## Plate Element DOFs

## Plate Element DOFs

(OP)

Hi,

I've got a simple mid-surface geometry of excavator bucket. I applied load a boundary conditions. For my first approach I used linear plate elements (CQUAD4) so I see if my model is right. But when I used parabolic quad elements (CQUAD8) for better results I've got an error (FATAL MESSAGE 9137 (SEKRRS)). From .f06 file I read there are some grid points which have DOF in z-direction (in this case). I used options "param,bailout,-1" to check behaviour of model with CQUAD8 elements. Translation and stresses look fine but due the FATAL MESSAGE there's a quite high total rotation. I try to fixed all surface but the error still remain. I don't understand what's wrong or where I'm wrong. Have anybody experience with this strange behaviour or can somebody give me some tips to fix that?

Regards

jrz

I've got a simple mid-surface geometry of excavator bucket. I applied load a boundary conditions. For my first approach I used linear plate elements (CQUAD4) so I see if my model is right. But when I used parabolic quad elements (CQUAD8) for better results I've got an error (FATAL MESSAGE 9137 (SEKRRS)). From .f06 file I read there are some grid points which have DOF in z-direction (in this case). I used options "param,bailout,-1" to check behaviour of model with CQUAD8 elements. Translation and stresses look fine but due the FATAL MESSAGE there's a quite high total rotation. I try to fixed all surface but the error still remain. I don't understand what's wrong or where I'm wrong. Have anybody experience with this strange behaviour or can somebody give me some tips to fix that?

Regards

jrz

## RE: Plate Element DOFs

## RE: Plate Element DOFs

it's possible that your problem is basic ... ie you haven't restrained the 6 rigid body motions ... check your constraints.

it could be that the FE is unhappy with the stiffness ratio of some elements, or it could be that the model is forcing a lot of load down a weak loadpath.

look into modifing the analysis exec deck ...

model/analysis/edit (you should be looking at the first analysis screen ... title, analysis program, analysis type.

next/next ... "NASTRAN bulk data options"

look at the value for "maxratio", increase it by several orders of magnitude (from 1E06 to 1E09 ...)

## RE: Plate Element DOFs

For the parabolic elements (CQUAD8) I changed "maxratio" by the output in .f06 file (where is the max value of maximum ratio of matrix diagonal) to 0.5e7 and solution went through. Results like stress and translation look fine. But I don't feel good with the output vectors of rotation. There are 10-1000x higher against the linear solution, I think that's too much. I read somewhere (I don't remember right now) that if maxration>10e5 (or 10e6) it may indicate trouble.

But I don't understand one thing. I tried to use fix support on the whole mid-surface geometry a do the solution (with CQUAD8) but there was still DOFs remain (R3 in my case)!

At this time I can do another step but I think that isn't clear solution (change "maxration"). I try to figure out what's wrong.

Thanks rb1957

## RE: Plate Element DOFs

is this a pure shell or a stiffened shell model ?

with quad8 plates, did you remesh the stiffeners to support the mid-side nodes ?

one thing is NASTRAN doesn't (as far as i know) have a beam3 compatable with a quad8 ... they refine the side using two beam2 elements, so the mid-side isn't "properly" consistent.

if the results (stresses) look good (and consistent with the quad4 model) then i guess they are good. one thing might be to refine the quad4 mesh (4 quad4 for each original element, 2 beam2s) and see.

## RE: Plate Element DOFs

I use shell without stiffness.

I have boundary conditions (load and constraint) applied on the geometry. I mesh the geometry with linear plate element (cquad4) and do solution without error. Instead linear plate element I want to use parabolic plate element (cquad8) to mesh the geometry. But solution ends with error I mention.

I have same idea to mesh geometry with cquad4 and two times higher density.

For now I think it could be some geometry problem. I'm going to make new geometry (quite complicated) and I see.

## RE: Plate Element DOFs

## RE: Plate Element DOFs

## RE: Plate Element DOFs

If you revise the file .F06 you will see the following problem in the RZ DOF of CQUAD8 elements:

GRID_POINT_ID DEGREE_OF_FREEDOM MATRIX/FACTOR_DIAGONAL RATIO_MATRIX_DIAGONAL1719 R3 1.11339E+07 9.51236E+05../..

^^^ 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

^^^ CONTINUE THE RUN WITH MECHANISMS.

