General Mechanical

General Mechanical

ERROR IN ELEMENT FORMULATION

    • Rana Nasser
      Subscriber

      Hi everyone,


      I'm solving a nonlinear transient analysis on a structure with normal and tangential elastic support boundary condition on some faces and fixed support boundary condition on some other faces and the transient load is a base excitation acceleration. after 6 hours of solving the solution have terminated due to an error. In the solver output, this was the only error I have found "ERROR IN ELEMENT FORMULATION". there are 7 warning also as shown in the solver output attached below.


      Now I need to know how to determine the element using the element number that used in the solver output? then is there any inspiration to solve this error??!


      Regards,


      Rana  


       

    • Sandeep Medikonda
      Ansys Employee

      Hi Rana,


      If you are using version 19 or above you can hit the 'M' key on your keyboard that should bring up a dialog box to insert an element number. For any previous versions, you can create a named selection of the element or element set to review.


      I would also look at the force convergence plot and more importantly the newton-raphson residuals. Look at where they are high? Please see this discussion.


      Regards,
      Sandeep
      Guidelines on the Student Community

    • peteroznewman
      Subscriber

      @Sandeep, here is the Solution Output from the attached zip file.


      There were some converged substeps, then Element 18862 failed to compute valid data in the material model for material 21.


              >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   2
      *** LOAD STEP 1 SUBSTEP 143 COMPLETED. CUM ITER = 440
      *** TIME = 0.708500 TIME INC = 0.175000E-02
      *** MAX PLASTIC STRAIN STEP = 0.5112E-02 CRITERION = 0.1500
      *** RESPONSE FREQ = 2.203 PERIOD= 0.4540 PTS/CYC = 0.26E+03
      *** AUTO TIME STEP: NEXT TIME INC = 0.26250E-02 INCREASED (FACTOR = 1.5000)

      FORCE CONVERGENCE VALUE = 0.4598E+08 CRITERION= 0.1207E+06
      DISP CONVERGENCE VALUE = 0.1605E-02 CRITERION= 0.3587E-03
      EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.1605E-02

      *** WARNING *** CP = 21703.891 TIME= 07:47:27
      The material solution failed for element 18862 with material 21.
      *** LOAD STEP 1 SUBSTEP 144 NOT COMPLETED. CUM ITER = 442
      *** BEGIN BISECTION NUMBER 1 NEW TIME INCREMENT= 0.10000E-02

      FORCE CONVERGENCE VALUE = 0.1116E+09 CRITERION= 0.1630E+06
      DISP CONVERGENCE VALUE = 0.8779E-03 CRITERION= 0.3587E-03
      EQUIL ITER 1 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 0.8779E-03

      *** WARNING *** CP = 21749.844 TIME= 07:48:13
      The material solution failed for element 18862 with material 21.
    • Sandeep Medikonda
      Ansys Employee

      Thanks Peter


      @Rana: Look at the strain in the failing element. If your stress-strain response is not being defined to this extent, please extend it in engineering data.


      Typically Element Shape distortion can occur due to:



      • Excessive strain

      • Volumetric locking (PLESOL,NL,HPRES)

      • Hourglass modes


        • Using Higher order elements or change to enhanced strain to eliminate reduced integration issues in lower order elements.

        • However, making the offending elements linear could be an option if that approximation is acceptable.



      • Very large force un-balance


      Decreasing the initial step size may also help. 


      Regards,
      Sandeep

    • Rana Nasser
      Subscriber

      Thanks so much Peter.


      @Sandeep: Thanks for your attention, I tried the "M key" method to find the element, but it didn't work. I hit the M key and changed the selection from node to element then pasted the element number and hit select then hit create name selection, but the named selection was created without any selections! 


      I have already changed the initial time step from 0.001 to 0.0005 and solved the model again but I have the same error.


      The attached images below shows the force conversions and displacement conversions for the second trial and the solver output is also attached.


      note: the failure occurred again because of the same element.   


       

    • Rana Nasser
      Subscriber

       There is also another question How can I know which material is material 21?

    • Rana Nasser
      Subscriber


      The previous pictures was taken from the model before changing the base excitation file and resolve the model (it was a solved model then I made a save as file to make some changes then i tried to solve it again when the mentioned error appeared and stopped the solution)


      the first pic. appeared when I opened he file after it was solved and closed, the second one is the files from view menu.


      when I hit repair as shown in the 3 rd pic.  a browsing window was opened and I followed the location bath and selected the ".xml" file of the engineering data folder after that  the text in row 5 become black like the other rows, but when I close the project and open it again I find the same message. Also when I was trying to make an archived file a there is warning message  talks about the missing file. Is there a relation between that and the error in the previous post?       

    • peteroznewman
      Subscriber

      I know that when the Geometry file is missing, that doesn't affect the ability of the solver to run. It does affect the ability to edit the geometry. I don't think this missing file has anything to do with your error.


      The model stopped with the same error on the material: The material solution failed for element 18862 with material 21.

      If you are using a material model that has an equation that becomes undefined if tensile stress is applied to the element, then there is no solution after that point. I believe this may be happening in your model.


      I don't know how to find out which material is 21.


      Regards,
      Peter

    • psh1988
      Subscriber

      Hi Sandeep


       


      I have encountered a similar warning which resulted in the termination of my analysis . How can I look at the strain in the failing element? it is worthy to note that my analysis is static structural. I am applying an acceleration to my slope model.

    • ahmeddabdelaal
      Subscriber

       


      Rana  


      I'm modelling an ROV Model & I was wondering If you Can help me I'm doing it for my graduation project thanks in advance <3


      Ahmed.abdelaaaallll@gmail.com


       


Viewing 9 reply threads
  • You must be logged in to reply to this topic.