UGNX 8.5 PSD input Vibration Analysis

[thecadguy]

Dear All,

I am new to vibration analysis and could use some direction in UGNX 8.5. My customer supplied me with a PSD input table which plots frequency (Hz) vs PSD (g)2 or (m/s2)^2. There are about 15 entries and I am not sure what solution to use and how to input this into the model. The model is basic plastic ring with four arms pointing toward the center. There are three separate PSD vibration for each (X,Y,Z) direction at each arm.

Approach
There are no constraints other than the four arms that attach to the part that is vibrating.
I am using sol 108 direct response solution and applied an enforced acceleration constraint at each arm.
I created three tables to use for each direction based on the PSD data

Questions
The only units I can find in the table are frequency (Hz) vs acceleration (m/s2).
The PSD data is (m/s2)^2 so do I just take the square root of the provided value and use this acceleration (m/s2) at the corresponding frequency (Hz)?
I did this it resulted in extremely low stresses, almost negligible
Should I be using a different solution instead of Sol 108?
Do I run a Sol 111 and Sol 103 first and try and input the PSD data to apply against the modes analysis? I tried this and it will only let me input displacement or loads no acceleration?


I feel I am real close just looking for some direction. I think my problems would be solved if I could just use the PSD data values directly and UGNX had an input form for PSD.

Thanks in advanced for any help!

The CAD GUY

 

[rothers]

PSD should be normalised by frequency, the units are g^2/Hz not g^2. If so to find g multiply by frequency then take the square root.

 

[thecadguy]

Dear Rothers,

Thanks for the response. This is what I was given in the form of a PSD table. So if I want just the acceleration in (m/s2) I would time the value by the given frequency and take the square root? Next create a table of frequency (Hz) vs Acceleration (m/s2) and apply this as an enforced acceleration at the point of entry?

Thanks,



Grms = 5.68 (55.7 m/s2)

Freq X Y Z
(Hz) PSD(m/s2)2/Hz PSD(m/s2)2/Hz PSD(m/s2)2/Hz
7 5.86 5.86 5.86
9 7.17 7.166 7.166
12 16.288 16.288 16.288
17 1.43 1.43 1.43
42 1.95 1.95 1.95
48 0.39 0.39 0.39
59 0.52 0.52 0.52
63 7.81 13.03 130.3
67 0.65 0.65 0.65
117 1.11 1.1 1.1
123 3.9 6.51 65.12
129 1.3 1.3 1.3
300 3.25 3.25 3.25
650 0.78 0.78 0.78
850 5.21 5.21 5.21
1100 0.65 0.65 0.65
1300 1.95 1.95 1.95
2000 0.065 0.065 0.065

 

[BlasMolero]

Dear CAD Guy,
Under NX AdvSim if you don't have license of NX RESPONSE SIMULATION then the only way to define a RANDOM VIBRATION analysis is go to the solution and click Edit to summon the Edit Solution dialog box:
• In the CASE CONTROL tab click the Create Modeling Object button adjacent to the User Defined Text pulldown menu and press the Keyin Text Button to add the following cards as Text to Insert at Start of Section:
RANDOM = 100
• In the Bulk Data tab of the Edit Solution dialog box, enter the following as User Defined Text and inoput the PSD on a TABRND1 card.
Etc ... Very complex to explain in a forum.

In summary, the NX AdvSim graphics user interface needs to be improved a lot to run with NX NASTRAN advanced dynamics analysis like Random Vibration, Response Spectrum Generation, Response Spectrum Application, etc.. Life is easy running "FEMAP with NX NASTRAN" Basic + "Dynamic Response" module, everything is there, plenty with menus and functions to define PSD excitation and Nastran Output Request for Random analysis.

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/

 

[thecadguy]

Dear Blas,

thanks, I agree the interface is very confusing but I think i did figure it out. Please let me know your thoughts.

I ran a sol 103 response and sweep thru about 100 modes.
I added a response to the results and picked the random event.
I added the enforced motion at the point when the vibration is introduced.
I added an excitation at this enforced motion in three directions. The trick was figuring out the PSD units. Not very intuitive in the function graphing tool. The units were acceleration squared but i did not figure it out until I graphed which added the /HZ to the end. This area needs a lot of work.
I then evaluated the rms stress results which i understand is only 1 sigma. Any thoughts how to get to 3 sigma?
THe PSD input was about 10 frequencies of input at the three directions.

Hope this is the correct path. Takes about 10 hours to run thru all the frequencies ( about 90 modes) on a 4 processor 64-bit machine. Should I have run the PSD against all these frequencies or rather just the forced frequencies of the PSD curve?

