Skew angle warning in SOL 103

[ImphaTonks]

Dear all,

I am running SOL 103 on a simplified body-in-white structure. The simulation come out without error and the deflection shape looks satisfying. However the the natural frequencies that i obtained is illogical.

MODE EXTRACTION EIGENVALUE RADIANS CYCLES GENERALIZED GENERALIZED
NO. ORDER MASS STIFFNESS
1 1 1.264173E+02 1.124355E+01 1.789466E+00 1.000000E+00 1.264173E+02
2 2 8.653103E+02 2.941616E+01 4.681726E+00 1.000000E+00 8.653103E+02
3 3 1.097032E+03 3.312147E+01 5.271446E+00 1.000000E+00 1.097032E+03
4 4 1.319294E+03 3.632209E+01 5.780840E+00 1.000000E+00 1.319294E+03
5 5 2.485403E+03 4.985382E+01 7.934481E+00 1.000000E+00 2.485403E+03
6 6 2.904925E+03 5.389736E+01 8.578031E+00 1.000000E+00 2.904925E+03
7 7 3.423773E+03 5.851302E+01 9.312635E+00 1.000000E+00 3.423773E+03
8 8 6.035509E+03 7.768854E+01 1.236451E+01 1.000000E+00 6.035509E+03
9 9 6.547044E+03 8.091381E+01 1.287783E+01 1.000000E+00 6.547044E+03
10 10 7.843182E+03 8.856174E+01 1.409504E+01 1.000000E+00 7.843182E+03


These warning messages come out in the .f06 file:

USER INFORMATION MESSAGE 7555 (GMTSTD)
FINITE ELEMENT GEOMETRY CHECK RESULTS EXCEED TOLERANCE LEVELS FOR THE FOLLOWING ELEMENTS. METRIC VALUES THAT EXCEED
TEST TOLERANCE LIMITS ARE IDENTIFIED BY ONE OF THE FOLLOWING FLAGS PLACED TO THE RIGHT OF THE METRIC VALUE.
"++++" FOR TEST RESULTS EXCEEDING TOLERANCES. INFORMATIONAL ONLY. PROBLEM SOLUTION CONTINUES. (DEFAULT FLAG)
"IGNR" FOR TEST RESULTS EXCEEDING TOLERANCES. INFORMATIONAL ONLY. PROBLEM SOLUTION CONTINUES.
"WARN" FOR TEST RESULTS EXCEEDING TOLERANCES. INFORMATIONAL ONLY. PROBLEM SOLUTION CONTINUES.
"FAIL" FOR TEST RESULTS EXCEEDING TOLERANCES. SEVERE ERROR. PROBLEM SOLUTION TERMINATES.
USER ACTION: USE THE GEOMCHECK (EXECUTIVE CONTROL STATEMENT) KEYWORD=VALUE TO CHANGE TOLERANCE VALUES IF DESIRED.
A MAXIMUM OF 100 SKEW ANGLE (SA) TOLERANCE LIMIT VIOLATIONS WILL BE IDENTIFIED BY THE FLAG "++++"
PLACED AFTER THE VALUE METRIC FOR THE TEST.
A MAXIMUM OF 100 MAX INT. ANGLE (IA) TOLERANCE LIMIT VIOLATIONS WILL BE IDENTIFIED BY THE FLAG "++++"
PLACED AFTER THE VALUE METRIC FOR THE TEST.
1 MSC.NASTRAN JOB CREATED ON 17-MAY-16 AT 10:53:32 MAY 29, 2016 MSC.NASTRAN 11/25/11 PAGE 5

0
TOLERANCE LIMITS ARE: SKEW = 10.00, IA(MAX) = 160.00 (++++ = LIMIT VIOLATED)
ELEMENT TYPE ID SKEW ANGLE MAX INT. ANGLE
TRIA3 1331 8.38 ++++ 90.00
TRIA3 1332 8.38 ++++ 90.00
TRIA3 1333 8.38 ++++ 90.00
TRIA3 1334 8.38 ++++ 90.00

Is the value of nat. frequencies obtained is affected by the warning? how can i solve this problem? can i get any suggestion?

 

[dmapguru]

It's unlikely that poorly shaped elements at this level are resulting in spurious modes; the elements have to be distorted to the point that the eigensolver will start baulking first. This is one of the reasons why MSC Nastran is a standard tool; its elements are as robust as hell.

On the other hand, I don't advocate poorly shaped elements, especially when there are only a few. Go look at the elements in Patran and you should be able to see how to adjust the mesh to avoid these warnings. They are on triangles, so I assume the region of the mesh is not that important anyway, and it is usually easy to split a triangle into 2 triangles to improve the mesh.

You said your model is a BIW, so I guess your remark about results being illogical stem from the lowest frequency that you expected to be higher than this? 1.8 Hz is right on the vomit on the seat frequency.

Go back to basics. What does the static checkout look like (SOL 101)? Apply loads at the seat mounts to model four rugby players sitting in the car, with all turret tops pinned (SPC in dofs 123). What is the magnitude of the displacement? It should be very small. If you get 50mm of displacement, there is a stiffness issue.

What does GROUNDCHECK(SET=ALL,DATAREC=YES)=YES report. The G set, N set and N+AUTOSPC sets should all "PASS" in at least the translational directions. If rotational directions "FAIL", inspect the nodal forces output by DATAREC=YES. If they are all small (compared with the tolerance), they can be ignored. If there are significant forces, these are modelling errors; resolve them and rerun the checks.

What does the mass/CG output look like? A major source of error in dynamics is inconsistent units (using millimetres and Kg will not give you Hz frequencies).

If all that checks out, look at the mode shapes. What exactly is flailing around at 1.8 Hz? Did you forget to attach something properly? Do you have bushes in the model; if so do they have reasonable stiffness values?