warning: There are 11 unconnected regions in the model

[HalaD]

Hello,
My goal is to model a brick wall in Abaqus/standard,
I started by a static simulation using 2D elements where 4 bricks(4 rectangular elements) were placed as fig.1 shows and a surface to surface contact was created between them(cohesive and friction properties)
I created two steps one to add gravity load and the other to apply horizontal displacement at the edge of the upper brick. after that I tried to add more elements to test if it's working(fig.2).
when I have this warning: There are 11 unconnected regions in the model, the job is aborted immediately form the first step with an error: Too many attempts made for this increment.
this warning is due to the horizontal interaction between the bricks. I tried an other time to simulate just the 4 elements (fig.1) by creating another model(the warning disappeared and the simulation was completed, I didn't know the difference between the two models, I did the same steps each time), the other simulations didn't work at all.
I checked every thing but I didn't resolve this problem. Mention that all the simulations are working with implicit method without any problems.

Any help, please.

 

[Erik Panos Kostson]

It is hard to say why without getting some more details.

Since you have the results from the implicit dynamics, have a look at these results, and see if the blocks are staying where there are suppose to stay or if the are taking off, flying away somewhere (rigid body motion can be solved of course in implicit dynamics but not in statics, without inertia relief at least)?

In general:
Is this happening for both load cases or just the horizontal one?

If that is the case, not sure how you restrain the model? and the interaction, perhaps there is not enough friction to prevent them from sliding away (this would be confirmed by looking at the implicit run)?

 

[HalaD]

Thanks for your replay.

In fact the implicit dynamics is running very well, and the blocks stay in there place(I applied a small displacement). I tried also to perform an implicit simulation by applying cyclic load for a whole wall, and the behaviour is normal, the wall swings with each displacement.
I am sure that the problem in static is caused by the interaction between the blocks(I tried to replace the interaction with tied constraint and it worked).
The parameters are realistic and verified by the response of the implicit simulation.
The job is aborted at the first time step of the gravity loading.

I want please to know the meaning of the warning, I didn't find any clear explanation about it,maybe it can solve the problem.

 

[Erik Panos Kostson]

It seems then that the contact is not working/activating as it should in statics.

Try to put some small horizontal restraints (gravity step) that can be removed in the second step when you add the horizontal load. This is to let the model develop some stability and to prevent rigid body motion. Alternatively apply local dash-pots/springs on nodes that will also help to stabilise it.

Try that and see how it goes.

 

[HalaD]

I tried but the it's the same, the job is aborted

 

[Erik Panos Kostson]

It is definitely the contact that is not working and that there is rigid body motion (the warning of unconstrained bodies you get in situations with rigid body motion), that you need to resolve. For instance move bodies in the assembly so that they are touching, if you do not do that and there is a gap between the blocks, you then need to add an adjust slave nodes in set in your contact and under the slave adjustment tab of the interaction edit tool (for every interaction defined). Also look on the direction of the gravity and the restraints.

 

[HalaD]

I tried to apply the slave adjustment on the horizontal interaction between the bricks, nothing changed.
I attached the .cae file here if you can check it please.

 

[Erik Panos Kostson]

Do the adjustment on all the interactions (also the vertical, that is in the vertical/gravity direction)

Well at least you can solve it with the implicit solver.

I will try and open it (have an old demo version, node limited, so must of the times I can not), that is next week.
(In my everyday work I do not use abaqus, I use Strand7, used abaqus some long time ago for research-feeling old now )

Have a good one

 

[Erik Panos Kostson]

Here is the problem.

The interaction in the model you attached is created in step 2, and is thus not active in step-1 when the gravity and the pressure is on (hence the rigid body motion). Just move it to the left in the interaction manager so it becomes created in step-1 and propagated to step-2 (I had also to mesh with linear elements and non reduced integration because of the node limit)

This will solve until the hor. load is too large (about middle of step-2), and you have to much damage. If you remove the damage, then it solves for both steps.

this is it for me (have done to much support this past week so I am looking forward to not doing any of that).

Have a good weekend -

 

[HalaD]

Thanks Erick,

You helped me a lot, I performed a simulation for the whole wall and I solved the problem by introducing the adjust slave node option as you mentioned to me before.