Too many attempts made for this increment in sandwich panel 1

[AbolfazlYZP]

Hi everyone
I have a model in abaqus standard, my model is a sandwich panel under in-plane compression and lateral pressure.
I’ve got this error:
Too many attempts made for this increment
and this warning:
Exhausted the contact constraint pool. Cutting back the time increment and redoing the current increment. Other wise, set the environment variable aba_gcont_pool_size to high or a numeric number (1,2,...) with 1 being equivalent to high.
The strain increment has exceeded fifty times the strain to cause first yield at 23 points
Excessive distortion at a total of 6319 integration points in solid (continuum) elements
My Model units is mm, the Young’s modulus and Yield stress in MPa.
also I have Cohesive layer and I used Quads Damage (Damage evolution and Damage stabilization Cohesive is also define for this) and Elastic with traction Type. for Enn and Ess, I did E/t cohesive layer for Enn and G/ t cohesive layer for Ess and Ett.
My step is General and Nlgeom is On. maximum number of increments is 300, initial increment size=0.01, minimum 1e-5.
In Interaction module I used Tie constraint for between cohesive and top layer and core layer. and coupling constraint is shown in below figure.
when I used coupling constraint and chose cohesive layer, my model errors for cohesive layer and I checked visualization module > Node sets > WarnNodeOverContieSlave. then I didn’t choose cohesive layer in coupling constraint. I figured out this error happened because the cohesive Layer was Slave.
my problem did not solve, but I didn’t get this warning again (WarnNodeOverContieSlave).
in Load module, My load is 0.01Mpa, and boundary condition shown in below figure. I define boundary condition with selected reference point for 3 side. for bottom side when I choose cohesive layer I’ve got warning incorrectDOF, so I did not select this layer.
I guess my problem is in coupling or boundary condition, but I don’t know what is it.
Can anyone help me?

 

[FEA way]

From your description it seems that you use element-based cohesive behavior (cohesive elements). If you are fine with the assumption of zero thickness adhesive layer, try surface-based cohesive behavior (specified via contact interaction with cohesive behavior property). It's easier to define, causes less trouble and solves faster.

You can also try using automatic stabilization in step settings.

I'm not sure what you mean by "coupled" in the picture with boundary conditions. Let's take the left side as an example. It states: UX = UZ = 0, UY = coupled, UR = 0. So coupling is only applied in the Y direction ? How are the remaining directions constrained in such case ? With boundary conditions applied directly to nodes (not via reference point) ? It would be best if you could attach a screen from Load module showing boundary conditions. Or attach the model's files if you can.

 

[AbolfazlYZP]

I decided to use surface-based cohesive behavior but I can't figure out how to calculate knn, kss and ktt, so I had to use cohesive elements.
in interaction module I used coupling constraint. I coupled in all directions and in boundary condition Ux=Uz=UR0. and applied boundary condition to reference point.
somebody told me don't use tie constraint between layers, is that right?

I also attached my load module and coupling

 

[FEA way]

Cohesive elements have to be embedded in a model via shared nodes or tie constraints. The latter approach is easier. Here are the steps to do this for 3D model:

a) if your cohesive layer is modeled as solid (finite thickness):
- create a finite thickness cohesive layer and position it properly with respect to the rest of the model, define surfaces for tie constraints
- mesh the parts
- edit coordinates of all nodes in the cohesive layer to make them lie along the interface between parts that are connected with adhesive
- define tie constraint using surfaces created in the first step

b) if your cohesive layer is modeled as shell:
- mesh the parts and create orphan mesh
- offset zero thickness layer of solid elements (check the options to: delete base shell elements, create set for new elements and create top and bottom surfaces)
- define tie constraint using surfaces created automatically in the previous step, check mesh stack orientation first to determine when you should use top and bottom surfaces

 

[AbolfazlYZP]

I checked your suggestion and used automatic stabilization in step settings.
but the error still is.
I send my Model for you. can you look at it?

 

[FEA way]

The cohesive layer needs to be aligned with interface (you have to adjust nodal coordinates to make this part flat). You should complete the second to last step of option a) in my previous post.

What’s more, the mesh of the whole model is too coarse in through-thickness direction.

If this doesn’t work, try with explicit solver.

 

[AbolfazlYZP]

My problem solved.
Thanks for your help