Convergence issues

[maheshh]

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

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

 

[Stringmaker]

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.

 

[maheshh]

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.

 

[maheshh]

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

 

[maheshh]

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.

 

[Stringmaker]

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?

 

[cbrn]

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

 

[maheshh]

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.

 

[doatis]

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