mesh problem

[Chen1]

I am modeling a uni-axial compression test for a rock sample using concrete damage plasticity approach, i found when the element size is 0.1 the model diverges while when the element size is 0.15, there is no divergence problem and the model reaches equilibrium.

the size of the mode is 2 in x 2 in

anybody has an explantion for that.

 

[Chen1]

is there any idea about why the model diverges when the element size is smaller.

i expect the model diverges when the element size is bigger.
Thanks

 

[burningDiesel]

Probably your element quality is lower.

 

[Chen1]

what do you mean by element quality is lower? you mean i am using linear element not second order element?

 

[burningDiesel]

No, I mean the shape of the elements, in the mesh module, click "verify mesh" and inspect the aspect shape, angles, etc.

 

[burningDiesel]

No, I mean the shape of the elements, in the mesh module, click "verify mesh" and inspect the aspect shape, angles, etc.

 

[Chen1]

I checked the element quality and no problems, no warning messages, by the way i used C3D8R, which is 3-dimension hex element reduced integration.

Thanks for your advice.

 

[burningDiesel]

Although they are not bad enough for a warning, it can still be that they are worse than they were for the larger mesh.
in tools -> job diagnostics you can see where exactly the problem is in your simulation i.e. what element(s) is giving trouble.

 

[Chen1]

I use only one type of element which is C3DR in the whole model, and the element size is the same everywhere in the model, so they are bricks of the same size. usually the job continue up to 60% then it starts to diverge

 

[Chen1]

Ｉ sent you the CAE file, i have Abaqus 6.12.

The model is just uni-axial compression test for rock sample, i used static general approach.

you can see that the element size for this model is 0.25. when i try to make element size smaller (0.1) the model diverges, i do not know why. please try to help me.

Thanks

 

[Chen1]

And this is the jnl file.

 

[Chen1]

Sdebock,

I sent you the CAE file, you can see that when the element size is 0.25 the model converges, while if you change it to 0.2 for instance, it will diverge.

could you please help me, i need to understand why this happens and i need to use finer mesh in my model.

Thanks.

 

[burningDiesel]

I don't know enough about the material model & damage you are using to comment.
I would not dismiss it as being a mesh problem, are you sure your material data is correct?
Try solving the compression using boundary conditions (vs the contact you do now) first.

 

[Chen1]

Hello Sdebock,

I took you advice and solved the model without the contact. i applied the load directly to the model, it works and and the mesh problem disappeared. That means that the contact was the main cause for the problem.

However i need to apply with contact.

So you helped me to know that the contact between the rigid platen and the coal sample is the main cause of the problem.

what should i do next?

Thanks.

 

[burningDiesel]

I would try to run it using contact, frictionless, so we can determine if the shear stresses from friction are the culprit. To aid in contact convergence, use penalty contact, and scale down the penalty stiffness.

 

[Chen1]

Hello Sdebock,

When i run the model with friction-less contact, in Abaqus viewer, i do not see the rock sample, i think since this friction-less model, the rock sample slides out of the rigid platens. so what i did is just remove the rigid platens and apply the load directly to the rock sample, i believe this is equivalent to the friction-less model. I did not find any problem with the model, no warning message, no error.

When i run the model again with contact, the rigid platen moves 0.02 inch & element size = 0.1 and the coefficient of friction = 0.1. I got many warning messages and the model diverges. this is an example of the warning messages:

The plasticity/creep/connector friction algorithm did not converge at 2 points

The plasticity/creep/connector friction algorithm did not converge at 1 points

The plasticity/creep/connector friction algorithm did not converge at 56 points

The plasticity/creep/connector friction algorithm did not converge at 21 points


While when i keep the load as it is an changing the element size from 0.1 to 0.2, the model converges.

Please note that, if i want to increase the load (increase the displacement of the rigid platen from 0.02 to 0.03 in), i have to increase the element size again.

I wish you understand my problem.
Thanks for helping me.

 

[burningDiesel]

you have to fix one of the nodes (better 1 edge) in the transverse direction!

 

[Chen1]

Hello Sdebock,

You mean i have to fix on of the nodes of the deformable rock sample, right? You know i am testing this rock sample between two rigid platens, one of them is fixed and the other one can move only in the vertical direction to apply the load.

So you want me to fix one node for the rock sample?

thanks

 

[burningDiesel]

yes, if you are compressing in Z-direction, fix at least 1 node in X and Y, but you better do the 2 planes (parallel X and Y resp.), because with only 1 node you can still rotate.