**Principles** #1

**1. ****Try to fix all nodes without displacement, and don’t let the solver determine the displacement of these nodes through iterative calculation.**

A simple example of a two-dimensional plane strain problem is illustrated in Fig. 1, which consists of a cylinder and a flat plate made of two elastomers.

The inner wall of the circular hole in the center of the cylinder is defined as the fixed boundary condition. The displacement U2 is defined at point a, located in the center of the top of the plate, with the intention of causing the plate to move directly downward and make contact with the cylinder.

Once the analysis is submitted, the calculation is carried out, but the results show an abnormal displacement of the plate, as depicted in Fig. 2.

What could be the cause of this?

Fig. 1 defines the model of displacement boundary

Fig. 2 abnormal displacement of the flat plate during post-processing

For a three-dimensional model, each component has three translational degrees of freedom and three rotational degrees of freedom. In contrast, a two-dimensional model has two translational degrees of freedom and one rotational degree of freedom.

When conducting a static analysis, it is crucial to define sufficient boundary conditions on all translational and rotational degrees of freedom of each entity in the model to prevent uncertain rigid body displacement. If boundary conditions are not defined, the analysis may not converge or produce incorrect results.

In this example, a fixed boundary condition is defined on the cylinder, ensuring no rigid body displacement. However, no boundary conditions are defined in the X direction for the plate, causing uncertainty in its rigid body displacement in that direction. In the Y direction, the displacement U2 is only given at one node (point A), allowing the plate to rotate rigidly around that point.

While it may seem that the model does not cause any rotation or X-direction translation of the plate, it does not meet the requirements for finite element analysis. The idea that “because there is no force, it will not move” is a logical analysis based on life experience, but the solution process of Abaqus/Standard is the opposite. It iteratively tries various possible displacement states to determine if they meet the static equilibrium equation.

In this example, no matter the magnitude of the plate’s rotation or X-direction translation, the static equilibrium equation can still be satisfied, resulting in an infinite number of displacement solutions and “numerical singularity.” As finite element is a numerical calculation method, small errors in the calculation process can lead to rigid motion of the plate on the degree of freedom lacking constraints. This can result in abnormal results, as shown in Fig. 2.

**R****esolvent:**

The model in this example is symmetrical from left to right. As a result, only half of the cylinder and plate need to be modeled, and the symmetrical boundary condition is applied to the entire symmetry plane. Specifically, U1=0, which prevents the plate from rotating or translating in the X direction.

It’s important to keep in mind that a model’s symmetry is not just determined by its geometry, but also by the symmetry of its material, loads, boundary conditions, and contacts. This means that the deformed model must also be symmetrical.

If the model lacks symmetry, it’s necessary to add appropriate boundary conditions based on the specific scenario to eliminate any uncertain rigid body displacement.

In this example, the boundary condition U1=0 can be applied to the central symmetry line of the plate.

It’s important to note that defining U1=0 at point A alone is not sufficient, as the entire plate can still rotate rigidly around that point.

**Principles** #2

In the model, achieving static equilibrium cannot be done solely through the application of two external forces. Instead, the equilibrium must be established through the reaction force at the boundary condition.

For example, consider a two-dimensional flat plate with uniformly distributed tension at both ends, as shown in Figure 3a. If the entire flat plate is modeled without any boundary conditions, the warning message “numerical singularity” often appears during the analysis. This occurs because, despite being in static equilibrium, the whole plate is suspended in the air and has an infinite number of possible displacement states.

A more appropriate modeling method is shown in Figure 3b, where only 1/4 of the plate is modeled based on symmetry and symmetrical boundary conditions are defined on two symmetrical planes. This ensures that the displacement solution of the static equilibrium equation is unique and the static analysis converges.

(a) Tension at both ends of two-dimensional plate

(b) Take 1/4 for modeling according to symmetry

Fig. 3

Before setting up a model, the first thing to consider is whether the model has symmetry and can only be modeled in 1/2, 1/4, or even 1/8.

This is crucial in many ways.

Defining symmetrical boundary conditions on the plane of symmetry helps to prevent rigid body displacement issues.

It significantly reduces the size of the model and shortens the calculation time.

By halving the number of nodes on the contact surface, the contact analysis becomes easier to converge.

Once the symmetrical boundary conditions are applied, the overall support condition of the model becomes more stable, reducing the potential displacement state. Abaqus/standard does not have to repeatedly try displacement solutions without symmetry, making it easier to find the correct solution and simplifying complex nonlinear analysis.