Thanks,

The CAD Guy

 

[BlasMolero]

Dear CAD guy,
Regarding units, entering the PSD as G2/Hz will cause all the output to be in G, including stress.
Most analysts we us prefer their stresses in psi or MPa. For output to be in psi, it is required to scale the PSD function so that it is in consistent units, instead of G. For instance, if the PSD input is 0.20 G2/Hz you will have to enter a value of 0.20*(386)2. Since the input is now in (in/s2)2/Hz, all of our output will be in inches, psi and in/s2. Scaling either the acceleration load, or the acceleration load curve will produce the same results, but it is more generally accepted to scale the PSD curve as described above.

RMS von Mises stress for Random analysis
NX Nastran can compute the response of a structure due to random loads. You can request a random analysis with the RANDOM case control command in the frequency response solutions SEDFREQ SOL108 and SEMFREQ SOL111. Random response output includes the response PSD, autocorrelation functions, the number of zero crossings with positive slope per unit time, and the RMS (root-mean-square) values of response. These random output options can be requested on the individual case control commands. For example, the STRESS, STRAIN, DISPLACEMENT, VELOCITY, and ACCELERATION commands.

Beginning with NX Nastran V9.0, when the stress RMS output is requested using the RMS describer on the STRESS case control command, an RMS von Mises stress is now included in the output for those elements that support von Mises stress calculation when computing the response of a structure to random loads.

This RMS stress represents how much stress the structure will experience 68.3% of the time. Statistically speaking, this stress value represents the "1σ" value and will be experienced 68.3% of the time. A "2σ" value is just "2*1σ" and will be experienced 27.1% of the time, and a "3σ=3*1σ" value will be experienced 4.33% of the time. These values represent 99.73% of the stresses.

Best regards and .. good luck!!.
Blas.
The "CAE" guy

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[thecadguy]

Thanks,

How many normal modes do you think is acceptable for the random vibration RMS stress accuracy? I am sweeping between 0 and 2000 hz and it finds 102 modes. This runs the solution time way up high and I was looking for a way to cut down the run times. I checked the .f06 file and it looks like the modal mass effects does not reach 80% until about about 300 hz only in T2. I don't get three directions (T2,R1,R3) until about 800 hz.

My question is how many of the degrees of freedom have to be over 80% to be effective. Is this the right approach. I am looking for some experience in this area to reduce my runs times.

Thanks,

TheCADGUY

 

[BlasMolero]

Hello!,
It is possible that not all of the computed modes are required in the frequency response solution. At an absolute minimum, you should include all the modes whose frequencies lie within the range of forcing frequencies. For example, if the forcing frequency range lies between 200 and 2000 Hz, all modes whose frequencies are in this range should be retained in the modal frequency response analysis. For better accuracy, include all modes up to at least two to three times the highest forcing frequency in the modal frequency response analysis. Residual vectors can also be requested to improve the response by adding the missing static flexibility associated with these higher modes.

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/

 

[thecadguy]

Blas,

Thanks, I actual found the UGNX tool that allows me to deselect the frequencies that have no or little contribution to the mass effects. Out of 100 frequencies I cut the run times down from 8hrs to 2 hrs.

One last strange thing that I found is related to units. The PSD chart I has the units in (m/s^2)^2/hz and (g2)^2/hz. When I use either of these inputs and units I get huge stresses on the part. Like 8-10 times I would expect. My first thought it was the units, my model is in mm, so I converted the (m/s^2)^2/hz to (mm/s^2)^2/hz. A 5.86 value is now a 5860 value.

I ran the larger value with the (mm/s^2)^2/hz units and the stress are more reasonable about 50% of the yield strength. What bothers me is that the results should be the same.

I ran some tests and the (m/s^2)^2/hz and (g2)^2/hz numbers provided results were the same. I know there is a 96 factor between these two. However, I can not believe that these results are correct, the stresses are just off the charts. the differences are on a order of 30 magnitude not 1000 like the conversion between meter and millimeter.

Any thoughts or suggestions? Am I missing something.

thanks

 

[Hibouchka]

Hello,
I am new to vibration analysis, and I have some questions:
I should correlate test with FEM models, in test I make many operations that I don’t know how introduce it in FEM models (subcase,..???)
TEST operations are:
1: Resonance frequencies search in range from 10 Hz to 2000Hz with a constant acceleration of 0.5g
2: Application of first spectral dynamic (PSD (g^2/Hz))
3: Application second spectral dynamic (PSD)
4: Resonance frequencies search in range from 10 Hz to 2000Hz with a constant acceleration of 0.5g
In test condition, I have difference between the first natural mode for step 1 and 4, for every step I should plot displacement (mm) and acceleration (mm/sec2)
My questions are:
For the step 2&3, as the input is PSD ((g^2/Hz)) , how can I get the displacement in mm?
For the step 4 , as I should evaluate the impact of endurance tests, should I make a combination of all others load cases?
Can you help me please?
thanks,