FEA - Plate to bar connection issue.

Creator
Creator

Hello everyone, 

I have a question about connection between CQUAD4 (plate ) and CBAR (bar) elemetns.

 

According to page from 4-8 to 4-9,  "Element Library Reference" that goes with FEMAP 11.4.2: 

 

"CQUAD4 and CTRIA3 Elements
The formulation of the CQUAD4 and CTRIA3 elements are based on the Mindlin-Reissner shell
theory. These elements do not provide direct elastic stiffness for the rotational degrees-of-freedom
which are normal to the surface of the element.
Consequently, for example, if a grid point is attached only to CQUAD4 elements only, all the elements
are in the same plane, then the rotational degrees of freedom about the surface normal have zero stiffness. This zero stiffness results in a singular stiffness matrix, which prevents NX Nastran from solving the model.

"

And further, two options to prevent analysis error are provided - AUTOSPC and PARAM K6ROT.

 

I built a FEM  with  AUTOSPC and PARAM K6ROT turnd off, see below


image.png

 

image.png

 

I wanted to reach the  error 9137

 

^^^ USER FATAL MESSAGE 9137 (SEKRRS)
^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL.  

^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO

 

Could someone please explaine me why it works not like I expected? 

Thanks in advanced.

 

The model is attached to the question. 

 

2 REPLIES 2

Re: FEA - Plate to bar connection issue.

Gears Phenom Gears Phenom
Gears Phenom

Ilya

 

The most probable cause is, that when you uncheck the  K6ROT PARAM within Femap [Nastran Bulk Data Options] Nastran is simply using the built in default and not doing what you want/expect - i.e turn off the K6ROT.

 

I ran your test model with K6ROT PARAM on but set to ZERO and this achieves what you expected.

 

 

Re: FEA - Plate to bar connection issue.

Creator
Creator

Thank you for your answer. You are right)

 

First of all, I also get the error when I set K6ROT to 0. 

 

But it is intresting that when simply turn off  AUTOSPC and  K6ROT in FEMAP Analysis menu, there is no K6ROT  parameter in input dat file.

INIT MASTER(S)
NASTRAN SYSTEM(442)=-1,SYSTEM(319)=1
ID model,Femap
SOL SESTATIC
CEND
TITLE = Static Analysis
ECHO = NONE
DISPLACEMENT(PLOT) = ALL
SPCFORCE(PLOT) = ALL
OLOAD(PLOT) = ALL
FORCE(PLOT,CORNER) = ALL
STRESS(PLOT,CORNER) = ALL
SPC = 1
LOAD = 1
BEGIN BULK
$ ***************************************************************************
$ Written by : Femap with NX Nastran
$ Version : 11.4.2
$ Translator : NX Nastran
$ From Model : C:\Users\USER-1\Desktop\Plate to bar conn - quest\model.modfem
$ Date : Wed Nov 07 11:58:18 2018
$ Output To : J:\FEMAP Analysis Files\
$ ***************************************************************************
$
PARAM,PRGPST,YES
PARAM,POST,-1
PARAM,OGEOM,NO
PARAM,AUTOSPC,NO
PARAM,GRDPNT,0
CORD2C 1 0 0. 0. 0. 0. 0. 1.+FEMAPC1
+FEMAPC1 1. 0. 1.
CORD2S 2 0 0. 0. 0. 0. 0. 1.+FEMAPC2
+FEMAPC2 1. 0. 1.
$ Femap with NX Nastran Load Set 1 : BL
MOMENT 1 50 0 1. 0. 0. 5.
$ Femap with NX Nastran Constraint Set 1 : BC

 

Do you think that this NASTRAN internal K6ROT parameter does not depend on dat file?