How can I simulate a vibration force on a steel structure and get nodal accelerations as time series
-
-
August 5, 2021 at 4:43 pmHuda111Subscriber
I have a 4 floors steel structure, and I want to simulate a vibration force in order to get accelerations in nodes as time series, I'm wondering witch type of analysis will be most suitable and how can i get the data I need to explore for other reasons.
Thanks in advance.
August 6, 2021 at 1:39 ampeteroznewmanSubscriberThere are a few possible dynamics analyses you could do.
A Transient Structural analysis will compute a time history response of all the nodes to a time history input of ground motion at the nodes on the ground. The problem is you have to come up with the time history of ground motion. There are sources that provide the acceleration time history record of earthquakes that you can download and use in the analysis.
A Response Spectrum analysis will compute the peak response of all the nodes to an input acceleration spectrum. The acceleration time history of an earthquake can be converted into an input acceleration spectrum.
A Harmonic Response analysis will compute the response of all the nodes to a sinusoidal ground motion and sweep over a range of frequencies. That is generally more appropriate for the frame supporting a machine that creates a harmonic vibration and is less relevant to a building, although wind can cause a harmonic forcing function.
August 6, 2021 at 3:35 pmHuda111SubscriberThank u a lot for ur suggestions, yet I can't make up my mind about one of the suggested analysis.
The data I need reflect the acceleration spectrum / time history in each node , how can I get that please .
Best regards.
August 6, 2021 at 6:53 pmpeteroznewmanSubscriberOutput of an acceleration spectrum is computed in a Response Spectrum analysis.
Output of a time history is computed in a Transient Structural analysis.
Tell me about the vibration input data that will apply a force to the structure. Where is the force applied? What is the magnitude of the force? What is the frequency of the vibration? Is the vibration continuously present, like an unbalanced motor, or is the vibration caused by a specific event that starts and ends? Do you have a time history for the input force or do you have an acceleration spectrum?
Best regards Peter
August 7, 2021 at 6:05 pmHuda111SubscriberI'm really grateful for ur response
The vibration is applied in the base (9 nodes/support fixe), I want to semulate a 30 seconds vibration and I want the acceleration in nodes during this time frame, can I do that with a command line (APDL) in mechanical, if so which one? Or is there another way to get them ?
Best regards
Houda
August 7, 2021 at 7:00 pmpeteroznewmanSubscriberDear Houda Okay, you answered where the vibration is; at the base nodes and you said the duration of the vibration is 30 seconds.
What direction is the vibration motion? I assume it is in the plane of the ground, and not vertical (Y axis). But at what angle? Is it along the X axis or the Z axis or at some angle in between? The kind of vibration is called ground motion.
Vibration is a very general word. There are different types of vibration. The simplest type is sinusoidal. For example x(t) = A*sin(wt) where A is the amplitude, w is the circular frequency and t is time. Do you want to apply sinusoidal vibration?
The amplitude can be in terms of acceleration, velocity or displacement. Acceleration amplitude is sometimes in the units of G or g which is the acceleration due to gravity, commonly set to 9.8 m/s^2. What amplitude do you have specified for the ground motion? Make sure to include the units.
The frequency of vibration is another required part of a sinusoidal vibration specification. The frequency of vibration is usually specified in the units of Hz, which is cycles per second where a cycle starts at the center, goes left, goes right and back to the center. Frequency f in Hz is related to circular frequency w by the equation: w = 2*Pi*f because that is how many radians are in one circle.
Another type of vibration input of ground motion is an earthquake. This motion is not described by a sinusoidal function, but the acceleration of the ground motion is recorded by seismic instruments and that data can be used in a Transient Structural analysis to replay that ground motion as input to a building in simulation.
August 7, 2021 at 7:05 pmHuda111SubscriberActually the excitation is in the y axis
August 7, 2021 at 7:30 pmpeteroznewmanSubscriberWhen you say the excitation is in the y axis, is that in the plane of the ground or is that vertical?
Assuming the vibration is sinusoidal:
What is the Amplitude (with units)?
What is the frequency in Hz?
The first thing you should do is run a Modal analysis on your building frame. What is the frequency of the first mode?
Look at the statistics for the Geometry where it shows you the properties. What is the Mass of the frame? Does that equal the mass of the building? If not, you need to add mass to the model to make them equal. There is a Distributed Mass object that can be added to the model.
August 7, 2021 at 7:37 pmHuda111SubscriberI don't have the exact values, because I'm waiting for the characteristics of the vibrating table for the real test, so I'm going to start with random values to get accelerations data for my python algorithm, that's why I need acceleration in nodes at each second of the excitation to compare them first with the data I'll get from sensors in real test and for other uses also.
Thank u
August 7, 2021 at 7:51 pmpeteroznewmanSubscriberWhen you say the excitation is in the y axis, is that in the plane of the ground or is that vertical?
Please insert an image into your reply showing the coordinate frame of the model in ANSYS.