*** USER INFORMATION MESSAGE 4158 (DFMSA)

---- STATISTICS FOR SPARSE DECOMPOSITION OF DATA BLOCK KLL FOLLOW

NUMBER OF NEGATIVE TERMS ON FACTOR DIAGONAL = 0

MAXIMUM RATIO OF MATRIX DIAGONAL TO FACTOR DIAGONAL = 1.2E+07 AT ROW NUMBER 32645

User information:

One, two or three of the statistics will be printed as follows:

(1) negative terms on factor diagonal only if they exist;

(2) maximum(3) spill rows only if the problem spills.ratio only if it exceeds a threshold defined by the paramater MAXRATIO

(default 1.0E7);

Depending on the context, these messages may indicate modeling

problems. The threshold may be changed with the parameter MAXRATIO,

however, the user is cautioned against arbitrarily increasing the

MAXRATIO value just to get the model to run. The cause of large

MAXRATIOs should be investigated.

According NX NASTRAN manuals the Shell CQUAD4 do not have the Z-rotational DOF. The problem could be avoided with the use of "PARAM,AUTOSPC,YES", or adding an artificial stiffness to the DOF using "PARAM,K6ROT,100".

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.

To avoid this problem, you can:

Constrain the rotational degree-of-freedom either manually with an SPC entry (either in field 8 of the GRID entry or an SPC entry) or automatically with the AUTOSPC parameter. If using the SPC method, ensure that you do not constrain any components that have stiffness attached.

Apply an artificial stiffness term to the degrees of freedom using PARAM K6ROT. Remember when using this parameter that the stiffness being included for the rotational degree of freedom is not a true stiffness and should not be used as such. For example, if you want to connect a CBAR element to the CQUAD4 element, you shouldn’t rely on the K6ROT stiffness to transfer the bending moment at the end of the CBAR into the plate.

But according to the QUICK REFERENCE GUIDE (QRG) manual of NX NASTRAN the K6ROT parameter is ignored for CQUAD8 elements!!

K – Parameters________________________________________

K6ROT Default = 100.0

K6ROT specifies the stiffness to be added to the normal rotation for CQUAD4 and CTRIA3 elements. This is an alternate method to suppress the grid point singularities, and is intended primarily for geometric nonlinear analysis. A value between 1.0 and 100.0 is recommended to suppress singularities. A large value may be required in nonlinear and eigenvalue analyses. This parameter is ignored for CQUADR, CTRIAR, CQUAD8, and CTRIA6 elements. K6ROT is forced to 0 when only membrane elements exist.

Then the only resource left is to increase the value MAXRATIO, using for instance "PARAM,MAXRATIO,1E8"

M – Parameters________________________________________

MAXRATIO Default = 1.E7

Default = 1E10 if glue, linear contact or Lagrange rigid elements are present in the model.

The ratios of terms on the diagonal of the stiffness matrix to the corresponding terms on the diagonal of the triangular factor are computed.

If, for any row, this ratio is greater than MAXRATIO, the matrix will be considered to be nearly singular (having mechanisms). If any diagonal terms of the factor are negative, the stiffness matrix is considered implausible (nonpositive definite). The ratios greater than MAXRATIO and less than zero and their associated external grid identities will be printed out. The program will then take appropriate action as directed by the parameter BAILOUT.By default, in the superelement solution sequences the program will terminate processing for that superelement. A negative value for BAILOUT directs the program to continue processing the superelement.

Although forcing the program to continue with near-singularities is a useful modeling checkout technique, it may lead to solutions of poor quality or fatal messages later in the run. It is recommended that the default values be used for production runs. A related parameter is ERROR.The value -1 of BAILOUT causes the program to continue processing with near singularities and a zero value will cause the program to exit if near singularities are detected.

In SOLs 101 through 200 when PARAM,CHECKOUT,YES is specified, PARAM,MAXRATIO sets the tolerance for detecting multipoint constraint equations with poor linear independence. (See “Superelement Analysis” in the NX Nastran User’s Guide.)

BAILOUT and MAXRATIO may be specified in the Case Control Section in order to provide different values between superelements but not between different boundary conditions.

SOLUTION=========

Simply using MAXRATIO = 1.3E7 will solve the problem.

Best regards,

Blas.

~~~~~~~~~~~~~~~~~~~~~~

Blas Molero Hidalgo

Ingeniero Industrial

Director

IBERISA

48011 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog de FEMAP & NX Nastran: http://iberisa.wordpress.com/