This section describes the steps to define Condensed Geometry objects. You should review all associated documentation so that you understand the application-driven actions that take place as well as the inherent limitations of the feature.
The operation of condensing parts in Mechanical is largely automated. For example, Mechanical provides facilities that analyze the connectivity of the bodies in the model and group them into Condensed Parts. Connections are classified as interior or exterior (interfaces).
Application
To create a Condensed Part:
From the Workbench Project Schematic, create a supported analysis system.
Select a geometry and open Mechanical
Create and define the applicable boundary conditions and connections, that is Joints, Springs, Point Mass, Remote Points, Supports and/or Contacts.
For Rigid Dynamics analyses, expand the Geometry folder and specify the desired connected parts as . These parts will be converted to Condensed Parts following the completion of the steps below.
Select the Model object and insert a object.
Note: The application automatically inserts the Expansion Settings object under the Solution folder when a object is created.
From the Condensed Geometry object, you can create your condensed parts using the context (right-click) menu option Create Automatic Condensed Parts or you can insert individual objects in to the tree.
The application provides two automatic methods for defining interfaces for a Condensed Part using the context menu options:
: This option selects the bodies and detects the interfaces and automatically creates new Condensed Part objects. For example, in Rigid Dynamics analyses, flexible bodies may be grouped into condensed parts and linked to other bodies through joints at the interfaces.
: This option automatically suggests interfaces. This is especially useful if you would like to manually select bodies.
Note:The Condensed Part object displays the number of superelement master nodes resulting from interfaces in the Details view.
The application does not consider objects imported from External Model systems for the automatic interface detection. For the imported objects that are associated with condensed parts, use the promote feature in the worksheet of the imported objects in order to be able to perform interface detection.
In order to achieve better performance, for a Motion analysis the option does not automatically add interfaces. Adding interfaces will give more accurate results but condensed part generation will be slower.
The application does not consider Shared Topology for the automatic interface detection. For Condensed Part objects with interface connections containing shared topology, manually add their interfaces using Named Selection(s).
See the object reference pages for the Condensed Geometry and Condensed Part objects for descriptions of all associated Details view properties.
Insert desired results. This feature supports Deformation, Stress, and Strain results.
Solve the analysis.
As desired, you can obtain results in the original elements within the Condensed Part by selecting the Expansion Settings object and displaying the Worksheet. From there, select the desired result for your Condensed Part(s).
It is possible to add or remove interfaces directly on the Interfaces Worksheet using its context menus. This is especially useful for specifying new remote interfaces not already automatically detected. Mechanical attempts to verify all interface selections during the Generation and Use Passes and issues a warning should any be missing. Mechanical also tracks operations that remove and suppress upstream objects affecting the interface and reacts accordingly.
Note: To delete a Condensed Geometry object, it is necessary to clean and remove any generated Condensed Parts. Similarly, to delete an Expansion Settings object, it is necessary to clean any generated data.