Steady State Dynamics - No Imaginary Results

[Mechgru]

Hi,
I have carried out a Steady State Dyanmics step and obtained results. The model is a solid with first order tetrahedral elements (to reduce the run time). I have used ‘constant’ damping with a value of 0.0175 (I assume this would be 1.75% critical damping).
I was expecting Imaginary results, but only Real are available. What needs to be done to obtain imaginary, magnitude and phase results?
I requested 3 data points with a bias of 1 between 0 and 100 Hz. In the results I got 13 steps - how does this equate to the number of data points requested?
The model has 5 modes of vibration between 0 and 100 Hz ( I requested 6 modes in the Frequency step)
Thanks,

Rod (mechgru)

[FEAnalyst]

@Mechgru

I was expecting Imaginary results, but only Real are available. What needs to be done to obtain imaginary, magnitude and phase results?

Do you have in-phase loading only (Phase set to 0 in load settings and only *CLOAD, LOAD CASE=1 in the input file) ? Is Harmonic set to yes in SSD step settings ?

Keep in mind that only the individual components of output variables will have the imaginary part, not e.g. Mises stress or displacement magnitude.

@Mechgru

I requested 3 data points with a bias of 1 between 0 and 100 Hz. In the results I got 13 steps - how does this equate to the number of data points requested?

CalculiX uses n-2 points between the frequency range limits and extreme eigenfrequencies and between the eigenfrequencies themselves. So in total (m+1)(n−2)+m+2 = nm−m+n (where m means the number of eigenfrequencies while n means the number of specified data points) are used. In your case it will be 3*5-5+3=13. Bias of 1 indicates uniform spacing.

[Mechgru]

@FEAnalyst

Do you have in-phase loading only? Is Harmonic set to yes in SSD step settings

Yes and Yes
I found that the history output of displacement does contain Real, Imaginary, Magnitude and Phase results, but not the plot output.

@FEAnalyst

CalculiX uses n-2 points between the frequency range limits and extreme eigenfrequencies and between the eigenfrequencies themselves. So in total (m+1)(n−2)+m+2 = nm−m+n (where m means the number of eigenfrequencies while n means the number of specified data points)

Thank you so much for the explanation - it makes much more sense now.

Regards,

Rod

[FEAnalyst]

@Mechgru

I found that the history output of displacement does contain Real, Imaginary, Magnitude and Phase results, but not the plot output.

Yes, that’s because history output includes only the components, not Mises or displacement magnitude, for instance.

[Mechgru]

Got it, thanks.
Can you confirm the damping is proportion of critical?

Regards,

Rod

[FEAnalyst]

@Mechgru

I have used ‘constant’ damping with a value of 0.0175 (I assume this would be 1.75% critical damping).

@Mechgru

Can you confirm the damping is proportion of critical?

If you set damping to Constant and specify a value in the step definition, you get this:

*Modal damping
1, 1000000, 0.0175

which means that a modal damping of this value applies to modes from 1 to 1000000 (so essentially all modes). This keyword with no parameters results in the default MODAL=DIRECT (alternative is RAYLEIGH). So the value is a viscous damping factor ζ and yes - it’s a fraction of critical damping.