Deformation

Physical deformations can be calculated on and inside a part or an assembly. Fixed supports prevent deformation; locations without a fixed support usually experience deformation relative to the original location. Deformations are calculated relative to the part or assembly world coordinate system.

  Component deformations (Directional Deformation)

  Deformed shape (Total Deformation vector)

The three component deformations Ux, Uy, and Uz, and the deformed shape U are available as individual results.

Scoping is also possible to both geometric entities and to underlying meshing entities (see example below). Numerical data is for deformation in the global X, Y, and Z directions. These results can be viewed with the model under wireframe display, facilitating their visibility at interior nodes.

Example: Scoping Deformation Results to Mesh Nodes

The following example illustrates how to obtain deformation results for individual nodes in a model. The nodes are specified using criteria based named selections.

  1. Create a named selection by highlighting the Model tree object and clicking the Named Selection toolbar button.

  2. Highlight the Selection object and in the Details view, set Scoping Method to Worksheet.

  3. In the Worksheet, add a row and set the following items for the row. Refer to Specifying Named Selections using Worksheet Criteria for assistance, if needed.

    • Entity Type = Mesh Node.

    • Criterion = Location X.

    • Operator = Greater Than.

    • Value = 0.1.

  4. Add a second row with Criterion = Location Y, Value = 0.2, and all remaining items set the same as the first row.

  5. Add a third row with Criterion = Location Z, Value = 0.3, and all remaining items set the same as the first row.

    The table displays as shown below

  6. Click the Generate button. The Geometry field in the Details view displays the number of nodes that meet the criteria defined in the Worksheet.

  7. After applying loads and supports to the model, add a Total Deformation result object, highlight the object, set Scoping Method to Named Selection, and set Named Selection to the Selection object defined above that includes the mesh node criteria. Before solving, annotations are displayed at each selected node as shown below.

  8. Solve the analysis. Any element containing a selected node will display a contour color at the node. If all nodes on the element are selected, the element will display contour colors on all facets. Element facets that contain unselected nodes will be transparent. An example is shown below.

    Note that all element facets are drawn, not just the facets on the surface or skin of the model.

    To possibly reduce clutter for complex models, the size of the dots representing the nodes can be changed by choosing View>Large Vertex Contours.

Working with Deformations

Deformations can be used to:


Important:  The deformation result can exhibit a node-based display limitation. If a node represents a remote point, the application does not process result data for it and as a result, Mechanical does not display result data. Deformed shapes, deformation contour colors, and deformation MIN/MAX values can differ from the displays (and listings) of Mechanical APDL commands, such as PRNSOL, PLNSOL, and MONITOR.


Velocity and Acceleration

In addition to deformation results, velocity and acceleration results are also available for Transient Structural, Harmonic Response (Full and MSUP), Rigid Dynamics, Random Vibration, and Response Spectrum analyses. Both total and directional components are available for the Transient Structural and Harmonic Response analyses but only directional components are available for Random Vibration and Response Spectrum (Total Deformation is available).

Considerations for Random Vibration

For Random Vibration analyses, only component directional deformations are available because the directional results from the solver are statistical in nature. The X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses.

Directional Deformation, Directional Velocity, and Directional Acceleration result objects in Random Vibration analyses also include the following additional items in the Details view:


Release 18.2 - © ANSYS, Inc. All rights reserved.