I made a FE model with lot of surface contacts and bolt preloads. When I ran the solver, I received the next error message:
*** SYSTEM FATAL MESSAGE 6144 (MERGE1)
THE SIZES OF THE INPUT MATRICES AND PARTITIONING VECTORS ARE INCOMPATIBLE. SPECIFICALLY:
The number of columns in PT6 is not equal to the number of non-zeros in partitioning vector VT6
The number of rows in P6T is not equal to the number of non-zeros in partitioning vector VT6
User Information: Size of input matrices and partitioning vectors:
KTTCOM : Rows= 5961725 by Cols= 5961725
P6T : Rows= 1 by Cols= 5961725
PT6 : Rows= 5961725 by Cols= 1
VT6 : Rows= 5961731 no. of non-zeros= 6 no. of zeros= 5961725
My model was big (more then 2 Million nodes and 1 Million elements), and I used 18 pcs. M24 bolts, 4 pcs. M16 bolts, 2 pcs. hydraulic lock simulated with bolt preloads and 10 contact pairs. Neither bolt preloads weren't in direct relationship with contacts (only through solid elements).
I simplified my model (deleting a part of model, so new model had 1,17 Million nodes and 0,64 Million elements) and deleted all bolt preloads, but I didn't get results (same error message).
After that I modified constraints, to avoid using nodal constraints (symmetry) on that nodes, which nodes were on contact surfaces, and I got results.
I added again bolt preloads, and I got results only in that case, when I replaced M16 bolt preloads with temperature loads.
I maked this procedure on my full model, but a didn't get a results, only the same error message.
Then I changed all bolt preloads to temperature loads (to get the same preload), and I got results.
Can someone explain me, what is this error message? I maked a lot of finite element analisys like this time (contacts and bolt preloads in big model), but I never got this error message.
Solved! Go to Solution.
I use Femap v11.2 with NX Nastran v10.1. I ran static analisys (SOL 101) with default options (but Force Balance ON), with one Load Set and one Constraint Set.
Connection properties was defaults, one with friction 0,15, one with 0,28.
I used tetra elements with midside nodes for solids, bar elements for bolts and RBA2 elements.
My op. system Windows7 64 bit with 32 GB RAM and 8 core processor.
This is a very unusual error for a statics run. It would be better to contact support directly for this issue.
That being said, we will likely need the f04 file and if possible the f06 with all of the messages. Is it possible to share a portion the model with the bolt preload included to understand exactly how it is constructed? Does this model run in a previous version?
A few things to check for:
stiffness issues; materials and properties of the bolts, is it possible your model has large local stiffness changes(steel contacting rubber)?
RBE2 connections crossing the contact regions.
Just thought I would a little detail to this issue. The error message from Nastran was not very helpful here. It required reviewing the F04 file to understand what operations Nastran was performing when the error occurred. This revealed that inertia relief had been turned on(unintended) but he the model did not have 6 rigid body modes. Using he the automatic method of inertia relief requires the model to have 6 rigid body modes.