Analysis Times/Frequencies.
When ramped, the load value at step/sub-step is calculated using linear interpolation in the range where solve step/sub-step falls.
When stepped, the load value specified at t2 is applied in the range (t1, t2], where (t1, t2] is the range greater than t1 and less than or equal to t2.
When program controlled, the loads are sent as tables when Analysis Time(s)/Frequency(ies) not matching any step end times/maximum frequency are present in the load definition. The loads are ramped for static/steady state and harmonic analyses and step applied for transient analyses.
The loads are always sent as tables when Ramped or Stepped is chosen.
Important: Note that these options do not change the KBC command value (Key) which controls whether all of the loads within a load step are linearly interpolated or step changed. In addition, certain limitations apply to loads that do not support tabular loading, such as Imported Body Force Density. The limitations are described on the Help page for the respective loads.
Extrapolation is not performed when stepping/ramping the loads. If the solve time for a step/sub-step falls outside the specified Analysis Time/Frequency, then the load value at the nearest specified analysis time is used.
For temperature loads, the values are ramped from reference temperature for the first time step. For all other loads, the values are ramped from zero.
User can choose not to send the loads as tables using the Off option. The analysis times/frequencies specified in the load definition must match the step end times/maximum frequency in this case for the solution to succeed.
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 loads types, 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 loads types, contours plots of Equivalent (von-Mises) or XX/YY/ZZ/XY/YZ/ZX component can be viewed by changing the Data option in the details pane. Defaults to a Vector Principal plot (All).
For Imported Convection 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.
The Legend controls options allow the user to control the range of data displayed in the graphics window. By default, it is set to Program control, which allows for complete data to be displayed. If you are interested in a particular range of data, you can select the Manual option, and then set the minimum/maximum for the range.
When you scope imported loading conditions to elements, you may see graphic artifacts on your model in the form of color "bleeding". Selecting Wireframe mode corrects the display.
The isoline option is drawn based on nodal values. When drawing isolines for imported loads that store element values (Imported Body Force Density, Imported Convection, Imported Heat Generation, Imported Heat Flux, Imported Pressure, Imported Surface Force Density, Imported Initial Stress and Imported Initial Strain), the program automatically calculates nodal values by averaging values of the elements to which a node is attached.
The minimum and maximum values of source data are also available in Legend Controls for External Data Import, Thermal-Stress, Submodeling, and Acoustic Coupling analyses.
To preview the imported load contour that applies to a given row in the Data View, use the Active Row option in the Details view.
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.
To export data, select the Imported Load object, right-click the mouse, and then select .