Convergence issues in nonlinear masonry model

[Sti_MA]

Hello everyone,

I am working on a 3D layered shell FE model of a masonry building in STKO. In my model, the vaults have been neglected, and the vault loads were applied as node forces at the impost nodes. Each floor has been modelled as a rigid diaphragm using the equalDOF constraint, with the master nodes placed at the center of mass of each level. The floor masses are concentrated in these master nodes.

The model is nonlinear, and I adopted the damageTC3D material model for the masonry. I am performing parallel time-history analyses, but the structural response does not appear to be global. I attach my first model (“Model_base.scd”), where this issue is clearly visible.

In order to mitigate the widespread local damage, I tried introducing elastic and rigid plates. At first glance, this seemed to improve the behavior. However, the analysis now stops at around 20–25% due to convergence problems. I already tried different solution algorithms (Newton, Newton with Line Search, Krylov-Newton with max dim 100), but without success: the analysis always stops at the same point.

I am attaching the "Model_Withplates.scd" file with the added plates and the post-processing results at the step where the analysis fails (post-processing files are in the folder "Out_Sat"). After a certain number of steps, the structure again shows a non-global response, with localized damage and unrealistically high accelerations.

Could you please help me identify where the problem might be, or suggest possible solutions/workarounds? I would be very grateful for your support, especially since I am in the final phase of my PhD and need to finalize these analyses quite urgently.

Thank you very much in advance for your help!

Best regards,

[STKO Team]

From the results, I can see that you partitioned your model into multiple domains for parallel processing. However, you used

1. the RCM numberer, and
2. the UmfPack system,

which are both intended for sequential analyses. As a result, each partition is treated as a stand-alone model rather than as part of a global parallel system.

For partitioned (domain-decomposition) parallel analyses, you should instead use:

1. Parallel RCM numberer, and
2. Mumps system,

which are specifically designed for distributed parallel computations.

[Sti_MA]

Thanks for pointing this out! Apologies for the confusion — the file I shared earlier was from some of my test runs. In my actual work I have already set up the analysis with Parallel RCM numberer and Mumps system. The issues I described (non-global response, convergence problems, etc.) are precisely the ones occurring in the parallel analysis with the correct settings.

I’m now attaching the correct file launched in parallel with 5 processors (but I experienced the same problem also when running with 16 processors), together with the post-processing outputs where the anomalous behavior appears.

I am also re-attaching the model with the added plates. This solution was already tested on 16 processors, and in that case the analysis stopped due to convergence issues after about 20–25% of the run.

Could you kindly help me understand where the problem might lie, or suggest possible solutions? Your support would be greatly appreciated.

[STKO Team]

When using a continuum (or shell) model, you cannot lump masses and forces at single nodes as you would in a frame model.
If you do so — especially with a fine mesh — you will experience stress singularities.

In your model, the vertex 1189 (of Geometry 1800) fails under gravity, which causes the dynamic analysis to diverge.

LOCAL_FAILURE.png (72.88 KiB) Viewed 1542 times

This node has a total of -162650.94 N of concentrated node force acting on it in the vertical direction.
With a mesh size of approximately 500 mm, the applied force acts on roughly half of an element, i.e., over a length of 250 mm.
Given a thickness of 350 mm, the resisting area can be estimated as:
A = 250 mm × 350 mm = 87500 mm^2

If the peak compressive strength of the material is 1 MPa, the maximum resistant force at that section is:
Fmax​ = 1 MPa × 87500 mm^2 = 87500 N
which is less then the applied vertical force.


Key Insight
In reality, the force does not act on a point — it is distributed over a contact area.
Applying it at a single node in a continuum model artificially concentrates the load, leading to localized failure and numerical instability.