Having only five rigid modes not 6 from Free-Free Modal Analysis 1

[Mo_S]

Hello everyone,

It is my first time using MSC Patran/Nastran and also my first time doing a free-free modal analysis. I am doing that analysis on a beam of hollow circular cross-section. I assigned the dims, material, made the mesh, and everything as shown in the BDF file however I get only the five rigid modes and I don't get the last one. I read the F06 file it shows warning messages:

USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX SCRATCH.
THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
1.000000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.
USER INFORMATION:
THIS MESSAGE MAY BE IGNORED IF NO GRID POINT IDS OR HIGH RATIO MESSAGES APPEAR IN THE TABLE ON THE NEXT PAGE.
0 SUBCASE 1
0
GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

3 R1 -4.50360E+15 1.00000E+00

*** SYSTEM WARNING MESSAGE 7340 (LNNHERR)
PROCESS ERROR REPORTED BY SUBROUTINE LNNP2CS (IER= -729)
USER INFORMATION: REPEATED SINGULAR MATRIX -- PROBABLY ILL-POSED PROBLEM.
*** SYSTEM WARNING MESSAGE 7340 (LNNHERR)
PROCESS ERROR REPORTED BY SUBROUTINE LNNDRVS (IER= -729)
USER INFORMATION: REPEATED SINGULAR MATRIX -- PROBABLY ILL-POSED PROBLEM.

TABLE OF SHIFTS: (LNNRIGL)
SHIFT # SHIFT VALUE FREQUENCY, CYCLES # EIGENVALUES BELOW # NEW EIGENVALUES FOUND
1. 1.5621309E+07 6.2904083E+02 FACTOR ERROR 0
2. -1.2758284E+04 -1.7976961E+01 FACTOR ERROR 0
3. -3.2628134E+04 -2.8748570E+01 FACTOR ERROR 0

*** SYSTEM WARNING MESSAGE 7340 (LNNRIGL)
REPEATED SINGULAR MATRIX -- PROBABLY ILL-POSED PROBLEM.
^^^
*** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KXX.
THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
1.000000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.
USER INFORMATION:
THIS MESSAGE MAY BE IGNORED IF NO GRID POINT IDS OR HIGH RATIO MESSAGES APPEAR IN THE TABLE ON THE NEXT PAGE.

0 SUBCASE 1
0
GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

1 T1 1.00000E+15 7.31389E+07
1 T2 -2.34837E+15 6.56128E+06
1 T3 -2.34837E+15 6.56128E+06
1 R1 2.34837E+15 1.23918E+03
1 R2 2.62036E+13 4.25402E+03
1 R3 2.62036E+13 4.25402E+03


I didn't understand these messages if someone can clear them out and suggest what I need to do to solve this issue that would be great.

Thanks

https://files.engineering.com/getfile.aspx?folder=6078d46e-f7a8-47d9-840c-ff960578876b&file=Beam.bdf

https://files.engineering.com/getfile.aspx?folder=1fb19586-fb53-4064-8713-0a66ecda83a0&file=Beam.f06

 

[dmapguru]

You have defined the model of the beam using CBAR elements. Although this is not wrong, these elements do have some limitations. The CBAR element was introduced to MSC Nastran on day 1, and they are simple, prismatic stiffness elements that in their original form do not generate a mass moment of inertia about the axis of the element. For static analysis, this is not a problem, but for normal modes, this leads to a phenomenon known as a massless mechanism if the CBAR elements are free to rotate about their axis, which is your case. Your model is missing the torsional rigid body mode because MSC Nastran detected the massless mechanism (that is what those messages are about) and restrained it.

In V2004, an enhancement was introduced to MSC Nastran that allowed a mass moment of inertia to be computed for the CBAR elements, but for backward compatibility reasons, it is not switched on by default, i.e. you have to request it. To do this, add the following line as the very first line in the input file:

NASTRAN BARMASS=1

Alternatively, you could use a different type of beam element like the CBEAM. If you want to create CBEAM elements in Patran, when you create the beam properties in the Element Properties dialogue with the Create, 1D, Beam option, towards the bottom of the dialogue you will see Options: - this will probably be set to General Section, which means CBAR elements will be created. If you click the General Section button, you can change this to General Section (CBEAM). Now when you define the properties, the beam elements Patran will create are CBEAM elements.

If you want to change the CBAR to a CBEAM by editing the input file, simple change CBAR to CBEAM and PBARL to PBEAML, it is as simple as that. CBEAM elements are flexibility elements which means they generate flexibility matrices at the element level which is then inverted to yield stiffness. This allows the CBEAM elements to have more refined behaviour, such as a varying cross section along its length and its neutral axis may be offset from the shear centre of the beam. CBAR elements are stiffness elements and stiffness terms are generated directly at the element level, but they are rudimentary. This means that you may omit some of the properties for the CBAR element, but you must define all properties for the CBEAM, even when you may think you don’t need to. For example, if you use a CBAR element and wanted an element that had no bending stiffness in one of its bending directions, you could simply omit the I1 or I2 property definition on the PBAR entry. If you try this with CBEAM elements on the PBEAM entry, the job will fail.

DG

 

[Mo_S]

Thank you so much... that was very helpful