*D4TRI WARNING* Sign of diagonal changed when reducing

[butho]

Hello everyone,

I'm working with pressure elements in the case of a contact. It appears that when high level of refinement is used I get this warning. n1=80 n2=48 converges without warnings while i get one warning at the first step fourth iteration for n1=120 n2=72. For information, vonmises_max should reach 2609MPa at (0,5.14).
 
I read that this indicates a singular system of equations. I checked the boundary conditions (specially the use of axisymmetric and pressure element, in a file attached Itest.f90), the mesh looks fine and the load is applied slowly with delta_t=0.01.

I guess the solution command is not appropriate in this case (I tried other methods from the manual but this one is the most convicing), or the contact description needs some amelioration (solm penality ?). None of my tries seem to affect this warning.

Does anyone have some leads I could try ?
Please find the input file Ihertzaxisym2d.f90 attached.
Thank you for your time,
Thomas

version 8.4.1

[Prof. R.L. Taylor]

The warning only gives information that the tangent stiffness is not positive definite.  In the case of a finite deformation problem this warning could be telling you that the system is becoming unstable and you have passed a point in which the load path could change.  Also, when you use a follower force the equations may be unsymmetric and you should use UTAN instead of TANG.  Does the warning persist if you turn off the follower loading?  My guess is that the deformations

[butho]

Thank you for the quick reply Professor.

The warning persists if the follower loading is turned off. It also persists with UTAN.

My guess is that the deformations

I can't see the second part of the sentence, and I'm sure it will help me

Thomas

[Prof. R.L. Taylor]

I am assuming the deformations are creating a state in which some form of "buckling" might be possible.  Does it converge?

[butho]

Nothing indicates that it converges.
What bothers me is that the maximum vm stress evolution is not increasing. I checked the residual norm evolution and it is constant **e-9.

From what you said, maybe I should start the calculation with an "interference fit" state ? The mesh of one block penetrating with the other (0.005mm, less than one mesh) to avoid these deformations ? I'm not sure it could work with the applied load..

[Prof. R.L. Taylor]

I assume you are running the axisymmetric problem.  I did run it but used the Pardiso solver because the profile was slow.  It seemed to run fine but the contact area is very small and very few nodes are in contact.  One thing I would suggest is to grade the mesh so the contact region has small elements but the rest is larger, you should not need so many elements to run this case.

The residual norm is about what you say but the energy norm was satisfied so it is considered to be converged.  Since you use pressure load, there are no boundary conditions on the disk, thus if feap ever things it is not incontact you will have a singular system.  If you restrain the disk and load by slow displacements you would not have this and it would be stable.  You will have to recover the load from the sum of residuals on one of the faces (there is an option to do this in tplot).

[butho]

Thank you for these suggestions !

Yes it is slow .. I tried different meshing options but if i am not wrong, as I use POLAr command in the contact options for the ball, I need to define the disk quater by the same command or feap can't recognize the surface.
This kind of error will appear  *ERROR* CRSURF: Multiple segments on surfaces. Correct by using TIE for surface area.

I got the same error message contact surfaces defined by tied blocks edges. I still have to work on the mesh.

I knew that using loads instead of displacement would be challenging in this case but I guess displacements are safer !