Sorry, bin momentan zu faul zum Erklären. Deshalb Manualauszug:
51.2.2 Selection methods for creating or editing a display group
You can use the following selection methods to specify the items that will be contained in a display group:
To specify geometry (cells, faces, or edges), elements, or nodes by picking them directly from the viewport, select them from the Item list. (For orphan mesh elements and nodes, you must also select Pick from viewport from the Selection Method list.) ABAQUS/CAE automatically enters the pick mode, and Select items for the display group appears in the prompt area. See Chapter 6, “Selecting objects within the viewport,” for more information on picking items in the viewport.
Click Done in the prompt area when you have finished picking items in the viewport.
Click Edit selection, Add selection, or Delete selection in the dialog box to further modify your viewport selections.
To specify elements or nodes by number, select Element labels or Node labels from the Selection Method list. Select the name of the part instance to which the nodes or elements belong from the list in the Part instance field on the right side of the Create Display Group dialog box. Type into the Labels field a list of element or node numbers separated by commas or a range of numbers such as 1:4.
To specify elements in the Visualization module by type, select Element type from the Selection Method list. A list of the available element types in your model appears on the right side of the Create Display Group dialog box. Select one or more element types from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
To specify elements in the Visualization module by material or section, select Material assignment or Section assignment from the Selection Method list. A list of the available materials or sections in your model appears on the right side of the Create Display Group dialog box. Select one or more materials or sections from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
To specify geometry, element, or node sets in part- and assembly-related modules or surfaces in assembly-related modules, select Set names or Surface names from the Selection Method list. A list of the available set or surface names in your model appears on the right side of the Create Display Group dialog box. Select one or more set names from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
To specify internal (created by ABAQUS/CAE) sets in part- and assembly-related modules or internal surfaces in assembly-related modules, select Internal sets or Internal surfaces from the Item list. A list of the available set or surface names in your model appears on the right side of the Create Display Group dialog box. Select one or more set names from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
To specify element, node, surface, or internal (created by ABAQUS/CAE) sets in the Visualization module, select Element sets, Node sets, Surface sets, or Internal sets from the Selection Method list. A list of the available set names in your model appears on the right side of the Create Display Group dialog box. Select one or more set names from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
To select all items of the specified type in your model, select All elements, All nodes, or All surfaces from the Selection Method list. No further item specification is necessary.
If you selected Part instances or Display groups from the Item list, a list of the available part instances or display groups in your model appears on the right side of the Create Display Group dialog box. Select one or more part instance or display group names from this list (see “Selecting multiple items from lists and tables,” Section 3.2.11, for more information).
Note: In assembly-related modules you can also display a subset of the part instances in your model using the visibility options in the Instance tabbed page of the Assembly Display Options dialog box (see “Controlling instance visibility,” Section 50.10). Part instances that have been toggled off in the Assembly Display Options dialog box cannot be made visible using display groups.
To specify elements, nodes, or surfaces containing results within a given range of values in the Visualization module, select Result value.
The output variable to be considered is displayed at the top right side of the dialog box. To select a new result variable, click Field Output; see “Selecting the field output to display,” Section 24.3, for more information on the Field Output dialog box. Choose from the filtering methods in the Result values field.
If you select (inside) or (outside), enter values for the upper and lower bounds of the range of results in the Min value and Max value fields, respectively.
If you select , enter a value above which the results should fall in the Min value field.
If you select , enter a value below which the results should fall in the Max value field.
Every element (or node or surface) in the model is used in the filtering process, regardless of the current active display group in the model. If you choose a range of values for which no elements (or nodes or surfaces) exist, you will create an empty display group.
Note: The bounds for filtering based on element, nodal, or surface output variables are always based on the values of a variable at the nodes. Therefore, element- and surface-based output quantities are extrapolated and averaged at the nodes before comparing them against the user-defined bounds. The averaging settings in the Result Options dialog box determine how element- and surface-based variables are calculated at the nodes. For example, consider a case where elements are filtered based on Mises stress using the default averaging threshold of 75%. After extrapolation to the nodes, the values are averaged according to this threshold. This conditional averaging may result in several distinct values of Mises stress at the node based on contributions from the various elements to which the node belongs. Any element whose Mises stress contribution falls within the user-defined bounds is included in the display group.
Eine Antwort auf diesen Beitrag verfassen (mit Zitat/Zitat des Beitrags) IP
Foren auf CAD.de (alle Foren)
| 
