A non-zero static load/displacement has been applied in a nonlinear analysis. This may lead to non-converging solution. In order to avoid this, please try to ramp the load/displacement by the help of a function or table upload
This is a warning message which points to any static load/displacement applied in nonlinear analysis. This message warns the user to avoid doing this in order to allow the solution to converge more easily.
What could be the possible reason?
One of the loads or displacements has been applied with a single non-zero static value in a nonlinear analysis. Especially in cases where geometric or material nonlinearities are present, a single static load may introduce high nonlinearities that can not be resolved correctly. At each time step the same equation system will be solved. This means that solver will try to solve for a high load in a first time step and will most probably fail to converge. If Auto timestep definition is used, the solver will try to reduce the nonlinearity by breaking the time steps in to smaller ones but this has no effect and the simulation will fail to converge.
What can I do now?
Make sure that a high load or displacement has not been applied in a single step if a nonlinearity is involved. A good practice is to ramp the load or displacement either by using a function or table upload. A simple example below elaborates the case.
Let’s consider a strain test simulation of an elastoplastic structured steel probe as shown in the figure below.
Since in this case both geometric and material nonlinearities will be involved, therefore Nonlinear is set to true under Analysis type as shown in figure below.
Considering that the deformation would be high, Geometric behavior is set to nonlinear under Simulation Model Properties as shown in figure below.
The probe was than given an elastoplastic material behaviour via table upload. The material definition is shown in the figure below.
The probe was than constrained in all directions from one end and a force was applied in positive x-direction on the other end (red highlighted face in above geometry figure). Now here comes the most interesting part for which we can distibute our case in to two important cases; Bad practice and Good practice.
We apply a static force of 10,000 N as shown in the figure below.
Next we select Auto timstepping scheme under Simulation Control as shown in figure below.
If we now run our case, the simulation will start diverging after even the first time step of 0.1 since the solver will apply a full load of 10,000 N in this single step and tries to solve a high nonlinearity occuring with in this step. After failing under user specified Newton iterations, it will start cutting the timestep in order to reach convergence and keeps on doing it until minimum timestep level is reached. In the figure below one can see the divergence on the first step due to non-resolution of the material behavior.
In order to solve this problem, we can do to things; ramp our load over time using function or using table upload. To ramp it using function, we can define the function as shown in figure below.
To ramp it using table upload, we have to upload a table defining the load increment over specific time. Figure below shows how it can be done. Please note that the Interpolation is set to linear in order to let the load increase linearly over specified time.
By doing any of the above option, we actually now ramp the load over time running from 0.1 to 1 second. Which means that now (10,000 x 0.1) = 1,000 N of force will be applied in each step and increase linearily which can be easily resolved by the solver. By doing this one can easily obtain a converged solution as shown in figure below.
If none of the above suggestions did solve your problem, then please post the issue on our forum or contact us.
Last updated: January 29th, 2019
Did you find this article helpful?
How can we do better?
We appreciate and value your feedback.