abaqus cohesive contact respose warning explanation 1

[rw5]

hi,

im modeling a cyclic loaded masonry wall in abaqus.
I keep getting warnings such as:

COHESIVE CONTACT RESPOSE IS COMPUTED AT SLAVE NODE 24 INSTANCE
OPEKA-2-LIN-2-1-1-LIN-1-2-1-LIN-1-7 THAT FELL OFF THE MASTER SIDE
OPEKA-2-LIN-2-1-1-LIN-1-2-1-LIN-3-1 THAT FELL OFF THE MASTER SIDE
USING A SEPARATION OF 1.00000E+36.
USING A SEPARATION OF 1.00000E+36.

The warnings show up on the beginning of the calculation, and continue to show up the whole time.
Eventually the calculation is aborted, and I suppose it has to do with these warnings.
Could someone explain what these warnings are about?

Tnx

 

[FEA way]

What is the error message when the analysis fails ? Are there no other warning messages ? Did you check the results (mainly field outputs and deformed shape) from right before the analysis stopped ?

 

[rw5]

Error message:
Too many attempts made for this increment
The analysis has been terminated due to previous errors. All output requests have been written for the last converged increment.
Abaqus/Standard Analysis exited with an error - Please see the message file for possible error messages if the file exists.

Other warning messages include:
Whenever a translation (rotation) dof at a node is constrained by a kinematic coupling definition the translation (rotation) dofs for that node cannot be included in any other constraint including mpcs, rigid bodies, etc.
For *tie pair (assembly__pickedsurf1284-assembly__pickedsurf1283), adjusted nodes with very small adjustments were not printed. Specify *preprint,model=yes for complete printout.
Not all the nodes that have been adjusted were printed. Specify *preprint,contact=yes for complete printout.
Not all the nodes that have been adjusted were printed. Specify *preprint,contact=yes for complete printout.
1156 nodes have been adjusted more than once. The subsequent adjustments may cause these nodes not to lie on their master surface. The nodes have been identified in node set WarnNodeAdjust.
MPCS (EXTERNAL or INTERNAL, including those generated from rigid body definitions), KINEMATIC COUPLINGS, AND/OR EQUATIONS WILL ACTIVATE ADDITIONAL DEGREES OF FREEDOM

But I don't thing that these errors are something that would cause the calculation to fail (?)

Deformed shape and field output look ok to me.
It's a masonry wall simplified micro model and the analysis fails when the wall starts to fail (rocking failure), or after 2-3 cycles of relatively small loading (comparing to experimental data). The wall is loaded by cyclic load and the goal is to obtain the hysteresis curve.

 

[FEA way]

This is a typical non-convergence error message. There can be many reasons but if the analysis stops once a failure begins to occur, you may have to add some artificial stabilization to the model. In the case of analyses involving cohesive contact, you can try adding vicious regularization (called damage stabilization in contact property settings).

 

[rw5]

yeah,I've already assigned the viscosity coefficient (=0.002).
I can try to increase the value of the coefficient.
Do you have any advice on choosing the values of the viscosity coefficient? If I understood correctly, it's related to the size of the time increment..

 

[FEA way]

Yes, it should be small compared to the characteristic time increment. There are also other ways to avoid convergence issues (with the most effective one being dynamic explicit analysis) but they are more general and not directly related to cohesive behavior.

 

[rw5]

I'll try to do the calculation with the modified viscosity coefficient but I'll also try the dynamic analysis.
I have several testing specimens and expect relatively large displacements so I think the dynamic analysis could be more suitable.

Can you please tell me, is dynamic explicit analysis suitable for models with prestressing? I intend to reinforce the masonry with prestressed frp laminates. Is prestressing compatible with dynamic explicit analysis?

 

[FEA way]

Abaqus/Explicit always solves for dynamic equilibrium but it can be used to perform quasi-static simulations as well. However, it's often more efficient to use Abaqus/Standard (general static analysis) and then utilize the import functionality to transfer the results to Abaqus/Explicit.