Context:
To verify the quality of the mesh, you can display the part in the
Mesh module
and select
from the main menu bar. In addition, you can use the
Mesh module
to change the element type assigned to the mesh and to edit the original mesh
definition. For more information, see
What can I do with the Edit Mesh toolset?,
and
Assigning Abaqus element types.
From the main menu bar, select
.
The Import Part dialog box appears.
From the File Filter menu at the bottom of the
Import Part dialog box, select Output Database
(*.odb).
Abaqus/CAE
lists all the files in the selected directory with an .odb
file extension.
Select the output database containing the part to import, and click
OK.
The Create Part from Output Database dialog box
appears. The dialog box lists each part instance in the output database along
with its type (deformable body or discrete rigid surface).
From the dialog box, select the instances to import.
If you selected only a single part instance,
Abaqus/CAE
uses the name of the instance to name the resulting part, although you can
change the name if desired. In contrast, if you selected more than one part
instance to import,
Abaqus/CAE
uses the name of each instance to name each part and you cannot change their
names.
Abaqus/CAE
determines the modeling space (three-dimensional, two-dimensional, or
axisymmetric) of the part instances. You cannot change the modeling space or
the type.
By default,
Abaqus/CAE
imports the undeformed configuration of the parts. To import the deformed
parts, click Import deformed configuration. Select the
step and frame containing the deformed shape from the available steps and
frames in the output database.
When importing deformed parts, the deformations are read from the
field output variable U, if available; otherwise, the deformations are read from the
field output variable UT.
Click OK to import the orphan mesh from the
output database and to close the dialog box.
If the name that you entered is the same as the name of an existing
part in the model,
Abaqus/CAE
asks if you want to overwrite the existing part or replace the mesh.
If you choose to replace the mesh,
Abaqus/CAE
replaces the nodes and elements of the existing part with the nodes and
elements of the imported orphan mesh. Sets and section assignments that
referred to the original part are maintained. However, because the sets and
section assignments refer to node and element numbers, the mesh of the imported
part should be similar to the mesh of the original part. For example, you could
replace the undeformed mesh with the deformed mesh.
Abaqus/CAE
enters the
Part module,
the imported part replaces the contents of the current viewport, and the part
appears in the model's list of parts in the context bar.