×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Convergence issues

Convergence issues

Convergence issues

(OP)
All

Am having terrible convergence issues in the model that I have set up. After days of debugging I have narrowed it down to at least the problem location.

I have a very low Youngs Modulus material (X) sandwiched between two high Young's Modulus materials : B - bottom and T-top.

The contact X-B is surface to surface bonded.
The contact X-T is surface to surface no-separation.

This is a static structural (non linear because of contact element as well as material non linearities) problem.

The material X behaves as expected till about 47% of the load (stepped loading). After that I get the following output (pasted in the end). If I look at the deformation plot, the material X cuboid is all distorted - like an explosion occuring in the cuboid :)

I know it is going to be hard for anybody to debug just with this much information, but can somebody at least give me some pointers to what I should look for in the model to fix?

One thing that bugs me is that if I make both sides of the contacts (B-X and T-X) as bonded, then it converges fine.

am in workbench environment
element shape checking is on
loading is in small steps with autots on

------------
Solver Output

     FORCE CONVERGENCE VALUE  = 0.8645      CRITERION=  2.337     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION  16
 *** LOAD STEP     1   SUBSTEP     6  COMPLETED.    CUM ITER =     31
 *** TIME =  0.475000         TIME INC =  0.112500    
 *** MAX PLASTIC STRAIN STEP = 0.2993E-01   CRITERION = 0.1500    
 *** AUTO STEP TIME:  NEXT TIME INC = 0.11250      UNCHANGED

     FORCE CONVERGENCE VALUE  = 0.4198E+05  CRITERION=  20.75    
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.1512E-02

 *** ERROR ***                           CP =   21736.016   TIME= 10:00:12
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         

 *** ERROR ***                           CP =   21736.047   TIME= 10:00:12
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         

 *** NOTE ***                            CP =   21736.078   TIME= 10:00:12
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         
 *** LOAD STEP     1   SUBSTEP     7  NOT COMPLETED.  CUM ITER =     33
 *** BEGIN BISECTION NUMBER   1    NEW TIME INCREMENT=  0.39375E-01

     FORCE CONVERGENCE VALUE  = 0.1104E+05  CRITERION=  3.929    
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2457E-03
     LINE SEARCH PARAMETER =  0.4490     SCALED MAX DOF INC = -0.1103E-03
     FORCE CONVERGENCE VALUE  =  5505.      CRITERION=  4.309    
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.3747E-01

 *** ERROR ***                           CP =   23320.703   TIME= 10:15:07
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         

 *** ERROR ***                           CP =   23320.719   TIME= 10:15:07
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         

 *** NOTE ***                            CP =   23320.750   TIME= 10:15:07
 One or more elements have become highly distorted.  Excessive           
 distortion of elements is usually a symptom indicating the need for     
 corrective action elsewhere.  Try incrementing the load more slowly     
 (increase the number of substeps or decrease the time step size).  You  
 may need to improve your mesh to obtain elements with better aspect     
 ratios.  Also consider the behavior of materials, contact pairs,        
 and/or constraint equations.  If this message appears in the first      
 iteration of first substep, be sure to perform element shape checking.  
                                                                         
                                                                         
 *** LOAD STEP     1   SUBSTEP     7  NOT COMPLETED.  CUM ITER =     35
 *** BEGIN BISECTION NUMBER   2    NEW TIME INCREMENT=  0.13781E-01

