General Mechanical

Transient Structural Analysis

Subscriber

Hi, i am doing a transient-structural analysis of a sandwich viscoelastic cantilever beam. My question is that how can i know the natural frequencies (let say first five natural frequencies) of this structure, because i can't perform the modal analysis as in my case it is a non-linear problem.

• peteroznewman
Subscriber

Here is a relevant discussion, specifically this post which is fairly advanced, mathematically.

If math is not your strong suit, you could have a Transient Dynamics model that performs a sine sweep. Review the time history to look for frequencies during the sweep when the response indicates a resonance has been found.  Here is a relevant discussion on sine sweep of a nonlinear system.

Regards,
Peter

Subscriber

Thanks peter. Yeah i followed the links and these were the questions that i posted before. For natural frequencies can you please mention me steps how to proceed further because i am still stuck and didn't understand even by reading the previous posts. Also the sine sweep method is new for me. I 'd appreciate it if you could help me in this regard. Thanks

i have attached my work. please see the attached file.

Regards,

Subscriber

Hi, i am waiting for the comments on my previous question, especially Peter, Sandeep and bsista. Also i want to ask that, I obtained the input of accelaration vs time and now i am interested in acceleration vs frequency (spectrum) from this time history plot. So, can i do it in Ansys or i need matlab or other software. Thanks

Regards,

• peteroznewman
Subscriber

Right, sorry I didn't notice those were your questions from before : )

Make a version of your model that has a linear approximation for the visoelastic material so that you can run Modal. Reply with the table of the first five natural frequencies. We need to know (or guess) the starting frequency and ending frequency for the sweep.

The acceleration vs time file, is that the base acceleration of the fixture holding the cantilever? Do you have matlab? That would be ideal as there is a good free package called vibrationdata. Please put the data in a zip file and attach it to your reply so I can look at it.

Subscriber

Thanks peter for the help, i have already defined prony constants to my model, but also ogden, i.e, i have considered the core as hyper-viscoelastic. So, can i run the modal analysis for hyper-viscoelastic also?

Secondly, the acceleration vs time is the output of the free end of the cantilever beam. I defined a ramp force at the free end of cantilever beam and the other end is fixed.

Regards,

• peteroznewman
Subscriber

Modal is a linear analysis so only linear material properties are permitted. Linear Elasticity.

Do you mean you have experimental data from an accelerometer fastened to the free end of the cantilever that has an applied force? Please describe in more detail the nature of that force.

Regards,
Peter

• sk_cheah
Subscriber

My question is that how can i know the natural frequencies (let say first five natural frequencies) of this structure, because i can't perform the modal analysis as in my case it is a non-linear problem.

Not sure if it's acceptable to you, but you could apply a very small constant amplitude random broadband load in time-transient analysis. Do an FFT on the responses to identify the natural frequencies. Make sure your excitation is not at a node and can excite all the relevant modes.

Kind regards,
Jason

• hgsdvd
Subscriber

U may find this video helpful.

Good Luck

Muha,

Subscriber

Peter, that is why i asked because in this case now i cannot do the modal analysis.

No, i don't have experimental data, yet we have to do the experiment but it will take some time due to some issues. So, i tried to predict the response through FEM and later on compare it with the experimental one. In simple words " i need to solve the response to the force-time history applied to the end point or other point of the cantilever beam"

The force-time history i assumed to be ramp (assumed) in the ansys and i have attached the picture or it can also be impulse like during experiment when striking the end of the cantilever beam with hammer. After this analysis i got the response of acceleration vs time in the y-direction. The force is shown in the picture attached.

Regards,

Subscriber

Thanks Jason for helpful advice, ok i will look into it. but how can i assure that excitation is not at a node, i mean that if i apply force at the free end of the beam, then it is ok or i have to apply somewhere near the middle of it because in this case i don't know the mode shape in advance.

Subscriber

Muha,

Thanks for your help, actually this video is for linear materials, i.e, linear elasticity. In my case it is a sandwich cantilever beam and it is non-linear. So, we can't use it for non-linear materials. Also mentioned by Sandeep and Peter in previous comments.

Regards,

• sk_cheah
Subscriber

how can i assure that excitation is not at a node

You could apply your load at many different locations. For example, if you are seeking 5 modes, applying random forces at 9 equally spaced locations simultaneously should get you what you need. A pulse load like an impact hammer is good for linear structures but tiny random loads are better for non-linear systems.

Thanks,
Jason

• peteroznewman
Subscriber

I suggested you make a linear approximation of your model so you can run a Modal analysis.  Right now, I don't know if the first natural frequency is closer to 0.1 Hz, 1 Hz, 10 Hz, 100 Hz or 1,000 Hz, but that would be very useful information to know because it can inform how you setup a nonlinear simulation.

Your viscoelastic material has an elastic component. Delete the viscoelastic property and just use a linear elastic material to run the Modal analysis. Say you get a first natural frequency at 30 Hz. It's not important that the natural frequency with the viscoelastic material might be 15 Hz or 45 Hz, what is important is that you can throw out consideration that it might have been 0.1 Hz or 1,000 Hz.

