How to generate a response spectrum from an analysis..?

[adam.a.kendal]

Good afternoon,

Would anyone be able to help with this query please?

One of our client's requirements from analysis is that the seismic response spectrum analysis includes the amplification of the support as-modelled into Inventor Nastran (itself subject to the building response spectrum). The desired outcome is to know if the support amplifies the building vibrations on the instrument that is mounted to the support by more than a factor of 1.5x. I had hoped to compare accelerations in each of the translational directions with the building response spectra however this doesn't really give the full picture, as the results are an SRSS of the individual modes so its not clear what contributions are present from which mode / the magnitude of the acceleration and associated frequency etc in order to compare with the input spectrum.

I can only envisage that I need to be able to generate a response spectrum from the support itself  in order to compare it to the input response spectrum of the building, in order to be able to state the amplification of the support. Unfortunately I cannot

find online help on this topic leading me to think this is not an available feature.

Could anyone assist with this please?

Thank you and best regards

Adam

[John_Holtz]

Hi Adam,

Hopefully someone more knowledgeable about vibrations will reply. But first, your question gives me the opportunity to mention something that I learned last week. 🙂 When you open the Inventor Nastran Help, the home page that looks like a figure is actually links. And more importantly, the one link that does not appear anywhere else is the "Download the Help" link.

That link goes to a page named "Autodesk Inventor Nastran Offline Help". What's good about the offline help page is the document "Inventor Nastran Solver 20YY Users Manual". (I was familiar with the Users Manual but always needed to Google it to find it. Now I know there is a link to the page.) Section 6.3 of the Solver User's Manual describes which command you need to add to the Nastran file to generate a response spectrum input. Note that a response spectrum is generated from a transient analysis. It is the time-varying results that are used to calculate the frequencies for the response spectrum.

However, I am not sure that you need to calculate the response spectrum. My interpretation of the customer's question is whether the acceleration of the "device" mounted on their support structure is within 50% of the acceleration of the base. For example, if the base accelerates at 40 in/sec^2 and the device accelerates at 45, then the amplification is 45/40 = 1.125. I agree that the results of a response spectrum analysis is an SRSS of all modes of vibration, but that is true for the constraint points as well as for the "device". I think you do not need the response at different frequencies to do the comparison.

Let me know what you think.

(edited Feb 8 to indicate the "Download the Help" link does not appear anywhere else. My original post said "does appear anywhere else". 🤔)

John

[adam.a.kendal]

Thank you for the reply John.



The input response spectrum(s) varies wildly. So for an example:



- At less than 1 Hz the response is between 1 m/s2 and 20 m/s2.

- Up to 6 Hz this climbs rapidly to 50 m/s2.

- Between 6 Hz and 50 Hz the accelerations reduce to 10 m/s2.



As I get an output including acceleration but not frequencies, and the acceleration (SRSS combined) is in excess of 200 m/s2, my possible amplifications could be anywhere between 4 (200/50) and 200 (200/1).



Hence if I could compare a chart with a chart (response spectrum vs response spectrum) it would look a little more definitive.



Best regards



Adam

[adam.a.kendal]

I should probably also add here John that the input response spectrum is from the floor response spectra for a particular level of a building and these supports and instruments could be located anywhere on that floor. So I have added a rigid body connector in here for the response spectra to be input with, there is no concentrated mass like a stiff foundation slab so I cannot see the motion of the floor to get absolute accelerations for floor and instrument to compare. The analysis as-run is effectively like a shaker table; the acceleration at the bottom is reported as zero so whatever the response happens to be is relative to the input spectrum and that in itself is not a fixed value and thus not easily comparable.

[adam.a.kendal]

Good afternoon John,

Can I ask please. I'm trying to run an analysis per the above which will give me a clear base acceleration and support / instrument acceleration so I can clearly display the amplification factor described. There are three different direction accelerations applied with two different spectra - two horizontal, one vertical.

Using a response spectrum analysis I only seem to be able to create a virtual shaker table which provides me with results. This being where I apply a structural support (fully fixed translationally and rotationally) and then add a response spectra to the same restraint node at the base of the support. This results in 0 (or near-zero) reported acceleration at the base, increasing as stiffness reduces up to the top of the support and instrument.

Having watched various Autodesk videos and read various Autodesk help files I've applied concentrated mass at the base (to emulate a floor of a building), I cannot get non-zero results. I've tried restraining some degrees of freedom, all and none. The concentrated mass is applied at a rigid body connector. With or without restraint (except for full restraint) the stresses, displacements and accelerations are zero. I was hoping that using the concentrated mass as a reference point would show the total acceleration at the base (from the three combined accelerations) and the accelerations in the support relative to the base. However that doesn't appear to have happened and I can't work out why.

Is there any advice you can offer please?

