March 30, 2020 at 10:54 pmmasud407Subscriber
I would like to apply sunusoidal 1g, 30 Hz acceleration and sinusoidal 1g, 100 Hz acceleration along the horizontal direction at the base of the object. How should I do it? Do I need to use harmonic analysis after modal extraction or using the transient analysis (only) is fine?
For 1g 30 Hz acceleration, I can use acceleration function= 9.8*sin(2*pi*30*time) or displacement function 9.8*sin(2*pi*30*time/((2*pi*30).^2).
Shouldn't it provide the same result?
April 1, 2020 at 3:26 pmWenlongAnsys Employee
A harmonic analysis would be an efficient way to do it. You can add acceleration and apply it to a boundary condition. If you want to use mode combination, you can run a modal analysis first (in other words, do a modal extraction, as you mentioned). Or you can do a full harmonic analysis and it doesn't need modal extraction.
Using transient analysis only and apply a sinusoidal acceleration boundary should also work, but it will take much longer to run. However, in the transient analysis(without MSUP) you will be able to apply nonlinearities. If you want to simulate any nonlinearity, you should go with transient analysis (without MSUP) and it will provide different results from harmonic analysis.
April 1, 2020 at 4:31 pmmasud407Subscriber
Thanks for your reply. I understand that I can add acceleration at the harmonic response. However, how can I add a particular frequency (say 1g, 30 Hz) by using harmonic analysis?
I know how to add acceleration in transient analysis. Yes, you are right that transient analysis takes a lot of time. But how can I add nonlinearities in transient analysis?
April 1, 2020 at 4:41 pmWenlongAnsys Employee
1. You can define the frequency range to be maybe 29~31Hz, then you can find the response at 30Hz.
2. Nonlinearity can be introduced by nonlinear material (softening or cracking or plasticity, etc.), contact (frictionless or frictional contact, etc.), large deformation, and so on.
April 1, 2020 at 6:49 pmmasud407Subscriber
I am a bit confused with the answer is transient analysis. When I apply 1g, 30 Hz and 1g, 100Hz vibration separately, I am getting higher displacement (total) for 30 Hz, not for 100 Hz. The reason is if I convert the acceleration to displacement, then it becomes 9.8/(2*pi*f)^2. So increasing f, increase the displacement that is going to be applied to the structure, therefore, it results in lower total displacement (after simulation) for 100 Hz. Is it normal?
April 1, 2020 at 9:01 pmWenlongAnsys Employee
Higher vibration frequency doesn't necessarily give you higher displacement. It depends on your model's natural frequency. If the natural frequency is around 30Hz, then it won't be surprising that you are getting higher displacement at 30Hz.
April 2, 2020 at 8:24 ammasud407Subscriber
I have tried the problem in both ways (modal+transient, modal+harmonic). I am finding different results. For the first one, I am getting a relative displacement of 377 nm for 100 Hz, 1g acceleration, Whereas, this value is .357 nm for modal+harmonic analysis. I have attached the file and am confused about the right process. Would you please have a look at it?
April 2, 2020 at 2:16 pmpeteroznewmanSubscriber
So increasing f, increase the displacement that is going to be applied to the structure, therefore, it results in lower total displacement (after simulation) for 100 Hz. Is it normal?
Yes, it's normal. It is mathematical.
Acceleration load sine wave with a 1 G amplitude has the following displacement amplitudes:
- 30 Hz = 0.2761 mm
- 100 Hz = 0.02485 mm
ANSYS staff are not permitted to open attachments.
The Modal analysis shows the following modal frequencies.
At 30 Hz, the object is moving nearly 1000 times slower than it can vibrate. All one would expect to see in the output of a Transient model with base acceleration is a rigid body motion.
Looking at the Displacement function in the Transient Structural, the amplitude is 0.0207 mm but there are only 9.5 cycles in 5 seconds. That is 1.9 Hz.
What frequency were you intending to produce?
To see the transient response of an object that vibrates at around 40 kHz, you need 20 time steps per cycle. That means the sampling rate should be 800 kHz or a time step of 0.00000125 seconds. The Analysis settings currently request 50 substeps in 5 seconds. That is a sampling rate of 10 Hz, you need 800,000 Hz.
Under Damping Controls, there is no damping and there is no damping in the material either. Transient response is highly dependent on damping if the object is excited anywhere near its modal frequencies. In this case, since it is so far away, it may not be important.
April 3, 2020 at 1:42 ammasud407Subscriber
Thanks a lot for your reply. Replying to some of your inquiry:
What frequency were you intending to produce?
I am looking for 30 Hz (not 30 KHz) and 100 Hz.
I have changed the units (converted to degree ) and found the attached inputs for 100 Hz.
