Elements have distorted excesivelly 1

[AleksaBgd94]

Hello everyone,

error "The elements contained in element set ErrElemExcessDistortion-step3 have distrorted excesivelly" occured.
Attached are the photos of distorted elements. The elements are really being subjected to high values of deformation and their material definition is Hyperfoam, but does anyone know how I can solve this problem and carry out the calculation until the end? The high deformation of element is expected,, but I need to carry out the calculation to the end of step?
Is mass scaling a solution ? Which parameters should be entered there?
What else could you recommend to avoid this problem?

Thanks in advance.

 

[FEA way]

Most likely something is wrong with interactions in this model (contact/tie constraints). Check dat and msg files for warnings, some of them may indicate the reason of the problem.

 

[AleksaBgd94]

I found this warning in Data file:

WARNING: THE FOLLOWING SLAVE NODES INVOLVED IN *TIE,ARE WITHIN
COMBINED MASTER AND SLAVE THICKNESS AWAY FROM THEIR PROJECTION POINTS
ON THE MASTER SURFACE. THE COORDINATES OF THESE NODES HAVE THEREFORE
NOT BEEN ADJUSTED.

But it is still not clear to me what can be the problem... Do you have any idea?

Thanks

 

[FEA way]

I think that this distortion might be caused by incorrect adjustment of tie constraint. Check the node sets generated by Abaqus and available in the output database. Also take a look at elements contained in set ErrElemExcessDistortion. Are they located in the regions where tie constraint was applied ?

 

[AleksaBgd94]

FEA way, thanks for the help.
It was something wrong in the model, but I am not sure what. It was possible to run and complete the calculation when I redefined the model.

 

[AleksaBgd94]

FEA way, I faced problem again with excessive distortion of elements. I run calculations of similar models and the error sometimes occurs , sometimes not. So I am really not sure what is the problem.

Elements ErrElemExcessDistortion are not located where tie constraint was applied. They actually should not have really large deformations, but can be damaged to a certain degree (even fully damaged, the material is defined via CDP with plasticity parameters). How can this problem be solved? What about distortion control or element deletion? I investigated about element deletion, but it is mostly assigned to ductile metals? My element is made of brick material (defined by CDP).

 

[FEA way]

Since Abaqus 2019 release, element deletion is possible with CDP model but only in Explicit analyses.

It’s important to determine the reason of element distortion. Here it seems that something is wrong either with boundary condition or with interaction.

 

[AleksaBgd94]

I agree. I still cant figure it out. The distorted element is part of the brick instance. It is the model of masonry infill wall and the distortion occurs in element which is part of brick. The only interaction is interaction between surfaces of bricks (nteraction definition - hard contact, tangential behaviour, cohesive and damage parameters are defined). I cant see a place for mistake in interaction definition :/

 

[FEA way]

Is slave adjustment enabled in contact pair definition ? Also try running the analysis without cohesive contact behavior.

 

[AleksaBgd94]

I am sorry, i am new to the software. Where can I check if the slave adjustment is enabled in contact pair definition? I am running analysis in Abaqus / Explicit. Attached are the contact properties I have defined.

 

[FEA way]

Slave adjustment settings can be found in the Surface-to-surface contact interaction editor (Interactions --> contact_interaction_name --> Edit).

 

[AleksaBgd94]

I have defined interactions by individual contact propert assignment. I have general contact defined and then individual contact property assignments which overwrite the general contact. I havent defined surface-to-surface contact. (Attached)

 

[FEA way]

In such case it would be best to check whether the excessive element distortion occurs when cohesive behavior isn't included in the model. Based on your picture it appears that these distorted elements stick to another part and are stretched by it. Seems that contact isn't working properly in this model.

 

[AleksaBgd94]

Dear FEA way,

I think that you described my problem right.
I ran calculations without cohesive behaviour and damage parameters defined in contact definition and it was possible to complete the calculations.
Can an overlap of parts be an issue in this problem?

Thanks and regaards

 

[FEA way]

Yes, you should eliminate any significant initial overclosures. General contact algorithm with default settings may not be able to properly adjust large overlaps.