Remote Point Boundary Conditions
The purpose of this project is to bring a guide to the community on how to use remote point boundary conditions in 3D finite element models, an explanation on how they work, and give some hints on when and why they are useful.
To accomplish this goal, we will begin with a small theoretical background needed to fully understand the topic; then we will present some example simulation and analyse the modelling assumptions and results. Although it won’t be deep or mathematically intensive, I think it should be enough to tackle modelling problems and take informed decisions on when (or not) to use this type of boundary conditions. And for those eager to dive deeper and know the technical or mathematical details of the topic, I will leave some links for further reading.
Finite Element 3D Discretisation and Degrees of Freedom
In the Finite Elements Method the continuous solid object is modelled by placing a number of points inside the geometry of the object and then connecting points with their closest neighbors. This process is called meshing (the result of the process is called a “mesh”). The points are called “nodes” and the connection of closest nodes are called “elements”. At the end, we have this set of multiple small elements packed together, just like filling the space the original object would occupy, and they are all connected to their neighbors through the nodes they share.
Figure 1. Finite Element Mesh. Nodes are located at line joints.
The deformation of the object is measured by the movement of the nodes. We can imagine the solid deforming under the action of an external force just like all this points are moving in the space, each one in different directions and proportions. Numerically, the movement of a node is measured with a displacement vector with three space components. This three components are called “degrees of freedom”. A fancy term, but all it means is that no more or less numbers are needed to completely describe the movement of the point. The elements come into play because they are what connect the nodes, relating them and giving the solid stiffness, just as if there were small springs connecting close nodes.
Figure 2: A node in space and six possible degrees of freedom: three translations (UX, UY, UZ) and three rotations (RX, RY, RZ). In Finite Element 3D solid models, only the translations are used. Note that for each degree of freedom, a force or torque load exists that acts in the same direction.
Boundary Condition Modelling and Correlation With Reality
In the modelling of a structural problem, and after the mesh is built and material parameters are defined, something else is needed, and that is the so called “boundary conditions”. There are two types of them: displacements and loads. They are applied to the nodes of the mesh and determine how the body will deform. Also, they are closely related to each other, and are proportional according to the stiffness of the body (think of Hooke’s law, the relation between the elongation of a spring and the applied force).
The boundary conditions are used to model real life physical characteristics of the body under consideration in the following way:
Displacement boundary conditions: used to model regions where the solid has restricted movement. This can occur in the presence of anchor points, bolting, welding, bearing surfaces, structural foundations, known deformations, and the like. At least one of these type of condition is needed for a structural model to be valid, otherwise the model is said to have free-body movement.
Load boundary conditions: used to model interactions with other bodies or phenomena that imposes stress on the solid. This can occur due to weight bearing, fluid static or dynamic pressure, thermal deformation, accelerated movement (inertial loads), and the like. Note that all of these real life loads act in a distributed manner over a surface or volume region; concentrated, nodal forces are modelling constructs that don’t occur in real life. Also, it is important to know that any type of load is always converted to equivalent nodal loads in the Finite Elements Model.
As they are modelling constructs, boundary conditions in a finite elements model can not represent real life conditions in a completely accurate way. For example, a fixed face with all degrees of freedom set to zero will not have any deformation; in the real life though, anchoring always has some grade of flexibility thus deformation. Other example could be an applied load due to carrying weight, which is modeled as a constant distributed pressure over a surface; in real life though, pressure distribution due to contact is not uniform. The structural analyst must be prepared to take into account this facts when interpreting simulation results.
Figure 3. Simulation result of a face with all DoF (degrees of freedom) restricted. See study case below.
Remote Point Boundary Conditions
Imagine a body supported by an axle through a hole. The axle prevents movement in the radial directions, but allows longitudinal movement and also rotation around its axis. How to model this with traditional boundary conditions? You could tackle the translation restrictions, but what about the rotations? Another case could be the a torque load distributed over a face. How do you apply nodal forces such that the resulting effect is equivalent?
One answer to this questions is remote point boundary conditions. The objective is to abstract our model in such a way that we can treat a face as if it was a single point with six degrees of freedom. Then one can apply simple restrictions or loads to this point, and the solver takes care of creating the complex numerical models to make the face behave as we want to. Let’s take a look in more detail:
A remote point displacement boundary condition relates the movements of every node in a face with the movements of a single point in space. This is achieved through a set of linear equations that relate the degrees of freedom of the nodes. It can be visualized as if rigid links connected the remote point to each node in the face.
So, the result is that if the point moves a unit in the X axis, the whole face will move in the X axis. If the point rotates around the Z axis, the whole face will follow the rotation. On the other hand, if the point has its degrees of freedom restricted in a given direction or rotation, the face will follow. Hence you can see the solution to the axle restriction problem.
The analogous to the remote displacement is a remote force. With it, one can apply a force or torque to the remote point and the solver will transfer it to the face (through the same relations created for the remote displacement). The forces on the nodes are distributed according with their distance
One important application of remote forces is torque loads. Remote force allows us to apply torque on a face with great easiness. For that matter, the load must be expressed as a vector with three spatial components (mx, my and mz). The remote point and the vector direction will determine the axis of application of the torque.
In the project you will find several cases and simulations where the capabilities of remote displacements and forces are demonstrated, listed here:
Flexion of an I beam
- Shear load and fixed end, remote point and traditional
- Moment load and fixed end, remote point and traditional
- Top load and pivot ends
- Top load, ends one pivot one sliding
It is left to the reader to examine the project configurations and results. With the post processor stress and deformation results can be visualized. When going through the project, try to bear in mind and answer questions like these:
- How do compare results from traditional boundary conditions versus remote point?
- What are the benefits from one or another?
- Why is this condition modeled this way?
- Which one is more realistic?
References and Further Reading
SimScale documentation for remote displacement
SimScale documentation for remote force
CodeAster theoretical documentation