This feature enables you to import data from a Polyflow system and apply it in a Mechanical application analysis. Temperature data can be imported into a static structural, transient structural[3] steady-state thermal, transient thermal or thermal-electric analysis.
To import data from a Polyflow system:
In the Project Schematic, right-click the Solution cell of the Polyflow system and select Transfer Data to New>
<Mechanical system>, a link is created to the Model cell of the selected Mechanical system. If you select Transfer Data to New ><Mechanical system>, this operation automatically creates a link to the Model cell of the Mechanical system. Alternatively, you can drag the Solution cell of the Polyflow system and drop it onto the Model cell of a Mechanical system to create the link.To transfer temperature data to Mechanical, drag the Solution cell of the Polyflow system and drop it onto the Setup cell of an applicable Mechanical system.
To transfer thickness data to Mechanical, drag the Solution cell of the Polyflow system and drop it onto the Model cell of an applicable Mechanical system.
If your simulation has thickness defined from a Polyflow 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 Mechanical APDL solver, the thickness value at each node must be greater than zero.
Right-click the Imported Thickness object, 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 temperature data defined from a Polyflow system, an Imported Load folder is added under the Environment folder.
Select an imported temperature load to add from the Imported Loads drop-down menu on the Environment Context tab 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.
Select appropriate options in the Details view. You can modify the mapper settings to achieve the desired mapping accuracy.
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.
Under Data View, select the desired data Identifier, for the imported load. The data identifier (File Identifier: Data Identifier) strings are specified by the upstream Polyflow system. You can also change the Analysis Time and specify Scale and Offset values for the imported loads.
Right-click in the Data View and select Add row to specify additional data for a different analysis time.
In the project tree, right-click the Imported Load object, and then click Import Load to import the load. When the load has been imported successfully, a contour plot will be displayed in the Geometry window.
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.
Change any of the columns in the Data View tab as needed:
Magnitude
Select the appropriate data identifier that represents the load values to be applied from the drop-down list.
Analysis Time
Choose the analysis time, when the load will be applied. For the Mechanical APDL solver, this must coincide with the end time of a step defined in the Analysis Settings object in the tree.
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.
To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivateat this step! See Activating and Deactivating Loads for additional rules when multiple load objects of the same type exist on common geometry selections.