## Negative terms on the factor diagonal

## Negative terms on the factor diagonal

(OP)

Hello,

I have a few questions regarding the negative terms on the factor diagonal error when launching an analysis on nastran.

My problem:

*** SYSTEM INFORMATION MESSAGE 4159 (DFMSA)

THE DECOMPOSITION OF KLL YIELDS A MAXIMUM MATRIX-TO-FACTOR-DIAGONAL RATIO OF 1.247295E+05

*** USER WARNING MESSAGE 4698 (DCMPD)

STATISTICS FOR DECOMPOSITION OF MATRIX KLL.

THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN

1.000000+200 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.

USER INFORMATION:

GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

20019 T2 8.28362E-01 -1.74108E+02

20019 T3 2.23246E-01 -5.61770E+01

20020 T1 -2.46866E+01 4.15088E+02

20020 T2 -4.31962E+00 -7.86122E+01

20020 T3 -2.85832E-01 -1.50575E+02

20021 T2 -3.20852E-01 1.43679E+01

20021 T3 9.61730E-01 -2.49802E+02

20022 T3 1.23418E+00 -3.57038E+02

20023 T3 -4.48815E+00 -4.75721E+02

20024 T3 -3.79101E-01 -6.09658E+02

20025 T2 -4.82163E+00 4.21503E+02

20025 T3 -8.72780E-01 -7.63142E+02

20026 T3 -5.12149E+00 -9.41100E+02

20027 T3 -1.90611E+00 -1.14923E+03

20028 T2 -1.08507E+00 7.69955E+02

20028 T3 2.15322E+00 -1.26161E+03

20029 T3 -3.54330E+00 -1.14923E+03

20030 T2 -5.65539E+00 5.48362E+02

20030 T3 -4.07993E-01 -9.41102E+02

20031 T3 2.16420E+00 -7.63150E+02

20032 T3 2.03869E+00 -6.09663E+02

Multiple nodes like this, all regarding to the same material

As you can see, i set the MAXRATIO value to absurds values until I noticed the problem was not the maxratio, but that i had negative terms. Is there a way to solve this?

I read that negative terms mean this material is buckling, in such case, I guess my analysis is failing and the material is not stiff enough in comparison with the rest of materials? (I'm comparing PVC foam with aluminium.

Thank you very much

I have a few questions regarding the negative terms on the factor diagonal error when launching an analysis on nastran.

My problem:

*** SYSTEM INFORMATION MESSAGE 4159 (DFMSA)

THE DECOMPOSITION OF KLL YIELDS A MAXIMUM MATRIX-TO-FACTOR-DIAGONAL RATIO OF 1.247295E+05

*** USER WARNING MESSAGE 4698 (DCMPD)

STATISTICS FOR DECOMPOSITION OF MATRIX KLL.

THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN

1.000000+200 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.

USER INFORMATION:

GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

20019 T2 8.28362E-01 -1.74108E+02

20019 T3 2.23246E-01 -5.61770E+01

20020 T1 -2.46866E+01 4.15088E+02

20020 T2 -4.31962E+00 -7.86122E+01

20020 T3 -2.85832E-01 -1.50575E+02

20021 T2 -3.20852E-01 1.43679E+01

20021 T3 9.61730E-01 -2.49802E+02

20022 T3 1.23418E+00 -3.57038E+02

20023 T3 -4.48815E+00 -4.75721E+02

20024 T3 -3.79101E-01 -6.09658E+02

20025 T2 -4.82163E+00 4.21503E+02

20025 T3 -8.72780E-01 -7.63142E+02

20026 T3 -5.12149E+00 -9.41100E+02

20027 T3 -1.90611E+00 -1.14923E+03

20028 T2 -1.08507E+00 7.69955E+02

20028 T3 2.15322E+00 -1.26161E+03

20029 T3 -3.54330E+00 -1.14923E+03

20030 T2 -5.65539E+00 5.48362E+02

20030 T3 -4.07993E-01 -9.41102E+02

20031 T3 2.16420E+00 -7.63150E+02

20032 T3 2.03869E+00 -6.09663E+02

Multiple nodes like this, all regarding to the same material

As you can see, i set the MAXRATIO value to absurds values until I noticed the problem was not the maxratio, but that i had negative terms. Is there a way to solve this?