     FORCE CONVERGENCE VALUE  =  3282.      CRITERION=  1.985    
    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.8871E-05
     LINE SEARCH PARAMETER =  0.9967     SCALED MAX DOF INC = -0.8842E-05
     FORCE CONVERGENCE VALUE  =  44.34      CRITERION=  1.773    
    EQUIL ITER   2 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.4511E-05
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC =  0.4511E-05
     FORCE CONVERGENCE VALUE  =  3.979      CRITERION=  1.804    
    EQUIL ITER   3 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.1199E-05
     LINE SEARCH PARAMETER =   1.000     SCALED MAX DOF INC = -0.1199E-05
     FORCE CONVERGENCE VALUE  = 0.5016      CRITERION=  1.840     <<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION   3
 *** LOAD STEP     1   SUBSTEP     7  COMPLETED.    CUM ITER =     37
 *** TIME =  0.488781         TIME INC =  0.137812E-01
 *** MAX PLASTIC STRAIN STEP = 0.4066E-02   CRITERION = 0.1500    
 *** AUTO STEP TIME:  NEXT TIME INC = 0.13781E-01  UNCHANGED

     FORCE CONVERGENCE VALUE  =  784.2      CRITERION=  1.793    

------------

RE: Convergence issues

What element types are you using?  Try using linear reduced-integration elements.  You may have to enter a command snippet within workbench to actually do this as I'm not sure how much flexibility it gives you in element formulation.  Also, if you take my suggestion keep in mind that you have a much more robust element for extreme deformation problems but it is also a constant strain element so if you want good stress results you will have to use a faily fine mesh in the region of interest.  If you just want to know the overall effect or displacements you can go coarser on the mesh, perhaps even the mesh you have no is suitable for this.

Hope this helps.

RE: Convergence issues

(OP)
Thanks for the response. I am trying to figure out how to add a code snippet to force reduced-integration elements.

On your suggestion on meshing: the only purpose of this cuboid is dis[placement effects. I am not interested in stresses. I have tried many different meshing strategies (coarse, fine, sweep, hex, tets), and all have failed. It gives me erratic deformation along the edges of the cuboid.

I will update once more if I figure out how to add the code snippet in the Workbench.

Thanks again.

RE: Convergence issues

(OP)
If I turn Large Deflections, OFF, then it converges, but the deformation results for the cuboid do not make sense -

RE: Convergence issues

(OP)
Since I have not heard from anybody on this issue, here are a few pictures to describe the setup:

picture 1 shows the properties for the all three cuboids, and the center cuboid is the one showing erratic deformations. The top side contact is no separation and the bottom side is bonded.
http://farm3.static.flickr.com/2280/1579396241_91710387d0_o.jpg

picture 2 shows the deformation of the center cuboid.
http://farm3.static.flickr.com/2175/1580289700_344c7985c2_o.jpg

thanks.

RE: Convergence issues

Considering how your modulus of one material is five orders of magnitude different than the other at a bonded interface doesn't surprise me that you're seeing problems.  This is tough to diagnose remotely but if it were me I would try and use a common mesh size at the interface.  Secondly, you're going to have to cut your time-step drastically.  If you're performing a large deflection analysis you will get very bogus results using small deflection theory...so turn large deflections on.  What material models are you using?

RE: Convergence issues

Hi,
yes, I also believe that the problem is at the contact interface. More specifically: the computed "contact stiffness". Being the two "E" far different, the C.Stiff. can be computed so that it won't mutually restrain the contact nodes against the target ones.
I think Stringmaker's suggestion is the best you can try: have compatible meshes at the interface (merge nodes at the interface, or VGLUE the volumes), and get rid of the contacts. OK, you'll loose the ability to easily compute contact pressure and contact force, but at least you'll have some results...

Regards

RE: Convergence issues

(OP)
Gluing the volumes is what came to mind first but since I have moved to WBE I have not figured out the best way to do it. In Classic it was pretty straightforward.

Let me try it using named selections and vglue in Commands snippet. Anybody has done this before?

Thanks.

RE: Convergence issues

You can't glue in Simulation, because there *is* no geometry.  All that gets passed to the solver is nodes and elements.  If you look at your output file (or use Tools > Write ANSYS Input File), you will see that your named selections get passed as either nodal or element components.

If you want to glue your bodies together, bring your geometry into DesignModeler and use the 'Form New Part' tool.  This will create a continuous mesh between your parts.  

Hope this helps,
Doug

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources