# Node Interaction in Mechanical, Part 3: Nodal Boundary Conditions

This article is Part three in a four-part series about taking advantage of the new nodal interaction capabilities in Workbench 14.0. In Part 1 I discussed how to pick nodes and retrieve information about them. In Part 2 I covered various methods of creating nodal Named Selections. In this installment I’ll address the procedures for applying loads and constraints to mesh nodes, as well as rotating them into different coordinate systems.

All of the nodal boundary conditions, including nodal rotations (which I realize isn’t a boundary condition, per se, but it does affect how boundary conditions are applied) may be found in the Direct FE pull-down menu when the Analysis branch is highlighted.

One key thing to note about all of the nodal boundary conditions is that they may only be scoped to Named Selections, not Geometry Selection. So before you continue, make sure you’re well versed in nodal Named Selection creation.

Stepping through the Direct FE commands in menu order, the first item we come to is Nodal Orientation. This is how we rotate a node to another coordinate system. Of course, to be able to reorient a node to another coordinate system, we will have to create one first. Once that’s done, select Nodal Orientation from the Direct FE pull-down menu.

In this case, we will rotate the nodes belonging to the named selection EndNodes to a cylindrical coordinate system I created at the end of the tube called Cylindrical Coordinate System (because I’m original like that).

Click Direct FE > Nodal Orientation. In the Details window set the Named Selection to EndNodes and Coordinate System to Cylindrical Coordinate System. Easy peasy. Note that the Scoping Method cell is grayed in with “Named Selection,” indicating that you can’t change it.

Just as in Mechanical APDL, all forces and constraints are applied in the nodal coordinate system, defined by the Nodal Orientation. In this example, I applied FE Displacement constraints in the X (radial) direction and Nodal Forces in the Y (theta) direction and verified them in Mechanical APDL.

One thing to keep in mind is that Nodal Orientation is rarely necessary, since loads and constraints applied to solid model entities may be applied in user defined coordinate systems and Frictionless Supports rotate nodes to be normal to the surface.

Moving along, for the Nodal Force example we will apply a downward force to the 12 nodes contained in the Named Selection EndFaceNodes.

Following a similar procedure as before, click Direct FE > Nodal Forces. Set the Named Selection to EndFaceNodes and enter –1200 lbf for the Y Component of force. Note that Nodal Coordinate System is set in gray for the Coordinate System selection. The key item to note, however, is the Divide Load by Nodes option. If set to Yes, the load will be split evenly between the nodes, in this case 1200 lbf/12 or 100 lbf per node, for a total of 1200 lbf applied. If set to No, the full load is applied to each node in the Named Selection, giving a total applied load of 1200 lbf x 12 = 14,400 lbf total.

Here are the Probes of the Reaction Loads with the Divide Load by Nodes option set to Yes and No.

Divide Load by Nodes = Yes

Divide Load by Nodes = No

To applied pressures to nodes, click Direct FE > Nodal Pressure and specify the Named Selection and pressure value. Note that the pressure can only be applied in the normal direction to nodes. Also note that, at a minimum, the nodal Named Selection has to consist of all the corners on an element face for the pressure to have any meaning.

Apply constraints directly to nodes by clicking Direct FE > FE Displacement. Specify the Named Selection and enter the displacement values in the nodal coordinate system X, Y, and Z direction (or leave Free).

Nodal rotations (Direct FE > FE Rotation) may only be applied to nodes attached to elements with rotational degrees of freedom, such as beams and shells. The rotations themselves can only be fixed (i.e. zero degrees) or free. At this time there is no capability to impose a finite nodal rotation.

In the next and final installment, I will discuss how to scope results to nodes and verify nodal and element orientations. Get ready to be thrilled.