Convert Acceleration magnitude to ASD [g^2/Hz] for results of random response

[Anonymous]

Hi,

I wonder how convert acceleration magnitude from random response analysis to ASD[g^2/Hz] unit.

I've examined the random response analysis based on 10G gravity load (98000 mm/s^2 for y-direction).

g means g-force and 1g is 9800 mm/s^2 as I know.

So, I've converted like that ([acceleration magnitude]/9800.0)^2/[frequency] .

Is that right? 

It look simple, but I'm confusing.

help me.

Thanks

[John_Holtz]

Hi @Anonymous 

If I understand what result you are asking about, the result is already an ASD (but probably in units of (m/s^2)^2/Hz). The In-CAD/Inventor Nastran interface shows the units incorrectly.

Please see this article Units of PSD results are shown incorrect in Nastran for more details.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Thank for your reply, john

(As you said) if the results is already ASD unit, result values are too high I think...(even in length=mm, time=second)

When I see the graph (acceleration magnitude vs frequency), the order of magnitude is 10^5 ~ 10^6 (5~6 in log scale).

But, in the real vibration test results, the order of ASD values is 10^1~10^2 (the example in attached file which is final result I want to)

Is mass difference affect to results? If that be so, how do I calibrate the difference?

ps. I've saw the document you linked. But, I don't know what is wrong (unit in drop-down menu and unit in contour are same as meter.). Furthermore, if I change the units to "STEP n, FREQ=" and "RMS OUTPUT", values change more higer, order of ~10^12.

Thanks

[John_Holtz]

Hi @Anonymous 

It might have been helpful if you had included the entire graph instead of just one corner of it. For example, what are the units on the vertical axis?

I will assume the units of the graph are in g^2/Hz since that is the title of your post. If the In-CAD results are 1E6 (mm/s^2)^2/Hz, you convert this to g^2/Hz as follows:

• 1E6 (mm/s^2)^2/Hz * (1 g/9810 mm/s^2)^2 = 0.01 g^2/Hz

It looks like your results are too low.

If the units were set to SI when you ran the analysis, then the results are in units of m, sec, N, etc. Therefore, the ASD would be 1E6 (m/s^2)^2/Hz, and this converts as follows:

• 1E6 (m/s^2)^2/Hz * (1 g/9.81 m/s^2)^2 = 10391 g^2/Hz

Either way there is something different with your analysis.

1. What is the known load?
2. How did you enter that load?
3. What is the input under the "Dynamic Setup"? Images of the entered PSD and frequency intervals would be helpful.
4. What are the natural frequencies of the model?

[Anonymous]

Hi John.

Thanks for your reply.

I use modified SI units (mm, s, N, t..), so your first example would be right.

I attach setup (dynamic, damping and load) and result files.

Thanks.

ps. Sorry for my bad english

[John_Holtz]

Hi @Anonymous 

I see these possible problems.

1. The gravitation constant is 9800 mm/s^2, not 98000 mm/s^2! (9810 is the typical value used in mm/s^2)
2. Usually the acceleration PSD (G^2/Hz) is applied to the model through the constraints. In other words, your structure is bolted or welded to something, and that something is vibrating. The  vibration applies a load to the model at the location of the constraints. The entire model is not vibrating with the PSD acceleration, so you should not apply the load to the entire model. In other words, the load should not be a Gravity load. The load should be an Enforced Motion > Acceleration, and it is applied at the constraints (or wherever the model is being vibrated).
3. How did you get the results that are in your spreadsheet? What results are those? If you got those results from one of the pre-defined XY Plots, I think they are not plotting a useful result. (I cannot find the article that describes what the results are and why they are useless for most purposes.) You need to generate your own XY Plot and choose the correct information to graph. Keep in mind that a random response analysis outputs 4 different sets of results, some of which are useful and some of which are not that useful for the random vibration:
   1. "STEP n, FREQ =" results are from a frequency response analysis (that is, a sinusoidal load on the model). These result are not that meaningful!
   2. "PSD n, FREQ =" results are from the random vibration analysis. This is what you want to graph. So if looking at the "linear acceleration" results for PSD 1 through PSD n, this will show the acceleration spectral density (mm/s^2)^2/Hz.
   3. "RMS" is the root mean square of the PSD, so it is a result of the random vibration analysis. (This is a single result, so there is no need to graph its value. The contour plot is of this result is more useful.)
   4. "NPX" is related to fatigue and is not of interest unless you are performing a fatigue analysis (as far as I know).

Let us know if these changes give more realistic results.

