Windows Pardiso Nonlinear convergence problem

Analysis issues
1

I’m not sure if this issue relates only to the windows Pardiso solver when used nonlinear and displacement controlled neither the Pastix or the Spooles solvers seem having this issue at least with this specific combination, but later I have observed it as more general.
I sometime have had converge problems with the Pardiso solver when I used it in the above mode, speciel when a fixed and a moved part not yet wasn’t in direct contact.
A few days ago, I believe was able to isolate a part of this phenomenen down to a single element as listed in the following dataset.

**the Pardiso solvers (before juli 2026) will not converge despite the structure is unloaded and balanced
*Node
340, 1.38742060E+003, 7.44341400E+002, -9.38755720E+003
341, 1.46807520E+003, 5.03643260E+002, -9.38898610E+003
360, 1.43165120E+003, 6.25233640E+002, -9.38831562E+003
911, 1.48986560E+003, 4.61882580E+002, -9.08155652E+003
913, 1.40279840E+003, 7.25714900E+002, -9.13925252E+003
1409, 1.45116340E+003, 5.95337160E+002, -9.11048952E+003
1587, 1.48065960E+003, 4.83334720E+002, -9.23523678E+003
1592, 1.39585360E+003, 7.35451020E+002, -9.26339032E+003
**
*Element, Type=S8, Elset=Eall
449, 911, 913, 340, 341, 1409, 1592, 360, 1587
**
*Nset, Nset=Nskir_sless_top_LOAD
 340, 341, 360
**
*Material, Name=STEEL
*Elastic
210000, 0.3
*Density
7.8E-09
**
*Shell section, Elset=Eall, Material=STEEL, Offset=0
25
**
*Step, Nlgeom
*Static, solver=pardiso
**
*Boundary, op=New
*Boundary
Nskir_sless_top_LOAD, 1, 2, 0
Nskir_sless_top_LOAD, 3, 3, 100
Nskir_sless_top_LOAD, 4, 6, 0
**
*Node file
U
*El file
S, NOE
**
*End step

The really weird thing with the above dataset is that just renaming node 1592 to node 15 solving the converging problem and the dataset finished with the prediscribed displacement of 100mm.

An upgrading to the latest Intel Pardiso libraries dated July 1, 2026, solved the problem for this specific combination but doesn’t seem to solve the general problem for other combination so if anyone should have some general workaround to stabilize a dataset with a moved part until it will have hard contact to a fix boundary i would be thankful to hear.

1 Like
2

Have you confirmed the linear static solution is correct and robust between solvers, even with small loads? A distorted shell with SPCs looks like a prime candidate for knot/element bugs. It might be the matrix is singular or nearly and no solver has much hope but some cope with a bit of luck. The fact the node renumbering alters it seems to support this even more.

Another look - this seems to be a zero-strain rigid body displacement? CCX may have convergence problems with that. I would try to put a small force somewhere.

2 Likes
3

Abaqus also fails to converge.

image
image718×404 9.87 KB

2 Likes
4

@vicmw , thanks for the hint, you’re right, it just required a very tiny bit of counter force to stabilize the solver,

and thanks for remind me, that for a solver with an iterative approach the normal will always be a minimum deviation from start to obtain converge, oppesite the converge as starting point which will need to be handled as speciel case.