Failed convergence SOL106 nonlinear static 1

[adamas]

I am doing nonlinear static analyses with NX Nastran (SOL106) on a FE model of a wingbox made up of CQUAD4 and CBEAM elements. The loads are nodal forces and moments.

The analysis is often not converging and I get this error message:

*** USER INFORMATION MESSAGE 6194 (NCONVG)
*** STOPPED ITERATIONS DUE TO REACHING MAXIMUM ITERATION LIMIT WITHOUT CONVERGENCE ***
*** USER INFORMATION MESSAGE 6193 (NCONVG)
*** MAXIMUM NUMBER OF BISECTIONS OR MINIMUM LOAD STEP HAS BEEN REACHED.
*** USER FATAL MESSAGE 4551 (NCONVG)
*** STOPPED PROBLEM DUE TO FAILED CONVERGENCE

This happens more frequently when I increase the magnitude of the applied loads. Another warning I get, that I guess could be a reason for the failed convergence, is related to the singularity of the stiffness matrix and the degrees of freedom listed afterwards have all negative values for MATRIX/FACTOR DIAGONAL RATIO:

*** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .
THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.
^^^ USER INFORMATION MESSAGE 9004 (NLSTATIC)
^^^ FOR THIS ITERATION, THE DIFFERENTIAL STIFFNESS WILL BE IGNORED TO AVOID DECOMPOSITION OF A NON-POSITIVE
DEFINITE STIFFNESS MATRIX.

The only way in which I managed to run the analysis is by increasing the K6ROT from 100 to 1E7, but this changes dramatically the results.

Have you ever had such problems? Do you have any suggestion or help on what could be the causes?

Thank you.

 

[Tuw]

Hi adamas,

Some suggestions:
1. Try to toggle around the load magnitude, since u mentioned reduce the load will have better chance of convergence.
2. Try to reduce the nonlinearities complexity of your simulation model, or add the nonlinearities gradually (1 by 1). For example, if you have 3 contacts, try to use 1 contact definition first. If it converged, then add another definition. If your contact involve a large quantity of elements, try to reduce the number of elements.
3. When it says singularity of the stiffness matrix, please check whether in the F06 file it has mentioned the grid/node ID where this problem happens. After knowing which ID, check your model for that particular node, for any potential modeling error.

Good luck,
Tuw

 

[Bopeco]

I have a similar problem on a beam subjected to bending, the nonlinear solution (SOL106) fail to converge.
In my simulation i guess i have problems with buckling or crippling, maybe you should consider that

 

[adamas]

Thank you for the answers.

Actually there are no contacts in the model. The nonlinearities are just geometric nonlinearities activated by PARAM LGDISP 1.
I checked the F06 and the grids with negative MATRIX/FACTOR DIAGONAL RATIO. However it's not a specific area of the model, but these grids change throughout the different iterations of the solution or with a different load magnitude (but same distribution).

I run as well linear buckling analyses (SOL105) with the same loading conditions applied in SOL106 and there are a lot of eigenvalues less than 1, so apparently the structure has already buckled under this load. The buckling modes are all local modes of the ribs of the wingbox.

Could this be one of the cause of the failed convergence then as Bopeco mentioned? In this case the solution, in terms of having a SOL106 which is working, would be to redesign and stiffen up the structure?


Thanks.

 

[Tuw]

It does sounds logical according to Bopeco's suggestion, and also your findings with the eigenvalue less than 1..

 

[adamas]

I tried to increase the bending moment of inertia ratio (12I/T**3) in the PSHELL cards of the elements that were buckling and this improves the convergence, even though for the higher loads it is still a problem. There are some forces with a very high magnitude applied to a single grid, do you think that using RBE3 to spread the loads on more grids could help the convergence?
What about K6ROT? Should the default values of 100 used?

 

[jbrackin]

When you see messages about failed convergence, the traditional steps to take:
1) increase number of load increments, smaller steps usually help, up to a point.
2) change strategy, if you are using the default "auto" then try "iter" and force the stiffness matrix to update more often. This is usually very helpful when large displacement is involved. Use arc length methods when you have snapthrough or need to track a decreasing load capability.

The messages about negative matrix factor diagonal are the classic symptom of buckling in sol 106. You may want to create multiple subcases where you can get results at these critical load magnitudes and see what the deformed looks like to understand the buckling behavior. It could be local buckling and your structure might continue to take more load. Also by creating multiple subcases, you can change strategy/increments per subcase to get past these solution difficulties from local behavior.

Remember that sol 106 is a load history, each subcase starts from the previous subcase results.

Another thing to remember since you mention K6ROT, if you are depending on AUTOSPC to constrain drilling DOF or any other singularity, then that could be part of your problem. AUTOSPC "does not work" in sol 106, you need AUTOSPCR,yes

See the Nastran documentation for AUTOSPC for details.

 

[adamas]

I have another question regarding the applied load (OLOAD) and SPC force resultants in SOL106.
I am applying a balanced set of loads and, as expected, forces and moments resultants in OLOAD table are close to zero. Therefore I expected as well the SPC resultants to be zero, instead they are not.
What's the cause of this?

Thanks.

 

[jbrackin]

If the SPC forces do not match the applied loads, either the solution is not converged or there is some other modeling issue. Has the model been run using GROUNDCHECK? Or have you run the model in a linear solution to check the equilibrium of applied loads and SPC forces?

 

[adamas]

Yes, I have run a linear solution with the same applied loads and constraintes and here, as I expected, the SPC resultants are zero.
The nonlinear analysis apparently converged, the tolerances EPSP and EPSW are below the threshold.
Could the cause of this mismatching be the fact that the loads applied are follower forces and moments (i.e. FORCE1 and MOMENT1)?
Or this should not have anything to do with it?

 

[jbrackin]

I believe the follower force and moment are likely the issue. I would need to do a little testing to be sure.
The OLOAD resultant in the fo6 is before the structure deforms.
Have you requested GPFO, and can you look at freebody results to confirm that at the converged solution the "deformed loads" match the final SPCF?

 

[adamas]

I'll do the freebody check, thanks for the advice.