[Anonymous]

Hi, John.

Above all things, I appreciate your continued interest. Thanks.

1. I applied 98000 mm/s^2 on purpose that I want to give 10 g load to entire model

2. I can't understand this part exactly. My model is a part of payload of the satellite. So, entire model vibrates.

If I change the load from gravity to enforced motion, that load seems to be applied to entire model I think.

But, enforced motion need to specific line or surface. If I choose specific entry, the other entries do not vibrate or not effect from the load?

3. As you said, I got the results from pre-defined XY plot (like below figure).

If I want to exact result, do I make XY plot from PSD 1 to PSD n at the point of specific node ID?

I will try to the analysis again by referring to your explanation util your reply (if you do that..)

Thanks.

[John_Holtz]

Hi @Anonymous 

1. I am confused because I am not a rocket scientist. (Just an amateur astronomer/space enthusiast ). When doing a random vibration response analysis, I would think that the load is the PSD that is provided. There is no need to scale it. (Or if there is a need to scale the PSD, is multiplying the gravity constant the correct way to do it?) Perhaps you should be doing a static analysis with a 10G load?
2. The entire satellite is not vibrating with the 10G load. The rocket is vibrating with the PSD provided. That vibration is transmitted to the satellite through the payload adapter. The locations where the satellite is connected to the payload adapter is where the PSD is applied to the model. The way to apply the PSD is to put a constraint and "enforced motion > acceleration" at the connection between the satellite and the payload adapter. The other parts of the satellite vibrate at some value other than 10G -- maybe higher, maybe lower. That's why you are doing the analysis!
3. You right-click on "XY Plot > New Plot" and define what you want to graph. You want to graph the acceleration at a selected node, for steps "PSD 1" through "PSD n".

[Anonymous]

Hi, John

I use PSD profile in Dynamic setup. 10G force is just my poor assumption. After I read your comments, I use only PSD profile I think.

I tried to random response analysis again refer to your comments.

But, I met the E5001 fatal error (negative stiffness matrix) when I set the load as enforced motion - acceleration to fixed constraints (magnitude = -1 or -9800 in y-direction, which minus sign means just direction as I know)

I checked the properties of materials (elastic modulus, damping coefficient etc), surface contact (Bond, stiffness factor = 1.0).

Other setups are same as before I attached.

I've searched several times about the error in Google, but I've not found any satisfactory information.

[martin_madaj]

Hello @Anonymous and @John_Holtz,

first I have to admit that the topic of this post is kind of a very thin ice for me, nevertheless...

I assume ASD is the same as PSD. Isn't it that if you want to get the PSD from acceleration, you need to prepare the data, for example with something like this https://econpapers.repec.org/software/dgeqmrbcd/164.htm. I mean:
- first you have some stationary signal (acceleration in time),
- then you use Bandpass Filter Method (see the link above) to isolate different frequency ranges (5-10 Hz, 10-20 Hz,...),
- for the isolated frequency ranges calculate G_RMS = root((1/N)*sum((x_i)^2)),
- finally put it all to a chart of frequency vs PSD (G_RMS) and use it as a load in your analysis.

Regards, Martin Madaj.

[John_Holtz]

Hi @martin_madaj 

Thanks for joining the conversation. I am far from a vibrations expert, but I think your information is for converting a time-based measurement (such as acceleration versus time) to a PSD (power spectral density versus frequency). Is that correct?

@Anonymous has a PSD entered into his model, and I assume that the PSD was specified by his customer or a specification that governs his design. So he does not need to do that type of conversion. The results of the analysis (for the steps/subcases/increments identified as "PSD n, FREQ =") are also a PSD even though the units shown by the software do not indicate that they are a PSD. So when viewing the acceleration XY Plot, is would be an ASD (acceleration spectral density).

Hi @Anonymous.

It is strange that you would be getting an E5000 error when using the enforced acceleration. If you can provide your model, someone will be able to look at it and determine why you are getting an error. (When providing a model, please zip/rar/compress all of the part files (.ipt) and assembly files (.iam).)

Alternatively, you can look at my sample model attached to see how your setup differs from mine. (By the way, the "JSC" in the filename "JSC - satellite hull.ipt" stands for "John's Satellite Company", not the NASA "Johnson Space Center" )

[martin_madaj]

Hi @John_Holtz, you are right, it's my fault I did not read the post more thoroughly.

M.

[Anonymous]

Thanks to @John_Holtz  and @martin_madaj 

I attach my model (.ipt) file.

I can't expect to how model change when you open it.