Regards,
Peter

• peteroznewman
Subscriber

You can use this force-time history as input in a Transient Structural and observe the result.

This input force-time history has a very low frequency. A pulse width of 0.1 seconds has a frequency of 10 Hz. If your cantilever beam has a high natural frequency, like 100 Hz or higher, then this input force-time history will only produce a quasi-static response. In other words, the tip deformation will follow the force, x = F/k, which is not very interesting.

If the cantilever has a very low frequency, like 1 Hz, then you will get some dynamic response from this force-time history.

Regards,
Peter

Subscriber

Peter,

I have done the modal analysis as suggested by you and i got the first 6 modes. Please see the picture:

Now please give me some guidelines how to proceed further. Thanks

Regards,

Subscriber

Peter,

Thanks for clarifying this problem. I was trying this force-time history on steel cantilever beam just as an example to check it and i didn't got a dynamic response. Then i checked the modal analysis and found the fundamental frequency to be 98Hz. So, now to make this work i have to decrease the time step, right?

Regards,

Subscriber

Thanks Jason,

If i have understood well, you mean that, at the same time i apply random forces on 9 different equally spaced location, i.e, let say on location 1, i apply step force. On location 2 i apply ramp force and so on? or i should only apply step load on all location at the same time and just change the magnitude of force on each location?

Regards,

• sk_cheah
Subscriber

Simultaneous multiple inputs need inputs that are not coherent. That may be harder for you to do. Sorry I suggested this earlier.

An easier way is to sequentially apply random forces. For example, run first model with random forces at location 1, run second model with random forces at location 2 etc. When you identify resonant frequencies from each model, much of it should be the same.

Kind regards,
Jason

Subscriber

Jason,

Thank you so much for your patience and help. I will try to do it in parallel to the procedure suggested by Peter, and it will be good to compare the output from both methods and this will also give me confidence on my results. Meanwhile, if i face any problem related to your method i will ask you through this forum.

Regards,

• peteroznewman
Subscriber

If what you want is to have a force impact on the tip of the cantilever, then the reciprocal of the pulse width time has to be smaller than the frequency you are trying to excite.

In the example of a pulse width from your force-time history above, that is a 10 Hz frequency. Apply that to a cantilever where the first natural frequency is 100 Hz and the tip will just follow the force down and up and there will be no oscillation after.  Apply that to a cantilever where the first natural frequency is 1 Hz, then you will see some oscillations of that first mode.

One of the lower modes will be a twisting mode, but if your force is symmetric across the width, it won't excite the twisting mode.

Regards,
Peter

Subscriber

Peter,

Thanks for your explanation. I already done it, when you mentioned the problem in the yesterday post and it is now working fine. I changed the time-history plot and also added structural damping.

But, regarding the main problem of visco-elastic cantilever, in which you told me to find the modes by making it linear model. I have done it and attached the image of first 6 modes of beam yesterday. Now, what else should i do next for finding the natural frequencies? If you remember, you mentioned that we have to use Matlab for this and use sinesweep.

Regards.

• peteroznewman
Subscriber

I like Jason's idea of using different models to apply random vibration force at different locations to identify resonant frequencies in your cantilever.

For example, if you slice your model at three planes, 25%, 50% and 75% of the length, you will have four models. On each model you will apply a force-time history.

Your cantilever looks like it will go sideways as well as vertically and it will probably twist also.

Use the vibrationdata GUI in matlab to Generate Signal and make four random vibration force-time histories that have X and Y components (let's ignore Z for now) for two force inputs. Apply one force to the bottom of the sandwich and the second force to the top of the sandwich on one of the four locations.

Pick four vertices along the top and four vertices along the bottom of the cantilever and output X and Y displacement-time history and use vibrationdata in matlab to look at the FFT or the PSD of those 16 signals.

From the Modal analysis, there is a mode at 316 Hz, but you only asked for 6 modes. There are higher modes, but do you want to find them?

Sampling Frequency

In order to see a 316 Hz frequency, you need to sample at a minimum 2 times or 632 Hz. I recommend you sample much higher than that, say at 1000 Hz which is a 1e-3 second sampling. Under Analysis Settings, you only need one step under Step Controls but you must set the Maximum Time Step to 1e-3 seconds.

In order to drive a 316 Hz response by a time-history input, the minimum sampling frequency is 10 times or higher. In matlab, Generate Signal, and select white noise with a Low-Pass cutoff of 400 Hz. use a sampling frequency of 4000 Hz to generate a 1 second long time-history.

If you want a larger input, you can type in a larger value for Std Dev.

Perhaps Jason will have some other comments.

Regards,
Peter

Subscriber

ok Thanks peter for your detail explanation, I tried the first step as suggested by Jason and you and created 4 different force-time history. I just changed the sampling frequency in the vibrationdata gui and got 4 plots. Here is one of the force-time history plot. Please check it, is it ok? The rest of the parameters are same as in the picture you posted yesterday.

