General Mechanical

General Mechanical

Convergence error when including nonlinear material properties

    • Afneer Raghon

      Hello everybody,

      I am gonna brief all the steps for the analysis so there will be no info gap between us I hope. I'm reading this forum quite some time and want to give clear information to admins, specially dear Sandeep and Peter, who are helping us a lot. So lets jump in.

      I'm analyzing a steel transmission tower considering geometrical and material nonlinearity with imperfections (GMNIA) in ANSYS Workbench R16.2. The model consists only line elements (BEAM188). Firstly, Linear analysis is conducted (static structural) considering no imperfection, no large deformation and linear material properties and reasonable results are obtained. The tower meshed as 20mm. After that Linear Buckling analysis (Eigenvalue Buckling) is performed and buckling shapes are determined. From the buckling shapes that created after the analysis, 3rd buckling shape is selected as a initial imperfection shape for the nonlinear analysis. The last step is Nonlinear Analysis in the project schematic as you can guess. For the nonlinear analysis the 3rd buckling shape is used by scaling 1/1000 amplitude with proper command (UPGEOM). In the nonlinear analysis first geometrical nonlinearty with imperfections (GNIA) is performed, large deformation is set to ON, Stabilization ON and Automatic time stepp?ing ON. After the analysis reasonable results are obtained (No warning or error displayed). After this step material nonlinearity is intrudeced to the system with Bilinear isotropic hardening model. In the tower all members have same steel properties by the way. In the bilienar model Yield stress is set to 290 Mpa and Tangent Modulus is 2100. Note that the max compression and tension stresses values obtained in Linear analysis is 286Mpa and 188Mpa. 

      Now we come to problem. When the nonlinear material properties are introduced to the model, solver couldnt converge, no matter what I do. The error says: ''The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.''

      *** ERROR ***                           CP =     372.328   TIME= 143:48
       The value of UX at node 68552 is 1.202965934E+39.  It is greater than  
       the current limit of 1.E+30 (which can be reset on the NCNV command).  
       This generally indicates rigid body motion as a result of an           
       unconstrained model.  Verify that your model is properly constrained.  

       *** ERROR ***                           CP =     372.344   TIME= 143:48
       Rigid body motion can also occur when net section yielding has         
       occurred resulting in large displacements for small increments of load 
       or when buckling has occurred.  You can plot the time history curve    
       for node 68552 in the UX direction to check for stiffness (slope of    
       the curve) approaching zero

      I dig the forum to solve this. I changed and played a little with initial/max/min loadsteps, made the mesh finer no change. I used share topology on geometriy model no change. Then I used Node merge group, no change. I looked up the Newton-Raphson Residuals and got ''a member'' with high residual. Also note that whenever I made some changes, 'I 've got different member with high residuals. So thats strange i guess.

      To sum up I am stuck with this problem. I hope we can solve this issue. I'm posting some pictures to represent the situation.

      Thank you,

      A. Raghon.








    • peteroznewman

      Afneer, thank you for a nearly complete post.  Sorry I missed this the first time.

      The solver makes good progress with many converged substeps up to a time of 0.6875 in this nonlinear buckling solution.

      The only item missing from your post is the loading definition.

      In a nonlinear with plasticity buckling solution that is loaded with force, it is quite normal for the solution to fail to converge at the point where the structure has reached the critical buckling load when the next load increment results in collapse. You just don't get to see that.   In models loaded with displacement, it is possible to continue solving into the post-collapse domain.  In models loaded with force, sometimes stabilization can achieve convergence in the post-collapse domain.

      The clue that the solution has reached the point of collapse is that the force-displacement curve approaches a zero slope. Plot that curve and see if that is the case. If so, you have successfully identified the critical buckling load.  If there is a significant slope, then a numerical problem has stopped the convergence.


Viewing 1 reply thread
  • You must be logged in to reply to this topic.