Unknown Error Occurred During Solution

Hello,

I am running a static structural simulation of an animal's upper airway. I am applying a pressure on the airway walls and I am checking at which pressure the walls come into contact using the Contact Tool (Gap) in the solution. For more details about the model please refer to the discussion below.

I have added more bodies to the geometry shown in the previous discussion and I need to increase the number of substeps to 1000 because I need 4 digits of precision to determine an accurate pressure value. For a low number of substeps (15) the model is solving but when I increase the number of substeps I am getting an error ("Unknown Error has occurred").

I've attached the content of the Solver Output.

Could you please help me understand the reason behind this error and if it can be solved by using a different, more powerful computer.

Thank you for your help.

Best regards,

Diane

Comments

  • Hello again,

    I thought it would be helpful to add some screenshots of the Newton Raphson Residual Force.


    Best regards,

    Diane

  • Gary_SGary_S Forum Coordinator

    In the solve.out, it tells why the solution has stopped.

     ************************************************************************

     The number of ERROR and WARNING messages exceeds 10000.         

     Use the /NERR command to increase the number of messages.        

     The ANSYS run is terminated by this error.               

     ******************************************************************


    If you look further up in the solve.out, I see this same warning repeating over and over...

     *** WARNING ***             CP =   18.453  TIME= 13:03:08

     SURF153 element 14344 has more than one solid element underneath it.   

     Since KEYOPT(3) = 10, this element will be dropped. 


    When you increase the number of substeps, this error is then issued many more times (per substep), and the solve is stopped.


    Adjusting the number of errors/warnings with /neer is not a good idea at all.

    We need to find out why the warning is being issued, and resolve it.

    It seems like you may have multiple boundary conditions applied to the same feature.

  • Hello Gary,

    Thank you for your response.

    Is there a way I can get more details on this warning that keeps repeating? Can I know which is SURF153 for example?

    Best regards,

    Diane

  • Gary_SGary_S Forum Coordinator

    I cant be 100% sure, but here are some clues:

    The warning "SURF153 element XXX has more than one solid element underneath it. . " seems to indicate that you have applied a load at

    an intermediate surface between bodies. Imagine a simple 2 cube model with contact between the cubes, then also applying a force on the mating contact face.

    We need to find the element numbers that are affected.

    Process of elimination would be my first suggestion. Try the run with minimum boundary conditions. (Like a fixed support and a pressure). Add/suppress conditions/contacts/parts back in until the warning recurs.

    Another method: The warnings give an element number. You can use the Named Selection worksheet the select an element by number or range of numbers.



  • Hello Gary,

    Sorry for the delayed reply. Thank you very much, your comments were really helpful.

    For now, I got rid of the issue by just increasing the number of warnings or errors with the /NERR command but I will look into getting rid of the warning later when I optimize the model.

    Thanks again!

    Best regards,

    Diane

Sign In or Register to comment.