Regards,

• peteroznewman
Subscriber

Looks good.  Do all four white noise variables have the same sampling frequency?  You want them to have the same number of rows (4000) because you want to export them into Excel to create the ANSYS input which takes one of the variables that has two columns: time and accel then add the accel column from the other variable and then fill the fourth column with zeros to make a file that will look like this:

0.00025  -0.742235  1.243492  0.0
0.00050  -0.104845  0.945108  0.0
0.00075  etc.

That will be the Force input file for the force applied to the top edge of the beam. Repeat with the other two matlab variables to make a Force input file for the force applied to the bottom edge of the beam.

You might need to scale these number up by multiplying them by 10 or 100, or pasting them in using different units if, after running a Transient solution, the response at the 16 points is too small.

It will be quicker to duplicate this model and re-scope the forces to the next station since pasting in 4000 rows of data might take some time.

Subscriber

Peter,

No, i defined the sampling frequency different like:

1.  Force1=1000Hz, Force2=2000Hz, Force3=3000Hz, Force4=4000Hz

2.  About the following part (columns), i didn't understand. Can you please give a simple example

0.00025  -0.742235  1.243492  0.0

0.00050  -0.104845  0.945108  0.0
0.00075  etc

3. You mean multiplying the force magnitude by 10 or 100, so to get a big response?

4. Just i was wondering that as the top and bottom plate are of steel but do Ansys consider the structural damping (material) automatically or it needs to be entered and also for the non-linear material?

Regards,

Subscriber

Peter,

I also tried just as an example with a ramp input force and got the output of acceleration-time history of the free end vertex, then i find the FFT of this plot by using vibrationdata gui and i got the following peak frequency at approx 50Hz

• peteroznewman
Subscriber

FFT plot looks good.  If you close that Figure, the one behind it is the one I use as it does't show the Phase plot at the top.

1. Make all four matlab white noise variables have the same sampling frequency. Just hit Calculate to get a new random sample.

2. Double click on the matlab variable Force1, you will see it has two columns: time and acceleration.  If you copy and paste the data from matlab to Excel, you will have two columns.  Now double click on the matlab variable Force2, it also has two columns, but column 1 is identical to column 1 from Force1.  You only need column 2 from Force2. Copy column 2 from Force2 and paste it into column C in Excel. Finally type a 0.0 into cell D1 in Excel and copy and paste that down through all 4001 rows.  Now you will have in Excel four columns: time, accelX, accelY, accelZ that is suitable for pasting into ANSYS Force-time history.

3. Yes.

4. Put damping into the steel material. Make a small model of just one steel cantilever and verify that you get different results as you increase the damping in that material.

Regards,
Peter

• sk_cheah
Subscriber

Make sure your time period is a lot longer to have a finer frequency resolution.  [ frequency resolution = sampling frequency / block size ].

For the same sampling frequency in the most recent plot, I would suggest you increase the time period by a factor of 10. Plot your y-axis in log scale to better distinguish signal from noise.

Kind regards,
Jason

Subscriber

Peter,

I have generated 4 force-time history with same sampling frequency as you mentioned in the last post and also prepared the excel sheel. Now i am trying to input this into Ansys but  I have student version Ansys, so will it perform the computation of 4000 data points?... I mean there is no restriction on time taken to solve the model?

Regards,

Subscriber

Thanks Jason, Sorry i didn't understood well..you mean to refine the time steps, i.e, decreasing time-interval in the time-history plot so as i can get finer frequency resolution because this is the output i got from Ansys, the acceleration-time history. So, how can i increase the time-period of the output?

Regards,

• peteroznewman
Subscriber

There is no limit on solution time or number of points in a Force-time history for the Student license, only Geometry body (50) and face(300) limits and Node or Element (32,000) limits.

How many cores do you have on your computer?  If it is four or more, did you configure ANSYS Solve Process Settings to use them?

Regards,
Peter

• sk_cheah
Subscriber

I meant to suggest you increase your total simulation time while maintaining your time step. If you had it at 1s before, increase it to 10s.

Kind regards,
Jason

Subscriber

ok, Thanks Peter, Yeah, it is four core ( core i7 ). No, I don't know about configuring "ANSYS Solve Process Settings".

Subscriber

Jason,

ok got it. I will try to increase it. Thanks

Regards.

• peteroznewman
Subscriber

See this post for configuring the solver to use 4 cores.

I agree with Jason that a longer simulation time has some benefit, but you want 4000 sample points/second in the Force inputs and from my experience with xiaofuli, once you get up to 20,000 samples, Workbench takes a really long time to import the data. You might back off to 2000 Hz sample rate on the force to mitigate the slow down on the computer and maybe try 5 seconds instead of 10 seconds.

Regards,
Peter

Subscriber

Thanks peter,

I followed the post you shared and made changes in the "solve process settings". Yeah, when Jason suggested to increase it to 10 seconds so that what i was thinking that it will take too much time. So, it is best to back to 2000 sampling rate and 5 seconds.

Regards,