Wrapping a mesh about the Z-axis

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.

Related Topics
What can I do with the Edit Mesh toolset?
Will link to ker-obj-edt-pyc

The wrapping procedure will relocate a node at point (x, y) on the planar mesh to (r,θ,z), where r is the specified radius, θ = xr, and z=y, as shown in Figure 1. A point on the planar orphan mesh located at (0, 0) is mapped to location (r, 0, 0) on the cylindrical surface.

Figure 1. Wrapping a planar orphan mesh.

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:

  1. Use the tools in the Assembly module to translate and/or rotate an instance of the planar orphan mesh in the assembly.

  2. Use the Create Mesh Part tool in the Mesh module to create a planar mesh part from the reoriented instance.

  3. Wrap the reoriented mesh part.

  4. Create an instance of the wrapped part, and use the tools in the Assembly module to translate and/or rotate the instance in the assembly.

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.

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.