Create a node. You can specify the coordinates of the new node either in the global coordinate system or in a datum coordinate system that you specify.

Edit nodes. You can specify the new coordinates of the nodes either in the global coordinate system or in a datum coordinate system that you specify. Alternatively, you can specify an offset from the current position. You can edit a single node, or you can edit multiple nodes simultaneously.

Delete nodes. Any elements associated with the deleted nodes are also deleted. In addition, you have the option of deleting any remaining nodes that would be left unassociated with any elements once the nodes selected for deletion and their associated elements are deleted.

Merge selected nodes. If you select only two nodes to merge, ABAQUS/CAE creates a new node at the midpoint of the selected nodes. If you select more than two nodes, you can specify the Node merging tolerance, which is the maximum distance between nodes that will be merged. ABAQUS/CAE deletes nodes that are closer than the specified distance and replaces them with a single new node. The location of the new node is the average position of the group of nodes that were merged into the new node.

While ABAQUS/CAE is removing duplicate nodes, you can choose to remove duplicate elements that have the same connectivity. You can also merge instances of orphan mesh parts in the Assembly module; for more information, see “Merging meshed part instances,” Section 13.6.2.

Adjust the position of the midside node of second-order elements to allow for the singularity at the crack tip in a fracture mechanics analysis. You can select nodes and enter a bias parameter between 0 and 1. ABAQUS/CAE moves the midside nodes along connected element edges to a position based on the parameter that you entered. For example, if you enter a parameter of 0.25, ABAQUS/CAE biases the position of the midside nodes one quarter of the length of the element edge away from the selected nodes.

For more information, see “Controlling the singularity at the crack tip for a small-strain analysis,” Section 20.1.5, and “Constructing a fracture mechanics mesh for small-strain analysis” in “Contour integral evaluation,” Section 7.10.2 of the ABAQUS Analysis User's Manual.