Remote Points in ANSYS: What Are They and Why Use Them?

Remote Points are the primary technique ANSYS uses to attach a node, multiple nodes, or a collection of nodes scoped by vertices, edges, faces, elements, and named selections to a single node called a pilot node. A Remote Point utilizes multipoint constraint (MPC) equations to create the attachment between the selected nodes and the pilot node. In this article, we will focus primarily on the rigid and deformable behavior of the scoped nodes in the FE model.

Remote Points are used in the creation and attachment of the following:

• Point Masses

• Joints

• Springs

• Bearings

• Beam Connections

• Remote Forces

• Moments

• Remote Displacements

Therefore, the lessons and information defined in this article will also directly apply to point masses, joints, springs, bearings, beam connections, remote forces, moments, and remote displacements.

Let's get started using a simple rectangular steel beam placed in tension. The beam is 10 inches long, 1 inch wide, and 0.15 inches thick. The beam has been split into three pieces: the first section is 2.5 inches long, the second section is 5 inches long, and the third section is 2.5 inches long. The three sections of the beam are joined together as a single part, eliminating the need for contacts or merged nodes. The beam is made from steel with a modulus of elasticity of 2.9E7 psi.

Beam Example

Let's mesh the model using our default sizing.

Meshed Beam Model

Now that we have this model meshed, let's add a Remote Point that attaches all of the nodes in the center section of the beam to a single pilot node.

For our beam-in-tension example, let's hover over Model in the model tree, right-click, then hover over Insert and select Remote Point. We have now added an undefined Remote Point to our model.

To define this Remote Point, we must first define the nodes that are connected to the pilot node. ANSYS Mechanical gives us the option to select individual nodes, vertices, edges, faces, elements, and named selections for the scoping method. Please note that although ANSYS gives us the option to select vertices, edges, faces, elements, and named selections for a scoping method, it converts the selection to a collection of nodes in the background.

For this example, we will select all of the nodes in the center section of the beam. Simply hide the first and third sections of the beam. Then, using the node selection filter, box-select the center section of the beam or right-click and choose Select All.

Next, we need to define the location of the pilot node. ANSYS allows us to select a coordinate system and define the X, Y, and Z coordinates of the pilot node relative to that system. Because we selected all of the nodes in the center section of the beam, ANSYS has defined the X, Y, and Z coordinates at the center of these nodes and selected the Global Coordinate System. To make the Remote Point easier to see in this model, let's move its pilot node to 1.0 inch in the Y direction. Again, this step is not necessary, but it will show more clearly where the pilot node resides.

Let's see what this Remote Point looks like. Select the Display Tab, then select Remote Point Connections.

Remote Point 1

Now we are at the heart of this article: the behavior of this Remote Point. For this first run, let's set its behavior to Rigid.

We can now fix one side of the beam and add a tensile force of 1,000 lbf.

Loads and Boundary Conditions

Before we look at these ANSYS results, let's predict what we expect to happen. Because we set the Remote Point to Rigid, we have mathematically coupled these nodes using MPCs. We have explicitly modeled a 10-inch-long beam in ANSYS, but 5 inches of that beam is infinitely rigid; therefore, this 10-inch-long beam should behave as a 5-inch-long beam.

Now let's look at the results. We have excellent correlation between our hand calculations and this FE model with a Rigid Remote Point.

Let's get this beam to behave normally. Highlight our Remote Point and change Behavior from Rigid to Deformable. Now let's re-solve our FE model.

Please don't peek at those results; let's predict what we expect to happen. Because we set the Remote Point to Deformable, the nodes will be free to move independently and expand when this load is applied. We have explicitly modeled a 10-inch-long beam in ANSYS; therefore, this 10-inch-long beam should behave normally.

Now we can look at the results. Once again, we have excellent correlation between our hand calculations and this FE model with a Deformable Remote Point.

Let's recap what we have learned. Remote Points are extremely versatile and are used to create point masses, joints, springs, bearings, beam connections, remote forces, moments, and remote displacements. The behavior of Remote Points can be defined as Rigid or Deformable. When a Remote Point's behavior is set to Rigid, its nodes are mathematically locked together; essentially, they are infinitely stiff. When the behavior is set to Deformable, the Remote Point is flexible and adds no stiffness to the system. Other behavior options, such as Coupled and Beam, will be covered in Part 2 of Remote Points.

Thank you for taking the time to read this article, and please contact me if you have ideas for future articles.

John Parsons

Analyst

MESim LLC

John.Parsons@MESim.us

www.MESim.us