MET 415/425 Lecture Notes
SELECTING In the ANSYS Utility Menu
REF: Basic Analysis Procedures
Guide, Chapter 9
Lets you "activate" a portion of a model
("deactivating" the rest of the model)
Deactivated parts of a model are NOT deleted, but they are
not operated on: plotted, listed, deleted, loaded when you use "Pick All".
"Pick All" = all currently selected entities.
From the Utility Menu: Select
-> Entities ... (brings up the Select Tool)
-> Comp/Assembly ->
-> Everything
-> Everything Below ->
Select Tool
Entities: Nodes, Elements, Volumes, Areas, Lines, or
Keypoints
How to select ?
- By Num/Pick - type in the entity number or pick with the
mouse
- By Location - enter range of coordinate value in the active
CSYS
- Attached to - select by cross-ref. to other selected
entities
- By Attributes - by material ID, element type ID, real
constant ID
- By Results - select for a given range of stress, deflection,
temp.
- Exterior - select entities on the outside surface of the
model
- and others ...
Select from what ?
- From Full - ignores any previous selections
- Reselect - select from the currently active set
- Also Select - select from outside the current set, and add
to the current set
- Unselect - remove from the current set
Buttons on the select tool:
Sele All Sele None
Invert Sele Belo
OK Apply
Plot Replot
Cancel Help
|
 |
From the Utility Menu: Select -> Everything (makes the
whole model active)
From the Utility Menu: Select -> Everything Below ->
e.g., Below an area are its edge lines, corner keypoints,
as well as, any nodes and elements created in it by meshing
Selecting is used in Preprocessing to determine which
entities are operated on (i.e., Boolean operations, delete, load application, etc.)
Selecting is used in PostProcessing to evaluate error in
different materials or model thicknesses.
Error measure is correct from element-to-element when the
stiffness is constant. However, across boundaries between different material or different
thicknesses, the error estimate is incorrect (and large).
Select each material and/or different thicknesses of a
material to evaluate the mesh error.
CM, Cname,
Entity
Groups geometry items into a component.
Where Cname is: a user-specified alphanumeric name to identify this component. Cname may be up to 32 characters, beginning with a letter and containing only letters, numbers, and underscores. (not spaces)
For example:
- CM,symmetryedge,LINE !
creates a named component of selected lines
- CM,rigidpinbc,NODE
! creates a named component of selected nodes
Named components can be addressed directly by
some ANSYS commands
For example:
- DL,symmetryedge,,SYMM
- ! applies a symmetry b.c. to the component
lines of a 2D model
- NROTATE,rigidpinbc
- ! rotates the nodal csys. orientation of
the nodes in the component into the x, y, z, directions of the currently
active csys.
Named components can also be selected again
SIMPLY by using the component name.