How to incorporate RBE2 elements in SOL401 nonlinear analysis?

[Michal Czaja]

Hi, I am a facade engineer and I am trying to compute bracket analysis using SOL401 with nonlinear materials, glued and contact connections and RBE2 elements to transfer loads as well as introduce additional nodal constraints to the model. As I am pretty new to SOL401, I need some help with the last. When I ran the model with no RBE2 elements, and all the loads were put directly to solids surfaces, everything worked fine and I got the results.

Then I tried to introduce RBE2 element with a nodal load of the same value and the analysis could not converge, resulting in a message:

*** USER FATAL MESSAGE 23278 (NL2SPL2)
RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN LHS MATRIX.
USER ACTION: CONSTRAIN MECHANISMS WITH SPCI ENTRIES OR SPECIFY PARAMETER MSTAB TO 1 ON THE NLCNTL CARD.
1 NL SSANIE DECEMBER 7, 2021 SIMCENTER NASTRAN 7/30/20 PAGE 13

0
0
0
0

*** SYSTEM FATAL MESSAGE 3001 (SDR2)
THE INPUT DATA BLOCK IN POSITION 10 DOES NOT EXIST.
USER INFORMATION: THIS ERROR IS CAUSED BY ONE OF THE FOLLOWING:
1. THE DATA BLOCK IS UNSPECIFIED ON THE DMAP MODULE.
2. THE DATA BLOCK IS SPECIFIED ON THE DMAP MODULE AND ON THE SUBDMAP STATEMENT
BUT NOT ON THE CORRESPONDING CALL STATEMENT.
USER ACTION: 1. IF YOU ARE EXECUTING A SIEMENS PLM SOFTWARE SUPPLIED SOLUTION SEQUENCE AND NOT USING THE
ALTER EXECUTIVE CONTROL STATEMENT, THEN CHECK FOR BULK DATA AND/OR CASE CONTROL INPUT
ERRORS. IF NO ERRORS CAN BE FOUND, THEN CONTACT SIEMENS PLM SOFTWARE CUSTOMER SUPPORT.
2. IF YOU ARE EXECUTING A DMAP PROGRAM NOT SUPPLIED BY SIEMENS PLM SOFTWARE, THEN FOR DEBUGGING
PURPOSES INSERT STATEMENT DIAGON(20) BEFORE THE MODULE SHOWN ABOVE.
PROGRAMMER INFORMATION: THE FIST NUMBER IS 110 AND SUBROUTINE IS SDR2
0FATAL ERROR
1 * * * END OF JOB * * *

My goal is to create a more complex model with a higher number of RBE2 elements for which nodal constraints and loads will be put, but I can not succeed with a simple one first. I tried increasing the number of time increments, MAXITER value and changing Rigid Element Method from AUTO to LINEAR and nothing helped.
I would forget, I calculated the complex model using linear static analysis first, and everything worked fine there.

Thanks for any replies.
Michal.

 

[BlasMolero]

Dear Michal,
The rigid elements RBE2 are perpectly supported by the Nonlinear Multi-Step Structural solver of Nastran (SOL401), then no problem.
I note you have a rigid body motion in your model (a mechanism exist). If the same model runs OK with the linear static (SOL101)then is something related with the nonlinear solver.
Please note Simcenter Nastran automatically identifies and constrains singularities in the stiffness matrix using a parameter called AUTOSPC. When you add PARAM,AUTOSPC,YES to either the bulk data or case control sections of your input file, Simcenter Nastran automatically removes degrees of freedom that are either unconnected or very weakly coupled to the finite element model.

But AUTOSPC only runs in linear static analysis, then something is wrong with your FEMAP model, you have definitely a mechanism. AUTOSPEC is ignored for the residual structure in SOLs 106 (then SOL401 as well), 129, 153 and 159 when the solution is either material nonlinear or geometric nonlinear.
Post your FEMAP model here and we can take a look to it.
Best regards,
Blas.

To learn more about rigid RBE2 elements please visit my blog:

https://iberisa.wordpress.com/2015/10/13/rbe2-vs-rbe3-on-femap-with-nx-nastran/

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[Michal Czaja]

Dear Blas,

thank You for Your answer. It led me to the conclusion, that it was something wrong with my model. I spent a lot of time reviewing the model but finally came upon some issues:
1. I used CTETRA 10-noded elements for bolts and CHEXA 8-noded elements for plates, in which holes for the bolts are made, which was obviously wrong.
2. When I corrected the mesh, I still did not get the convergence, but I found out that the bolted connections became unstable during the analysis, so I pre-stressed the bolts, which led the analysis to converge and get me the results.

Another thing I am dealing with now is CGAP elements which I found out to be not supported in SOL401. Is there any other way to introduce one-directional contact between the bolt and the slot in SOL401 nonlinear analysis?

*** USER FATAL MESSAGE 22210 (IFPDRV)
SOL 401 DOES NOT SUPPORT THE FOLLOWING BULK DATA CARDS WHICH ARE IN THE INPUT DECK.
CGAP
PGAP
-END-

Regards,
Michal

 

[BlasMolero]

Dear Michal,
Yes, with Simcenter Nastran Multi-Step Nonlinear (SOL401) you can use CBUSH elements as a ONE-DIRECTIONAL COMPRESSION-ONLY CONTACT-ELEMENT, the CBUSH element type is impressing for nonlinear analysis!!.
The key: you can define a nonlinear function of displacement vs force like of the following image: when displacement is negative, then no stiffness, when displacement is positive, then infinite stiffness (well, for instance 1e6).
You have also the CBUSH1D element supported in FEMAP V2021.2, that is a one dimensional version of the BUSH element (without the rigid offsets) and supports large displacements.
Take a look to the following video:

https://youtu.be/GExlRaU5AmE

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/