da

[BTFEA]

I am working on the frequency response analysis using Sol 111 for a large structure. For this analysis I am defining a damping value as 5% in TABDMP1 card.

But from the .f06 file I see that Nastran reads this as 10% damping using the relation G=2*modal damping (zeta). I want to know if this is ok as my intention was to use only 5% damping but it turns out to be 10%?.


In .f06 file the damping value is not printed unless otherwise there is extrapolation of the damping curve. Please see .f06 output below:


*** USER WARNING MESSAGE 7697 (GKAM1A)
ONE OR MORE MODAL DAMPING VALUES FOR STRUCTURE MODES ARE EITHER NEGATIVE OR HAVE RESULTED FROM EXTRAPOLATION OF THE
TABDMP1 1 TABLE DATA AS SHOWN BELOW:

CYCLIC FREQUENCY = 3.603621E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 3.633056E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 4.103652E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 4.199019E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 4.281735E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 4.558051E+02 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)
CYCLIC FREQUENCY = 2.896406E+03 MODAL DAMPING VALUE = 1.000000E-01 (BY EXTRAPOLATION BEYOND THE RIGHT END OF THE TABLE)

 

[BlasMolero]

Hello!,
For SEMFREQ (SOL111) Modal Frequency Dynamic Response Analysis you can choose to define Structural Damping or Modal Damping, is up to you, not both, in FEMAP you can enter any of that value (the picture is for Modal Transient (Sol112), but the equivalent viscous damping definition section is the same for both analysis). If you want to use Modal damping, simply define G=0 and enter your modal damping curve of Critical Damping vs. Frequency and you are done.

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/

 

[BTFEA]

Hello Blas,
Thanks for the reply.

Though it is clearly understood how to define damping in the sol 111,It still does not solve my problem please see the problem definition below.

If I have to define a Modal damping of 5% in sol 111 which option is correct:

1) defining a CRITICAL damping value of 5% in TABDMP1 card ( used for defining damping vs frequency)
or
2) defining a STRUCTURAL damping of 5% in TABDMP1 card

IN MSC Nastran if we define a critical damping value of 5% (1st option) it get converted to a structural damping of 10% ( as defined in basic dynamic reference manual). Please see the attached pdf file for reference.

Regards,
Madhu

 

[BlasMolero]

Dear Madhu,
I run FEMAP & NX NASTRAN, then type of curve to use in FEMAP to define a modal damping of 5% is using function "7.. Critical Damping vs. Freq". In the picture above you see a range of frequency between 0 and 2100 Hz, really you can enter the only points (0,0.05) and (1,0.05) because NASTRAN will extrapolate values, no problem.

The TABDMP1 bulk entry is used to define modal damping. On the TABDMP1 entry, you define frequency/damping pairs. The software uses this table to calculate the damping value to apply at a particular frequency. To activate a TABDMP1 table, include a SDAMPING case control command that references the TID of the TABDMP1 entry.

With NX NASTRAN yYou can enter damping values on a TABDMP1 entry as either structural damping (default), Gi, damping factor, ζi, or quality factor, Qi. The software converts the entered damping values to modal damping values. To find the damping at a specific modal frequency, the software linearly interpolates or linearly extrapolates the values provided on the TABDMP1 entry.

Also by default, NX Nastran computes modal damping only once from the original modal solution. This can lead to inaccurate results if the model contains elements with frequency dependent stiffness properties. For example, frequency dependent stiffness properties can be defined for certain elements using the PBUSHT and PELAST property entries.

Hope it helps.
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/

 

[BTFEA]

Thanks Blas, for detailed explanation.

Yes it will certainly help.

Regards,
Madhu