I read that negative terms mean this material is buckling, in such case, I guess my analysis is failing and the material is not stiff enough in comparison with the rest of materials? (I'm comparing PVC foam with aluminium.

Thank you very much

## RE: Negative terms on the factor diagonal

A well-conditioned model should have neither negative terms nor high ratios on its factor terms. The reasons of negative terms could be the following:

1.- FE model not fully constrained: models used in static analysis must be constrained to ground in at least a statically determinate manner even for unloaded directions to avoid rigid body motions.

2.- Another source of high ratios arises from connecting

soft elements to stiff elements. Remember local stiffness is a function of element thickness. More reliable corrections are to replace the very stiff elements with rigid elements.3.- A third source of high ratios is the elements omitted through oversight.

At present, there are two major methods of identifying large ratios and nonpositive-definite matrices. In some solution sequences, the largest matrix diagonal to factor diagonal ratio greater than 105 (MAXRATIO default) is identified by its internal sequence number, and the number of negative factor diagonal terms is output. The best method to identify mechanisms here is to apply checkout loads that cause internal loads in all of the elements. Then inspect the displacement output for groups of grid points that move together with implausibly large displacements and common values of grid point rotation.

But without the nastran input file in hand is difficult to know the source of the problem (post your model here and I will investigate it). You can always run a

normal modes/eigenvalue analysis (SOL103)to compute the natural frequencies of the structure, if you have zero (or near to zero) frequency values this means you have a mechanism. Animate your deformed mode shape and you will realize of the modeling error, either in wrong boundary conditions or wrong material properties (see my blog here: https://iberisa.wordpress.com/2011/02/20/mensaje-d...)In general, a summary of the typical causes for singularity in FEM/FEA is the following:

• DOF without stiffness because of missing elements.

• A 2-D plate problem with the normal rotation unconstrained.

• A solid model with rotational DOFs at the corners unconstrained.

• Incorrect modeling of offset beams.

• Incorrect multipoint constraints.

• Mechanisms and free bodies, such as sloped plates, beam to plate connections, beam to solid connections, and plate-to-solid connections.

• Low stiffness in rotation.

• A stiff element adjacent to a very flexible element.

• A point mass input on a C0NM2 entry that uses offsets in three directions, etc..

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/

## RE: Negative terms on the factor diagonal

First of all thank you very much for your help, I am also a spaniard! I am just getting introduced to FEA as a student project.

I think my main problem is indeed connecting a soft element to a stiff element: I am studying a joint of sandwich panels and aluminium profile.

When I use a very low stiffness core (Young = 146 and shear mod = 30 MPa) the solution fails as described. But if I swap to one with higher shear modulus (Young 100 MPa and Shear Mod 200 MPa) it indeed works.

I was wondering then how to solve this, if the only solution is to solve with the param bailout or if I am missing something.

Thank you again

## RE: Negative terms on the factor diagonal

But be aware, ill conditioned stiffness matrix may produce large truncation errors. Your results will be numerically inaccurate or may not. Шt depends on the ratio of soft/hard elements to stiffness. You can enable double precision numerics to reduce roundoff errors.

You "touch" roundoff errors due to ill-conditioned matrix by making simple test example. Make cylindrical surface? mesh it with plate (PSHELL) elements, load them with pressure and constrain one node of mesh in all DOF`s. Now start to decrease element thickness - increase radius to thickness ratio (R/t) and check deformed shape. At some point deformed shape become non physical. If you enable double precision then deformed shape of "bad" results will be OK.