In the analysis settings, I have provided substeps of 500 for 100 Hz frequencies. Is it okay? I am a bit confused about the example (example of 800 kHz that you mentioned in your last reply). How should I select the sampling rate?
April 3, 2020 at 3:04 ampeteroznewmanSubscriber
Look at the Modal frequencies, mode 1 is 25 kHz. If you want to plot the motion of an object vibrating at 25 kHz, you need to plot 20 points per cycle. If you plot less than 20 points per cycle, you won't see a smooth sine curve, you will see a jagged mess. That means the plotting points or the points that sample the sine curve are coming at a frequency of 500 kHz. Therefore the time step is 1/500000 seconds or 0.000002? seconds.
Now if you shake an object with a first modal frequency of 25 kHz at 25 kHz, that is called resonance and the object will have some response to that input. That means if you are holding the base and moving the base left and right by X mm, the tip will move by more than X mm. There will be some displacement of the tip relative to the base.
But if you shake that object at 30 Hz, and move the base by 0.25 mm, the tip is going to move by 0.25 mm. There will be almost no relative displacement.
You could simulate shaking that object for 1 second and watch it go back and forth 30 times, but you will need to have 500,000 time steps to try to capture the motion of the tip relative to the base. But there will be almost no response.
Now if you had a much, much lower Young's Modulus, and the first natural frequency was 40 Hz, then the sampling frequency would be 800 Hz.
The 20 points per cycle applies to any sine curve in the time domain. You have a 100 Hz displacement function that lasts for 5 seconds. Therefore, you need 100x20 points/second or 100x20x5 = 10,000 points for 5 seconds. You set the Number of Segments to 200 in the displacement function. That number needs to be 10,000. In the analysis settings, you have asked for 500 substeps. That number needs to be 10,000.
Remember, 20 points per cycle. It's a simple rule. If you have multiple frequencies, you have to pick the highest frequency to get the smallest time step. So if the 40 Hz natural frequency is being excited by a 100 Hz acceleration, then it is the 100 Hz that you use to calculate the time step.
April 3, 2020 at 9:07 ammasud407Subscriber
Thanks a lot for your suggestions. It was really insightful. So it means that if the external frequency is higher than the first natural frequency, then I have to use the substeps based on external frequency.
However, if the external frequency is lower than the first natural frequency, can I use the substeps based on external frequency?
As my structure has first natural frequency at 25 kHz, I can understand that I have to have 500,000 time steps (for 1 second) to try to capture the motion of the tip relative to the base. But calculating 500000 time steps takes a lot of time. If I use 100*20*1=2000 (applying 100 Hz for 1 second) substeps to vibrate for 1 second time period, will that be okay?
For 5 seconds, the number will be 10000.
April 3, 2020 at 11:52 ampeteroznewmanSubscriber
If you have multiple frequencies, you have to pick the highest frequency to get the smallest time step. So if a structure has a first natural frequency of 200 Hz and is being excited by a 100 Hz acceleration, then it is the 200 Hz that you use to calculate the time step in order to see the response of the structure at 200 Hz. That is because though the base is moving at 100 Hz, the tip is moving at 200 Hz relative to the base.
Yes, calculating 500,000 time steps for 1 second will take a lot of time. No, you can't take 2000 time steps for 1 second. Say you move the base for a time increment of 1/2000 seconds, how many times will the tip vibrate back and forth in that time? If the natural frequency is 25 kHz, the answer is 25000/2000 = 12.5 times. Think about that. You are trying to track the motion of the tip and plot a sine wave of the motion of the tip and from one increment to the next, the tip has moved back and forth 12.5 times. You can't plot a sine wave from that data. In contrast, if you take 500000 time steps, the motion of the tip in one time increment is 25000/500000 = 1/20 or 5% of a sine wave. In other words, you can plot 20 points along one cycle of the sine wave. This is what you need to accurately measure the relative displacement of the tip relative to the base.
Because computing the time history of a transient can take a very long time, other methods exist to compute the response of a structure to harmonic excitation. That is called Harmonic Response analysis. It is much less computational effort to calculate just the amplitude and phase of the response of the steady state response than computing a transient response. Even less computational effort is needed if a Modal analysis solution feeds into the setup of a Harmonic Response.
April 3, 2020 at 11:34 pmmasud407Subscriber
As per your suggestion, I am trying to do the simulation (with transient response) by applying 500000 substeps.
As per my geometry and properties, I should get natural frequencies closer to 30 Hz only. I am getting way higher natural frequency, How can I check if my natural frequency is correct or not?
As an alternative, I am doing the harmonic analysis (feeder by modal analysis solution) too by using the displacement (maximum) that is created due to 1g acceleration. But how can I define 100 Hz in the harmonic analysis? To do that, I set the range from 99 Hz to 101 Hz in the analysis setting. Is this correct?