As I know, you will reset modal, damping and dynamic setups refer to images I attached before.

Input PSD data is Table 2. Modal damping-quality factor is 10. Range of frequency is 10 ~ 2000 Hz.

I have replaced complicate parts to concentrated mass.

My focus is on beam and bar structures.

My major is astronomy and this analysis is a part of development of a astronomical instrument.

So, I am doing this analysis in the lack of basic knowledge or experience about design using CAD.

For that reason, my simplified model is little poor. So, you can difficult to inspect it.

Thanks.

[John_Holtz]

Hi @Anonymous 

There are a number of things in your model that do not make sense to me. Do you have a friend or adviser who you can review the model with  to determine how you should set it up? For example,

1. The material properties for the G10 material are not correct, and this is creating a warning about unreasonable material. I think the value for G is wrong and should be deleted.
2. Why do the concentrated masses have a fully fixed constraint applied to them? (Constraints 20 and 17.) If the mass cannot vibrate, why are you including it in the analysis? Shouldn't the masses be free to vibrate, and this is what causes the stresses in the structure?
3. Why is there an enforced motion applied to the concentrated masses? I do not believe that the concentrated masses are bolted or welded to the structure that is causing vibration. 
4. Under the dynamic setup, you indicate in the Frequency Range to calculate 2948 results. I think that is unrealistic. You only need a few frequencies in between the natural frequencies.
5. The reason for the E5000 error (E5001? E5004? I have forgotten already) is the beams on Physical Property 2 are not fully fixed to the shells. A bonded contact only pins the nodes together, and this allows the beams free to spin about the Z axis. You have 20 "shafts" that are held by bearings and free to spin. You can try using Offset Bonded contact. If that does not work, then you should use the instructions from this article to connect the beams to the shells: Nastran In-CAD: How to connect beam and shell elements
6. Personally, I think your rigid connectors are probably attached to too many faces. But of course I do not know what the physical thing looks like. Look at Connector 19 for example, which connects the Coldbox to the plate. By attaching the rigid body to the entire face of the plate, that indicates the cold box is glued to the surface of the plate. The plate cannot bend, flex, move independently of the cold box because they are connected together so rigidly. Is that realistic?

Good luck.

[Anonymous]

Hi, John

Thanks for your answer.

Unfortunately, peoples around me are all pure astronomers. There is no one who expert about vibration analysis. (Only few persons who can design and thermal analysis). I do most of work. So, I really glad and appreciate to your comments.

1. G value of G10 is temporary to try to avoid E5001 error. I didn't assign any value before. I will check other values again.

2. I couldn't think about that. I just fixed except things that I consider to. Detail like this is what I didn't recognize.

3. That seems to be due to my lack of understanding for the enforced motion setting. Two concentrated mass bolted to the shell structure connected by rigid body. The condition what I think is that beam and bar is free, others are fixed and whole structure vibrates.

4. Frequency range is to compare to the real test results which shows 10~2000 Hz range and 0.675 Hz resolution.

5. Offset bond seems to right as your comments. I will try to that.

6. As I mentioned in 3, cooler and coldbox connect to shell structure by tight bolting connection. So, the shell structure connect to the coldbox can't flex, bend and move independently. If I set wrong to that condition, let me know your comment for that, please.

I will ask your help if I have other problem from the analysis.

Thanks.

[Anonymous]

Hi, @John_Holtz 

I tried to the analysis again. The site about the contact you introduced me to was very helpful.

(offset bond, split shell for matching between contacting points and shell nodes)

But, I got wrong results adapted the enforced motion loads.

The acceleration and displacement values are zero at any nodes on beam and bar structures.

Just points adapted the load moved to assigned direction weirdly.

So, I searched to get any information about the load.

Then, I used the force load to concentrated masses refer to linked video clip below.

(Used mass unit is tonne, so N means tonne·mm/s^2 I think. Therefore, I assigned force loads to each of the two concentrated masses with their own mass)

https://www.youtube.com/watch?v=huTGyuLq_tA

After that, I can get some reasonable results I think.

But, I'm not sure yet about using the force load.

To be exact, I can't understand the difference and used circumstance between the enforced motion and force on Nastran.

In addition,

I'd like to make sure about the analysis.

As I know, the frequency at Mode 1 of normal mode analysis is the natural frequency of the model.

And the result from normal mode is needed to the random response.

So, if I change any setup, I do the normal mode and change to the random response.

When I set the dynamic setup in the random response, I consider to the natural frequency from normal mode.

Is this the right way?

Thanks.