Thank you

Adam

[adam.a.kendal]

Good afternoon John,

Apologies just realised this was posted back to me not you.

Can I ask please. I'm trying to run an analysis per the above which will give me a clear base acceleration and support / instrument acceleration so I can clearly display the amplification factor described. There are three different direction accelerations applied with two different spectra - two horizontal, one vertical.

Using a response spectrum analysis I only seem to be able to create a virtual shaker table which provides me with results. This being where I apply a structural support (fully fixed translationally and rotationally) and then add a response spectra to the same restraint node at the base of the support. This results in 0 (or near-zero) reported acceleration at the base, increasing as stiffness reduces up to the top of the support and instrument.

Having watched various Autodesk videos and read various Autodesk help files I've applied concentrated mass at the base (to emulate a floor of a building), I cannot get non-zero results. I've tried restraining some degrees of freedom, all and none. The concentrated mass is applied at a rigid body connector. With or without restraint (except for full restraint) the stresses, displacements and accelerations are zero. I was hoping that using the concentrated mass as a reference point would show the total acceleration at the base (from the three combined accelerations) and the accelerations in the support relative to the base. However that doesn't appear to have happened and I can't work out why.

Is there any advice you can offer please?

Thank you

Adam

[John_Holtz · Accepted solution]

Hi Adam,

It looks like the response spectrum results (such as the displacements) are relative displacements - relative to the support. Therefore, the displacement, velocity, acceleration of the support will always be shown as zero.

This approach may work:

1. Add the two commands shown below to the top of the Nastran file, underneath the line "ID .....". This will tell the solver to output additional results. The extra results are each natural frequency which are combined to show the SRSS result that is normally given in Inventor. (These two commands can be added using the "Nastran File" tab in Inventor, or you could use the stand-alone Nastran Editor.) 
2. Based on the entered response spectrum, calculate what the result should be at the support.
3. Add that value to the point of interest in the model. This now gives the total result (not the relative result) at the support and point of interest.
4. Do that for each of the modes, then calculate the combined results (SRSS) if desired.
5. With the total results calculated, the amplification can be calculated.

$ Two commands to add to the top of the Nastran (.nas) file.
NASTRAN TRSLDDAMDATA=ON  
NASTRAN INMEMORYIO=OFF

Here are a few other suggestions:

• Do a test where a single response spectrum is applied. If that works, then try the multiple response spectra. However, there are reports that Inventor does not create the Nastran file properly when using multiple subcases to define multiple excitation directions. See How to run a multi-directional response spectra in Inventor Nastran (autodesk.com). (What's not suggested in the article is that it may be easier to run three separate analyses with one response spectrum in each analysis.)
• I think adding the concentrated mass to the support adds no value assuming the support is constrained in all directions. Adding the mass may actually be a hinderance. Since the support is fixed, the mass is not vibrating in the modal analysis and should have no effect on the natural frequencies. The mass is probably included in the total mass of the model, so the mass participation factors (shown in the output) are lower because the concentrated mass is not vibrating. Think of it like this:
  • If the concentrated mass is 1/2 the total mass of the model,
  • if the rest of the model is vibrating and contributing 100% of its mass to the participation factor,
  • then the (total) mass participation factor shown in the output will never exceed 50%.
  • The rule-of-thumb is to calculate enough modes to reach 85% to 90% mass participation factor. Showing a report to a customer/co-worker and trying to explain that 45% shown in the output file is really 90% because of the constrained mass is a conversation that you probably want to avoid.

Let us know what you find out.

John

[adam.a.kendal]

Thank you John,

I did alter a couple of other things before your reply. I noticed the Autodesk video I was watching had a lower frequency to analyse from. Knowing from a modal analysis that the lowest natural frequency is around 60Hz in the model I changed this lowest frequency to 10 Hz. I had previously read about the 'Rigidbodymode' parameter and tried this too - but it removes the first 6 modes - I wondered if rigid body motion was a problem here. But in the range I was analysing the first 6 modes would have been between 0-300 Hz (I think) and the input floor response spectra is from 0-50Hz so that probably would have cancelled out all results also - I got zero for all results here too. So with Rigidbodymode set to Auto again, and lowest frequency set to 10 Hz, the analysis ran. As you suggested, I had tried a single response spectra acting in all directions to keep things simple. And with the mass as the only 'constraint' (i.e. no structural restraints). The stresses are the same order of magnitude as I have previously had, so I'll go back and make the combined cases again where there are different spectra acting in horizontal and vertical.

Thank you for responding with those commands, I'm sure they will come in useful in this little quest I've been set. And absolutely noted about the missing mass. I think what I'll do is run one analysis with large mass in order to get the SRSS of the building motions so I can compare the accelerations / get the amplification. And run another analysis as a shaker table (fully fixed) in order to assess mass participation.

Thank you again for responding

Adam