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: a two-dimensional plane strain problem consists of two elastomers, a cylinder and a flat plate, as shown in Fig. 1.
The fixed boundary condition is defined on the inner wall of the circular hole in the center of the cylinder, and the displacement U2=-2 is defined at point a in the center of the top of the plate, hoping to make the plate move directly downward and contact the cylinder.
After submitting the analysis, the calculation can be completed, but the abnormal displacement of the plate is seen in the analysis results, as shown in Fig. 2.
What causes this?
Fig. 1 defines the model of displacement boundary
Fig. 2 abnormal displacement of the flat plate during post-processing
For the three-dimensional model, each component has three translational degrees of freedom and three rotational degrees of freedom;
For a two-dimensional model, each component has two translational degrees of freedom and one rotational degree of freedom.
When establishing the static analysis model, sufficient boundary conditions must be defined on all translational and rotational degrees of freedom of each entity in the model to avoid uncertain rigid body displacement, otherwise the analysis will often fail to converge, and even if it can converge, the result is often wrong.
In this example, the fixed boundary condition is defined on the cylinder, and there will be no rigid body displacement.
However, the plate does not define any boundary conditions in the X direction, so the displacement of the rigid body in the X direction is uncertain;
In the Y direction, the displacement U2 is given on only one node (point a).
At this time, the whole plate can still rotate rigidly around point a, that is, except for point A, U2 of other nodes on the plate is uncertain.
Although the whole model does not cause the load of rotation or X-direction translation of the plate, it seems to be no problem intuitively, but such a model meets the requirements of finite element analysis.
This kind of causal relationship of “because there is no force, it will not move” is just the idea of logical analysis in our mind according to life experience.
The solution process of abaqus/standard is exactly the opposite.
Its process is to iteratively try various possible displacement states to test whether they can meet the static equilibrium equation.
In this example, no matter how large the rotation of the plate or the translation in the X direction, the static equilibrium equation can be satisfied, that is, there are infinite displacement solutions that meet the static equilibrium conditions, so “numerical singularity” will appear.
Finite element is a numerical calculation method.
Small numerical errors in the calculation process will lead to rigid motion of the plate on the degree of freedom lacking constraints.
Therefore, abnormal results as shown in Fig. 2 will be seen.
The model in this example is left-right symmetrical, so both the cylinder and the plate should be modeled by taking only half, and the symmetrical boundary condition is defined on the whole symmetry plane, that is, U1=0, so that the plate will not rotate or translate in the X direction.
It should be noted that whether a model has symmetry depends not only on its geometry, but also on whether the material, load, boundary conditions and contact are symmetrical, that is, whether the deformed model is symmetrical.
If the model does not have symmetry, it is necessary to add appropriate boundary conditions according to the specific situation to eliminate the uncertain rigid body displacement.
In this example, the boundary condition U1=0 can be defined on the central symmetry line of the plate.
It should be noted that U1=0 of point A cannot be defined only, because the whole plate can still rotate rigidly around point A.
In the model, it is not enough to achieve static equilibrium only by two external forces, and the equilibrium must be achieved by means of the reaction force at the boundary condition.
A simple example is also given:
The two ends of the two-dimensional flat plate are under uniformly distributed tension, as shown in Fig. 3a.
If the whole flat plate is directly modeled, there is no boundary condition.
After submitting the analysis, the warning message of “numerical singularity” often appears. Because at this time, although the whole plate is in static equilibrium, there will still be uncertain rigid body displacement, because the whole plate is suspended in the air, and there are countless possible displacement states.
A more reasonable modeling method is shown in Fig. 3b.
According to symmetry, only 1/4 is used for modeling, and symmetrical boundary conditions are defined on two symmetrical planes.
In this way, the displacement solution of the static equilibrium equation can be guaranteed to be unique, and the static analysis can converge.
(a) Tension at both ends of two-dimensional plate
(b) Take 1/4 for modeling according to symmetry
Before establishing a model, the first thing to consider is whether the model has symmetry and whether it can only take 1/2, 1/4 or even 1/8 for modeling.
This is of great significance in many ways.