Is the y axis of the table the same as the y axis of the model in ANSYS? If not please insert another image showing the coordinate frame of the table.
Since you have a physical structure mounted to a table, the table is being driven by an input signal. The input signal could be a Sine Sweep. That means there is an amplitude A and the frequency sweeps from a low value to a high value. It would be good to know these numbers.
The first thing you should do is run a Modal analysis on your building frame. What is the frequency of the first mode?
August 8, 2021 at 5:32 pmHuda111Subscriberhello again,
I already performed the modal analysis to my structure, extracted the first 10 modes, the first frequency is 21,88 , the y axis is vertical in both cases (structure and table) , assuming that we have both the amplitude and the frequency of the input signal, how I'm going to extract acceleration as function of time in each node ?
best regards
August 8, 2021 at 6:15 pmpeteroznewmanSubscriberThere are two ways to extract that information: Harmonic Response and Transient Structural.
Harmonic Response will give you the steady state solution. Every node will have a harmonic motion and the solution will tell you the acceleration amplitude and phase of each node for each axis direction for each frequency in the range requested. For example, you could request frequencies from 10 Hz to 110 Hz in steps of 2 Hz. Therefore you can output a table of 50 frequencies, with the amplitude and phase of each node in three directions. There are 9 nodes x 4 floors x 6 outputs = 216 outputs x 50 frequencies = 10,800 pieces of information to describe the motion of the structure over that frequency range. The acceleration function over time is simply Acc(t) = A*sin(2*pi*f*t+Phase) where the Phase is in radians and A is the amplitude in m/s^2 and f is the frequency in Hz.
Transient Structural will give you 3 directions of acceleration at each node at each time step for one frequency. If the highest frequency of interest is 110 Hz, you need 20 time steps to capture that, so the sampling rate is 2,200 Hz. That means over 30 seconds there will be 66,000 time steps. Multiply that by the 3 directions x 36 nodes and you will have 7,128,000 pieces of information for one frequency. Multiply by 50 for the same frequencies as above for a total of 356 million pieces of information. It is hard to summarize that much data. That is why Harmonic Response is an attractive alternative to Transient Structural when the steady state response to a harmonic input is desired.
It will be easiest to show you how to build those models either in a recorded video or live during a Skype meeting. Would you like to schedule a Skype meeting?
Here is my discussion that includes a video on Harmonic Response: /forum/discussion/687/bridge-building-in-spaceclaim-with-modal-and-harmonic-response-analysis
There are free courses on this site that would be beneficial to watch to help you understand your model.
/courses/index.php/courses/mode-superposition-method/
/courses/index.php/courses/topics-in-harmonic-response-analysis/
/courses/index.php/courses/harmonic-analysis-of-structures/
/courses/index.php/courses/damping-effects/
/courses/index.php/courses/time-domain-dynamic-problems/
It will be easier if I have your Modal analysis. In Workbench, use the File, Archive menu to create a .wbpz file type and attach that to your reply. Also say what version of ANSYS you are using.
August 8, 2021 at 6:33 pmHuda111SubscriberA Skype meeting would be great, so that I can give u more details about the model, or can u give me ur IG or email so I can reach out to you?
Thank you
August 8, 2021 at 6:35 pmpeteroznewmanSubscriberI wonder why the shaking is vertical. Building typically are given horizontal accelerations to simulate earthquakes.
August 8, 2021 at 6:37 pmHuda111Subscriber
August 8, 2021 at 6:38 pmpeteroznewmanSubscriberFor now, please say the ANSYS Version and send me your .wbpz file. Thanks.
August 9, 2021 at 2:29 ampeteroznewmanSubscriberMore videos:
Viewing 16 reply threads- The topic ‘How can I simulate a vibration force on a steel structure and get nodal accelerations as time series’ is closed to new replies.
Ansys Innovation SpaceTrending discussions- Problem with access to session files
- Ayuda con Error: “Unable to access the source: EngineeringData”
- At least one body has been found to have only 1 element in at least 2 directions
- Error when opening saved Workbench project
- Geometric stiffness matrix for solid elements
- How to select the interface delamination surface of a laminate?
- How to apply Compression-only Support?
- Timestep range set for animation export
- Image to file in Mechanical is bugged and does not show text
- SMART crack under fatigue conditions, different crack sizes can’t growth
Top Contributors-
1191
-
513
-
488
-
225
-
209
Top Rated Tags© 2024 Copyright ANSYS, Inc. All rights reserved.
Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.
-
The Ansys Learning Forum is a public forum. You are prohibited from providing (i) information that is confidential to You, your employer, or any third party, (ii) Personal Data or individually identifiable health information, (iii) any information that is U.S. Government Classified, Controlled Unclassified Information, International Traffic in Arms Regulators (ITAR) or Export Administration Regulators (EAR) controlled or otherwise have been determined by the United States Government or by a foreign government to require protection against unauthorized disclosure for reasons of national security, or (iv) topics or information restricted by the People's Republic of China data protection and privacy laws.