April 6, 2020 at 1:16 ampeteroznewmanSubscriber
Structures can only vibrate at their natural frequencies. Vibration means a relative displacement of the tip to the base. The structure has a first natural frequency of 24.58 kHz. That is the frequency you would expect to see if you excite the structure. If you are exiting the structure with 100 Hz (or 30 Hz), you won't see hardly any relative displacement. But you will see the base move back and forth by 0.02485 mm (or 0.2761 mm) because that is the rigid body motion of the base. The tip will just follow along. If you excite the structure closer to 24.58 kHz, the tip will have more relative displacement to the base.
Here are the two images you attached because ANSYS staff are not permitted to open attachments.
April 6, 2020 at 2:22 ammasud407Subscriber
Thanks a lot for your reply. As per my geometry and properties, I should get natural frequencies closer to 30 Hz only (not 25kHz). I am getting way higher natural frequency now. I can understand that if I could vibrate the structure at 25 kHz, I would see the relative displacement. However, applying 500000 substeps is taking a lot of time to simulate. Considering my computational power, It seems impossible for me to get results using these 500000 substeps.
I am confused about the natural frequencies that I am getting. I believe it should me much lower (as per paper too).How can I calculate the natural frequencies manually? I know it's square root of k/m. But how can I get this stiffness (k) for a composite body.
As an alternative, I am doing the harmonic analysis (feeded by modal analysis solution) too by using the displacement (maximum) that is created due to 1g acceleration. But how can I define 100 Hz in the harmonic analysis? To do that, I set the range from 99 Hz to 101 Hz in the analysis setting . Is this correct?
April 6, 2020 at 10:59 ampeteroznewmanSubscriber
If a research paper says the natural frequency should be close to 30 Hz, then your stiffness is too high or your density is too low or your supports are wrong. For example, if there is a blob of material floating in water, then it would have a much lower natural frequency than if the same material is spread out on a rigid surface.
If you can get the natural frequency down to 30 Hz, then to simulate 100 Hz, you will only need 2,000 time steps for 1 second, which may be long enough to see the steady state motion develop after damping damps down the transient.
"But how can I define 100 Hz in the harmonic analysis? To do that, I set the range from 99 Hz to 101 Hz in the analysis setting.
Yes, that is correct.
April 15, 2020 at 8:43 ammasud407Subscriber
I am seriously confused about the modal results. Modal extraction is really easy. All I have to do is to set the bottom surface fixed. Even if setting material properties and doing the modal extraction correctly, I am getting very high natural frequencies. Is there any other thing that I can check to make sure that I am doing the modal extraction correctly?
April 15, 2020 at 12:12 pmpeteroznewmanSubscriber
Modal frequencies are calculated from the body dimensions, supports, and material density and stiffness (Young's Modulus). If you change any of those values by a factor of 1000, you will see a significant shift in the first natural frequency. If you change the supports, such as a beam supported at one end versus both ends, that will also have a large effect on the first natural frequency.
Find a textbook example of a modal frequency calculation. Build a model of the textbook case and demonstrate that you get something close to the textbook answer.
April 15, 2020 at 11:54 pmmasud407Subscriber
I have another basic inquiry. I applied a fixed base condition while performing modal analysis as I need to excite the base along the horizontal direction. The total scenario is vibration will be applied to support-plate on which the cell is placed. If I just want to know the natural frequency of the cell, then is it enough to apply fixed boundary conditions to get natural frequencies?
However, I saw that natural frequencies (first one) go down when I remove the fixed base condition or apply any other type of support other than fixed support. What is the significance of using a fixed boundary condition and not using a fixed boundary condition while performing the modal analysis?
April 16, 2020 at 12:40 pmpeteroznewmanSubscriber
If you have a long, wide, thin beam floating in space, it has a low first natural frequency (mode 7) as it bends along its length, which could be around 1 Hz. Modes 1-6 are zero for bodies floating in space. Adding a fixed support to the long wide side of the beam is the same as preventing any motion on all the nodes on that face. The remaining nodes through the thickness now have extremely high stiffness relative to the fixed nodes. The first natural frequency (mode 1) of the body with a fixed support could be around 100,000 Hz.
If the cell is floating in water and the water is wetting the surface of a glass slide, then the cell is not really fixed to the slide. Floating in a water is a bit like floating in space, but it is not the same. The modes are lower due to the mass of water that has to move.
March 11, 2021 at 8:33 pmGabiSubscriberHi! In this case, how do I calculate the magnitude of the acceleration. I was in doubt!nn
March 11, 2021 at 8:35 pmGabiSubscribernHi! I am realizing that changing the magnitude of the acceleration is not changing the result. What can it be?n
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.