For dynamic analysis, it is not necessary to define boundary conditions on all degrees of freedom, as dynamic analysis takes into account inertial forces, avoiding infinite instantaneous motion.

If you encounter the warning message of “numerical singularity” in dynamic analysis, it is often a result of other problems with the model, such as “over plasticity”.

**Principles** #3

In each analysis step, if there is no force load on a specific degree of freedom, it must be constrained by boundary conditions.

If a force load is applied, the boundary condition on that degree of freedom must be removed.

As shown in Figure 4, a fixed boundary condition is defined on the inner wall of the circular hole in the center of the cylinder. The boundary condition U1=0 is defined on the central symmetry line of the plate, and a downward point load is applied at point “a” on the top of the plate.

However, even after submitting this model for analysis, it fails to converge.

Fig. 4 defines the model of force load

Although this model may seem fine at first glance, it doesn’t meet the basic requirements of finite element analysis. The cylinder is fixed, and there is no rigid body displacement issue in the X direction as the plate is constrained. In the Y direction, the plate is subjected to a downward force and should move downward. However, this model doesn’t meet the basic requirement of finite element analysis as force load cannot replace the constraint of displacement boundary conditions.

In static analysis, the static equilibrium equation must be satisfied at each incremental step. In the initial state of this example, the top of the plate is subjected to a downward force, but the bottom has not yet touched the cylinder, so a static balance cannot be formed.

If only displacement boundary conditions are defined in the model and no force load is applied (i.e., the external force is 0), the model is always in static equilibrium, and convergence can be easily achieved. This highlights that if the displacement (i.e., the displacement load) can be specified during modeling, force load should not be applied, which can greatly reduce the difficulty of convergence.

This technique is especially important in dealing with complex nonlinear problems.

**R****esolvent:**

An analysis step is added before the application of the force load. Instead of defining the force load, a temporary displacement boundary condition, U2=-1.001, is defined at the position where the plate is subjected to external force. This will result in an interference of 0.001 between the plate and the cylinder, ensuring that the contact relationship between the two is fully established.

In the next analysis step, the temporary boundary condition is removed, and the force load is applied.

This example showcases a crucial finite element modeling technique: the displacement boundary condition is used to smoothly establish the contact relationship, followed by the application of the force load in the next analysis step.

The same technique can also be applied in other complex nonlinear problems, such as when the model struggles to converge due to large deformation under a large load. In such cases, we can first estimate the approximate displacement, define the critical displacement boundary condition at the position of the applied load, and let the model move to the approximate position of the final state.

Then, in the next analysis step, the temporary displacement boundary condition can be removed, and the force load can be applied. This helps the solver find the convergent displacement solution more easily.

**Important modeling skills of finite element contact analysis.**

**1. Mesh of contact surface**

If you’re worried about stress, strain, and displacement in the contact area, you need to refine the mesh in that specific location. The refined area should be slightly bigger than the actual contact area.

For other parts of the model, it’s recommended to use a coarser mesh, as illustrated in Figure 5.

Fig. 5 divide uniform fine mesh in the contact area

An important principle in finite element mesh generation is:

Refine the mesh in important areas to enhance calculation accuracy, and coarsen the mesh in unimportant areas to reduce computation time.

Uniformly meshing the entire model may appear aesthetically pleasing, but excessive refinement of the mesh can result in a substantial increase in computing time without any significant benefit.

**2. Master and slave surfaces**

In finite element contact analysis, it is important to ensure that the mesh density of the master surface is not finer than that of the slave surface to prevent penetration. The highest accuracy in calculation results is achieved when the mesh density of both surfaces is the same.

When defining the contact surface, it is best to make the slave surface as small as possible and exclude areas where contact is not possible, especially if the contact surface is limited slip. It should also be ensured that all parts of the slave surface remain within the normal coverage of the master surface during the entire analysis process.

Another key principle in finite element contact analysis is to define as many boundary conditions as possible based on actual engineering, rather than relying on friction to constrain the translation and rotation of rigid bodies. This is because at the start of the analysis, the contact relationships have not been established, and friction cannot play a constraint role.

## Conclusion

In addition to mesh division, the proper setting of loads, constraints, and boundary conditions is also crucial in finite element analysis.

To obtain accurate simulation results, it is important to perform a specific analysis based on the specific conditions such as product models and operating conditions. Accumulating experience through additional projects and using minimal computing resources can help achieve this goal.