Defining symmetric boundary conditions on the plane of symmetry is helpful to avoid rigid body displacement problems;
It can greatly reduce the scale of the model and shorten the calculation time;
If the nodes on the contact surface are reduced by half, the contact analysis is easier to converge;
After the symmetrical boundary conditions are applied, the support condition of the whole model becomes more stable, and the possible displacement state is greatly reduced. Abaqus/standard does not need to repeatedly try those displacement solutions that do not have symmetry, so it is easier to find the correct displacement solution, and it will make the complex nonlinear analysis easier to converge.
For dynamic analysis, it is not necessary to define sufficient boundary conditions on all degrees of freedom, because dynamic analysis will consider inertial forces, which can avoid infinite instantaneous motion.
If you see the warning message of “numerical singularity” in dynamic analysis, it is often due to other problems in the model, such as “over plasticity”.
In each analysis step, if there is no force load on a certain degree of freedom, there must be boundary conditions to constrain this degree of freedom;
If a force load is applied, the boundary condition on this degree of freedom must be removed.
As shown in Fig. 4, the 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.
After submitting this model for analysis, it also fails to converge.
Fig. 4 defines the model of force load
Although from the intuitive sense, this model seems to be no problem.
The cylinder is fixed, and there is no rigid body displacement problem.
In the X direction, there is no rigid body displacement problem when the plate is constrained;
In the Y direction, the plate is subjected to a downward force and should move downward.
Like “because there is no force, it will not move”, this model also does not meet the basic requirements of finite element analysis, because force load cannot replace the constraint of displacement boundary conditions.
In static analysis, the static equilibrium equation should 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 contacted the cylinder, so 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.
It can be seen that if the displacement (i.e. the displacement load) can be specified during modeling, the force load should not be applied, which can greatly reduce the difficulty of convergence.
This skill is particularly important for dealing with complex nonlinear problems.
An analysis step is added before the analysis step of applying force load.
Instead of defining force load, a temporary displacement boundary condition U2=-1.001 is defined at the position where the plate is subjected to external force, which will produce an interference of 0.001 between the plate and the cylinder, which can ensure that the contact relationship between the two is fully established.
In the next analysis step, remove the temporary boundary condition and apply the force load.
In this example, a very important finite element modeling technique is used:
Firstly, the displacement boundary condition is used to establish the contact relationship smoothly, and then the force load is applied in the next analysis step.
In other complex nonlinear problems, the above techniques can also be used.
For example, it is difficult for the model to converge due to large deformation under a large load. At this time, we can first estimate the approximate displacement, define the corresponding critical displacement boundary condition at the position of the applied load, and let the model move to the approximate position of the final state, and then remove this temporary displacement boundary condition in the next analysis step and apply the force load.
This can help the solver find the convergent displacement solution more easily.
Important modeling skills of finite element contact analysis.
1. Mesh of contact surface
If you are concerned about the stress, strain and displacement of the contact area, you need to refine the mesh at the corresponding position, and the refined area should be slightly larger than the contact area.
For other parts of the model, a coarser grid should be divided, as shown in Figure 5.
Fig. 5 divide uniform fine mesh in the contact area
An important principle of finite element mesh generation:
The mesh of important areas must be refined to improve the calculation accuracy, and the mesh of unimportant areas must be thicker to save calculation time.
Dividing the whole model into uniform meshes without thinking may be visually beautiful, but unnecessary refinement of the mesh often leads to a significant increase in computing time.
2. Master and slave surfaces
When meshing in finite element contact analysis, it is generally required that the mesh of the master surface should not be thinner than that of the slave surface to avoid penetration.
When the mesh density of the master surface and the slave surface is the same, the accuracy of the calculation result is the highest.
In addition, when defining the contact surface, if it is limited slip, the slave surface should be as small as possible, and do not include those areas where contact is impossible.
It should be ensured that all parts of the slave face are always within the normal coverage of the master face during the whole analysis process.
Another important principle in finite element contact analysis is not to rely on friction to constrain the translation and rotation of rigid bodies, but to define as many boundary conditions as possible according to the actual engineering.
Because at the beginning of the analysis, the contact relations have not been established, and the friction cannot play a constraint role.
In addition to grid division, the setting skills of loads, constraints and boundary conditions are also the focus of finite element analysis.
It is necessary to conduct specific analysis based on specific conditions such as product models and working conditions, do more projects to accumulate experience, and use as few computing resources as possible to obtain as accurate simulation analysis results as possible.