aborted with system error code 1073741819 1

[Ajith Kurian Baby]

I was trying to simulate a wear problem with mesh motion subroutine. the job ran for 1 increment after which it aborted with an error. I refined mesh with coarse size but still showing error. please help me to rectify this issue.

The executable standard.exe aborted with system error code 1073741819. 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.

 

[FEA way]

Can you attach msg, dat and sta files ? They may contain additional error and warning messages showing the actual reason of the problem.

 

[Ajith Kurian Baby]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1586145789/tips/Data_file.jpg_foogga.txt[/url]

 

[Ajith Kurian Baby]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1586145839/tips/msg_file_ct1b0y.txt[/url]

 

[Ajith Kurian Baby]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1586145870/tips/status_file_qzrfgz.txt[/url]

 

[Ajith Kurian Baby]

pls find the attached files

 

[FEA way]

Unfortunately these files don’t indicate the actual reason of the error.

Try running this model without subroutine. If you still get this error, disable adaptive meshing. If this doesn’t help, there’s probably an issue with features such as contact and constraints (ties, couplings).

 

[Ajith Kurian Baby]

When I disable subroutine it runs fine. Even when adaptive mesh is turned on .
In this problem i have two solid blocks in relative motion.
I am giving adaptive mesh to the lower body and for the same body iam specifying displacement in z direction using periodic boundary condition and arresting x and y dofs(rotation and displacement) , (rotation in z direction also). For top body iam giving pressure load only by restricting displacement in x and z direction. All boundary conditions and loads are specified using boundary condition manager.

Is there any mistake in specifying my boundary conditions?
There are no ties or coupling in this problem. It is held together by pressure load and friction contact is specified by defining master and slave.

 

[FEA way]

If these boundary conditions/loads are assigned to the top surface of the upper block and bottom surface of the lower block then it seems correct.

Apparently there’s a problem with your subroutine code.

Check the article "Material removal analysis for compliant polishing tool using adaptive meshing technique and Archard wear model" by A.P.S. Arunachalam et al. It may be helpful.

 

[Ajith Kurian Baby]

Pressure was applied on top of the top block and entire top block was given restrictions for x and z direction motion .
Entire bottom block was given z direction motion whereas bottom surface was given restrictions in dof in other directions.
Thanks for your reference suggestion.

 

[FEA way]

I think that it would be better to apply all constraints to the surfaces, not to entire blocks. The interface region should be left with contact only.

 

[Ajith Kurian Baby]

When I try to apply constraints to surface only, its showing error."too many attempts made for increment"

 

[FEA way]

That’s a typical convergence issue. It might be caused by rigid body motions occuring before the contact is established. Especially that you use load control. Try adding automatic stabilization or contact stabilization.

 

[Ajith Kurian Baby]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1586170845/tips/msg_file_dii6qt.txt[/url]

its showing excessive distortion even after switching automatic stabilization.

 

[FEA way]

Can you attach a picture showing this model (with boundary conditions and mesh visible) ? Or, even better, please attach its files (cae or inp) if possible.

 

[Ajith Kurian Baby]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1586171754/tips/reciprocation_periodic_static_model2_lrsqwo.cae[/url]

 

[Ajith Kurian Baby]

attached pics shows modified boundary condiitons

 

[FEA way]

Yes, the boundary conditions should look like in your picture.

Slave surface should be the one with finer mesh. And you may have to increase the mesh density for the whole model, especially for the region with adaptive meshing assigned. I would apply this feature only to the layer of elements close to the interface.

 

[Ajith Kurian Baby]

Mesh density was modified. slave surface was given highest mesh density.
I tried with the above boundary conditions. But it didn't worked . Always job is getting aborted even without ALE. But if I specify motion to the entire lower body and constraining other dofs of bottom surface of lower body, it will move in the periodic manner as specified.
I tried in different ways to avoid giving motion to entire body but it didn't worked. Even tried to give motion to upper body (along with pressure) alone by encastring bottom surface of lower body.but it also failed.

Iam specifying user defined adaptive mesh constrain only to top surface of lower body. Is it the correct way?

 

[FEA way]

I modified Model-2 in the database that you shared here:
- turned off the remeshing rule
- applied boundary conditions to faces instead of entire blocks
- switched surfaces in contact definition
- changed initial increment size to 0.1

And it works now. However the mesh should be refined anyway.

Yes, apply this constraint only to the surface nodes.