Use the Abaqus Scripting Interface method wrapMesh to wrap a planar orphan mesh around a cylindrical surface defined by the global Z-axis and a specified radius. The planar mesh must lie in the X–Y plane, and the modeling space of the part should be three-dimensional. If necessary, you can change the modeling space of a part by clicking mouse button 3 on the part in the Model Tree and selecting Edit from the menu that appears.

The wrapping procedure will relocate a node at point (, ) on the planar mesh to (), where is the specified radius, = , and =, as shown in Figure 64–19. A point on the planar orphan mesh located at (0, 0) is mapped to location (, 0, 0) on the cylindrical surface.

Because only part instances can be positioned and only parts can be wrapped, if you want to create an instance of an orphan mesh that is wrapped and oriented properly in the assembly, some planning is required. The following steps will help you achieve the desired goal:

If you are trying to create a full 360° wrap, discretization approximations may result in a small gap between nodes along the seam edge. You must use the merge nodes tool to stitch the seam by merging pairs of nodes into a single node; for more information, see “Merging nodes,” Section 64.5.6.

The following shows an example of using the Abaqus Scripting Interface to wrap a mesh:

model = mdb.models['Model-1']
part = model.parts['Part-1']
part.wrapMesh(radius=5.0)

You can use the command line interface to enter Abaqus Scripting Interface commands, as described in “Using the Python interpreter,” Section 4.3 of the Abaqus Scripting User's Guide.

For information on related topics, click any of the following items:

• “What can I do with the Edit Mesh toolset?,” Section 64.1

• Chapter 18, “Edit mesh commands,” of the Abaqus Scripting Reference Guide