The Edit Mesh toolset provides the following tools that allow you to manipulate the nodes in your mesh:

• 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.

• Drag nodes. You can click and drag the nodes in a model. You can drag only one node at a time, and you can use the Project to geometry option to project an exterior node to the geometry with which it is associated. Element quality checks are automatically activated to show element errors and warnings while you drag a node. For more information on element quality checks, see “Verifying element quality,” Section 17.19.1.

• Project nodes. You can specify a vertex, edge, or face and Abaqus/CAE projects the nodes from their current positions onto the selected entity. You can project a single node, or you can project multiple nodes simultaneously. You can also project nodes to other nodes, element edges, element faces, datum points, datum axes, or datum planes.

• 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 parts in the Assembly module and you have the option to merge nodes within this process; for more information, see “Merging and cutting part instances,” Section 13.7.1.

• Smooth selected nodes. You can select external nodes, and Abaqus/CAE smooths the node positions with respect to the surrounding nodes. You can smooth any external nodes of the native mesh on a part or on an assembly as long as they are not part of a region boundary; you can also smooth external orphan mesh nodes that lie within a planar mesh face.

• 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 31.2.5, and “Constructing a fracture mechanics mesh for small-strain analysis with the conventional finite element method” in “Contour integral evaluation,” Section 11.4.2 of the Abaqus Analysis User's Guide.

• Renumber selected nodes within an orphan mesh. You can renumber the selected nodes by specifying a starting label and an increment or by offsetting the existing label by a specified value.

For detailed instructions about each of these node manipulation techniques, see “Editing nodes,” Section 64.5.