Subdividing elements

Select MeshEdit from the main menu bar to subdivide one or more selected orphan mesh elements. The elements to be subdivided must be connected. You can select an edge, a face (solid elements), or All Directions to divide elements in one, two, or all directions—two for shell elements, three for solid elements. You must also specify the number of divisions to make. Abaqus/CAE divides the elements evenly into the specified number of divisions in each direction. The new elements have the same element type as the originals. You can subdivide elements in the mesh only if the element domain contains only linear elements.

Related Topics
What can I do with the Edit Mesh toolset?

  1. Enter the Mesh module. Select Part from the Object field in the context bar, and select a part that contains orphan mesh elements from the list.

  2. From the main menu bar, select MeshEdit.

    Abaqus/CAE displays the Edit Mesh dialog box.

    Tip: You can also display the Edit Mesh dialog box using the tool, located at the bottom of the Mesh module toolbox.

  3. From the Category field, choose Mesh.

  4. From the Method list, select Subdivide layers.

  5. Select the elements that you want to subdivide. You can use any of the following methods:

    • Select elements from the viewport. You can select elements individually, by angle, by feature edge, or by topology (for more information, see Selecting objects within the current viewport). Click mouse button 2 when you have finished making selections.

    • Select one or more existing element sets. Click Sets on the right side of the prompt area to display the Region Selection dialog box containing a list of available sets. Select one or more sets from the list, and click Continue.

    The selected elements must form a single connected set.

    Note:

    The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Sets on the right side of the prompt area.

  6. Select an element edge to indicate a single direction of subdivision; select the face of a solid element to indicate two directions; select All Directions in the prompt area to indicate all directions—two for shell elements or three for solid elements.

    Abaqus/CAE attempts to subdivide the elements. If dividing the elements will create incompatibilities in the mesh, Abaqus/CAE displays a dialog box indicating that the resulting mesh will be nonconforming. Click Yes to divide the elements or No to clear your selections and return to Step 4.

    Tip: If you make a mistake while dividing elements in a mesh, click Undo in the Edit Mesh dialog box to undo the change. Abaqus/CAE restores the original mesh.

After editing an orphan mesh, you should always verify node-, element-, and surface-based features such as section assignments, loads, and interactions to ensure that they are correctly applied to the modified mesh.