2012 Plasticity- "Severe 24 End of file error"

[Anonymous]

Hi All,

I have a simple model of a plastic hemisphere that I am loading with prescribed displacements. Element definition uses Von Mises with Isotropic hardening. During the run my model begins to deform plastically, but the run never finishes. The simulation always crashes with a "forrtl severe 24" error "end of file during read..."

I have tried changing a lot of settings, boundary conditions, loading, time steps, convergence, and depending on my settings the run is either faster or slower. However interms of displacement, the run always crashes  around the same value (to within 20%).

Any thoughts?

Just to confirm, I have also tried running this model on multiple machines, to no avail.

Thanks,

Abishek

[zhuangs]

Are you using Windows Vista?  If yes, turn user account control off to see whether it helps.

And what's the nunit number following the error?

-Shoubing

[Anonymous]

I am using Windows7.

The message box pops up saying the run was finished with one warning. But the monitor shows the following error

"forrtl:  severe  (24) : end-of-file during read, unit 24, file C:\............

I have attached a screen shot of the error. Hope it helps.

Thanks for your response.

Abishek

[Anonymous]

Just confirm, the user account control settings have been modified to "never notify". The error came up in spite of this UAC change.

[zhuangs]

The error happens in a file related to contact.  It seems that the slow convergence process results in the access issue of the file.  You can provide the model to investigate the divergence problem.

Shoubing

[Anonymous]

Can I email the file to you directly?

[zhuangs]

You can send the model to my Autodesk email.

Shoubing

[Anonymous]

For some reason when I send a private message to you (assuming it goes to your autodesk email) I am not able to attach the ach file.

Can you give your office email id? You could email me at abishek20@gmail.com

Thanks,

Abishek

[zhuangs]

Hi Abishek,

I investigated your model.  The divergence of the model results from Part 3, which has two problems:

1. Part 3 should have two surface boundary conditions resulting from symmetric conditions (one quarter of the model is used), like part 1 and part 2.
2. One layer of brick element is not enough for the compression deformation.  Considering its much higher Young’s modulus, I changed it from Brick element to 3D Kinematic element.

Once you fixed the two problems, you don’t need so small contact stiffness for contact pair.  Thus, I made some other changes to the element settings of part 1 and part 2, contact settings of the two contact pairs, the total number of time step from 500 (don’t need so many steps) to 50.  After that, the convergence is great, always on step level of 1.  The modified model has been sent to your email.  However, the deformed shape found two more problems (which you can fix):

1. Part 1 has too coarse mesh, which cannot well support its so large deformation.  The figure sent to your email shows this problem.  I would recommend finer mesh be used (at least 5 times more elements).
2. The contact pairs are not well defined.  I would like to define just one contact pair:

the bottom (along z-direction) surface  of part 3

with

the sphere surface of part 2

I am quite sure, once you fix the mesh of part 1 and refine the two contact surface, the model can both run well and provide good solution.

Shoubing