COMPRESSION AFTER IMPACT: https:// 1

[Vishwanna]

COMPRESSION AFTER IMPACT:

https://www.eng-tips.com/viewthread.cfm?qid=459632#post

Dear All, Using the above thread, I have tried compression after impact ANALYSIS several times. Impact analysis is done for a laminate using local-global approach for a 32 layered laminate with impactor having 5.2kg at a velocity of -2.4m/s. For Compression after impact analysis, I know the boundary conditions. But when I imported the whole model using File-import-model-relevant odb file and through load-predefined field-initial, I deleted the impactor from PART module (please tell me deleting the impactor from part is right or wrong). And ran the simulations. The output is not considering the deformed laminate from impact analysis in the beginning. Rather it it only getting compressed. I need to run the simulation for many imperfection factors and right now I am stuck with impacted plate without any imperfection factor. Please tell me should I decrease the values of Xt,Yt,Xc,Yc and cohesive properties for compression analysis?
Kindly give me a hint so that I can complete the work. Kindly help. Thank you in advance.

 

[FEA way]

If you use the import technique properly, you can select which instances will be imported with their deformed mesh and material state from the previous analysis. To do this in Abaqus/CAE (it's also possible with keywords) follow these steps:
1) Make sure that restart data is written in the impact analysis
2) Copy the model to a new one
3) Delete unnecessary interactions and BCs together with the impactor
4) Keep the laminate and its needed features, define new BCs/loads for compression analysis
5) Use "Create Predefined Field (Step: Initial) --> Other --> Initial State", uncheck the "Update reference configuration" option

 

[Vishwanna]

FEA way (Mechanical) Thank you Sir. I will follow this and will reply soon. Thanks for your time.

Regards,
Vishwanna

 

[SWComposites]

So … when you run the “impact” part of the analysis, what do you get for deflection and damage? Have you correlated that damage state to test data (NDT scans, cross sections, etc)??

And … when you run the compression loading analysis, how are you modelling the damage ( delams, fractures, etc)?

 

[Vishwanna]

SWComposites (Aerospace), For impact analysis meaningful output will be interms of energy absorbed, contact force due to contact pressure,frictional stress and both, and of course displacement. For compression analysis I am going to make use of same cohesive modeling and hashin damage properties from impact analysis.

 

[SWComposites]

No, for impact analysis, the useful output will be the locations and extent of fiber fractures, matrix cracks, and delaminations. This must be correlated to test data before you bother to run the compression analysis.

And the compression analysis must allow for sublaminate buckling in the delaminated areas.

 

[Vishwanna]

SWComposites (Aerospace), I totally agree with you. My reply was for a beginner. Thank you Sir.

 

[Vishwanna]

Dear All, I need your help in solving the Abaqus error: 28 nodes have dof on which velocity/displacement/acceleration/base motion etc. constraints are specified simultaneously. The nodes have been identified in node set ErrNodeBCRedundantDof.
In order to solve this, first I continued with the boundary conditions in step 2. I got same error.
secondly, I made boundary conditions in step2 as inactive and created fresh boundary conditions only for step2. Still getting the same error.
Lastly I selected the nodes on which displacement loads are supposed to be applied with the help of "coupling" under Interaction->constraints and a reference point. still getting the error.

I am getting this after following all the steps suggested by above answers. Please help. Thank you in advance.

 

[FEA way]

Can you share the file ? It's hard to say without looking at the model but basically, you have to avoid defining multiple boundary conditions acting at the same time in the same directions for the same nodes.

 

[Vishwanna]

Sir this is the .inp file of CAI analysis. Please find the file in the attachment.

 

[FEA way]

Is that the correct file ? I'm not getting any errors when submitting the analysis from this input deck.

 

[Vishwanna]

Sir I checked with single precision and double precision. I am getting
28 nodes have dof on which velocity/displacement/acceleration/base motion etc. constraints are specified simultaneously. The nodes have been identified in node set ErrNodeBCRedundantDof. I don't know why.

 

[FEA way]

Which version of Abaqus are you using ?

 

[Vishwanna]

I am using Abaqus/CAE 2018

 

[Vishwanna]

Sir Which version of Abaqus are you using ?

 

[FEA way]

I'm using the newest version - Abaqus 2022 with fix packs. Perhaps the treatment of overconstraints was changed in newer versions. But if you make sure that there are no duplicated boundary conditions (acting on the same DOFs of the same nodes at the same time) then it should work also in your version.

 

[Vishwanna]

Sir I managed to get rid of the error "28 nodes have dof on which velocity/displacement/acceleration/base motion etc. constraints are specified simultaneously. The nodes have been identified in node set ErrNodeBCRedundantDof" by deactivating the displacement load of -1.75mm.
And I created new set of nodes excluding those for which I was getting errnodebcredundantdof (the corner edge nodes).
Now I am getting a new error that states "The rigid bodies with the reference nodes contained in node set ErrNodeRefNodeNoRot1Axis have atleast one axis about which the rotary inertia magnitude is zero, and the rigid bodies have atleast one rotational degree of freedom which is unconstrained. Either rotary inertia must be defined at the reference nodes or all of the rotational degrees of freedom at the reference nodes must be constrained. See the status file for further details.
Job Job-25forjob-25: Abaqus/Explicit Packager aborted due to errors."
But after importing the required parts and odb session, I checked for all the reference points for which inertia was defined. I deleted all the unnecessary sets of nodes, geometry, surfaces and interaction. Now i am getting this error.
Please tell me how to get rid of this.

 

[FEA way]

Only mass is specified for this reference node, add rotary inertia to it.

 

[Vishwanna]

Sir I fixed the error following your valuable suggestion. It is showing

"The job input file "Job-25forjob-25.inp" has been submitted for analysis.
Analysis Input File Processor completed successfully.
Job Job-25forjob-25: Abaqus/Explicit Packager completed successfully.
ERROR in job messaging system: Error in connection to analysis
The executable explicit.exe aborted with system error code 3. Please check the .dat, .msg, and .sta files for error messages if the files exist. If there are no error messages and you cannot resolve the problem, please run the command "abaqus job=support information=support" to report and save your system information. Use the same command to run Abaqus that you used when the problem occurred. Please contact your local Abaqus support office and send them the input file, the file support.log which you just created, the executable name, and the error code.
Job Job-25forjob-25 aborted due to errors."

Sir as per a youtube video

https://www.youtube.com/watch?v=ZTEMySxOjho,

I renamed the file mkl_avx2.dll to mkl_avx2.dll.18.0.0. Still not working. Please help. Thanks in advance.

 

[FEA way]

Are there any additional error messages in the .dat, .msg or .sta file ?