Learning Forum

[Autonewbie]

Hi,

I am running a static nonlinear analysis, nonlinear material with contact that changes abruptly from open to penetrate and open at the last time by applying displacement into 3 steps. Firs two steps are converged and last step seems not stable. I did use stabilization factor but it is still not able to get converged. Last step using time step with min time step at 1E-5. Any idea?

[peteroznewman]

It helps to look at the Solution Output text to see the reason why the solver stopped.

Under Solution Information, change the Newton Raphson Residual line from 0 to 5, then Solve. That will create five plots under the Solution Information folder of the N-R Residual Force plot. Each plot shows where equilibrium is not being achieved on the last five iterations. Sometimes, the location of the maximum jumps around from iteration to iteration if you have a large contact area or multiple contacts in the model. Other times, the maximum will be at the same location on each of the five plots.

The maximum of this plot is the location where making smaller sized elements and better shaped elements will help the solver to obtain convergence at this load.  Add a mesh control to make smaller elements and Solve.

[Autonewbie]

Hi,

I managed to get it converged by refining the mesh.

 

Meanwhile, another new scenario that I face is the contact stress singularity. It has to be sharp corner as it is due to fabrication method. Apart from avoid reading the stress there, I also refine the mesh to check if the stress getting better, still running...

Any suggestion?

The top part is being pushed in and contact with the bottom part to simulate snap thru.

 

[peteroznewman]

As you said, this is a stress singularity, and if you want an accurate evaluation of the stress at this point, you can't get it from this geometry.

You could just ignore the stress in this region as long as the model is converging.

One corrective action is to add a blend radius to the sharp corner and use small enough elements on the blend and flat face touching the blend so that the contact is spread across a many elements. Even "sharp" corners are not sharp at a small enough scale. This will increase the number of nodes in the model and may slow down the solution time significantly.

I often have models with ductile metals. By adding plasticity to the model, the elements at a location like this develop plastic strain and the load is shared by adjacent elements. This prevents the stress from continuing to rise without adding the blend radius to the geometry.