

December 19, 2019 at 2:26 pmsmehboobSubscriber
Dear All
Can anyone help me in the following matter:
I have a 2D steel frame model and i have to apply a time history of random vibration signal at its base. The total time of time vs acceleration data is of 310 sec and signal has a sampling frequency of 128 Hz. So i have total 39680 data points. How can i add this load history in transient analysis? When i choose the acceleration as a load then in the details as shown in figure attached there are some yellow areas, please help me (i) how to set boundary condition, and as i am applying it as base excitation and (ii) how to select direction? (iii) Can i directly import the time history data from excel file to workbench?
If someone has expertise in this side you can also directly share your valuable comments and guidance on my email id: syed.saqib@uettaxila.edu.pk
Regards

December 20, 2019 at 7:09 amsmehboobSubscriber
In workbench 2019 R3 (Academic Version), for the transient analysis. I am applying time vs acceleration history on a base of structure using the "Acceleration" as load type. Once the load type is selected the tabular data dialog box appears on right bottom. Now when i copy my time ans acceleration values from excel file and paste in the tabular data area it pastes only 23 rows on one paste click. For example i had copied 10 rows from excel, now i would have to press Ctrl+V for 5 time in the tabular data area to completely obtain my data there. Is this any software bug/limitation of i am doing something wrong to paste the data?
It is supposed to be pasted all data on one time. isn't it?
Look forward to hearing for any solution from this forum.
Thanks

December 20, 2019 at 1:00 pmpeteroznewmanSubscriber
(i) You should have a Fixed Support that you would choose as the boundary condition.
(ii) Click on the Yellow Box and then click on an Edge that is parallel to the direction recorded by the accelerometer. I assume it is horizontal ground motion, so that would be the Xaxis.
(iii) Yes, you can copy and paste from Excel to Mechanical. It is a bit tricky. I have experienced that behavior of it only taking a few rows. It might help if you have already put 310 seconds in the Analysis Settings as the End Time.
The sampling frequency of 128 Hz is very low. What is the first natural frequency of your 2D frame? If it is higher than 6 Hz, then you do not have an adequate sampling frequency. The sampling frequency should be 20 times higher than the highest frequency of interest in the structure.

December 22, 2019 at 7:24 amsmehboobSubscriber
Thank you Peteroznewman. I was looking you are very helpful and respond to the students with your great knowledge.
Point wise:
(i) Successfully applied boundary condition as fixed support.
(ii) Successfully selected the acceleration direction.
(iii) Data copy and paste from Excel. I had total 39680 data points of total 310 sec. I added 310 steps in the analysis settings, then each step is further divided into 128 substeps. After that i copied data from excel as a set of 100 sec (12800 points) in first step and pasted over in the tabular data column, similarly repeating this i had completed copying of data process in 4 steps. Data successfully obtained in the tabular data without missing any data point.
On the adequacy of samples per second / sampling frequency i am using this literature (Ref. Book: Introduction to Operational Modal Analysis" by Rune Brincker & Carlos Ventura, Chapter 7, Article # 7.2.3). I am attaching its screen shots as well for your ready reference. The structure i am studying having first modal frequency as 3.4001 Hz and as i am concerned about only for first 4 transnational/bending modes with max. frequency in that case is 18.992 Hz so base on Nyquist frequency concept i thought this 128 Hz sampling frequency would be sufficient. Please comment if you have any other information on this and correct me.
Thank You

December 22, 2019 at 7:27 pmpeteroznewmanSubscriber
(iii) You should be able to have one step with an end time of 310 seconds and paste in the 39680 rows of data. I managed to copy 30 seconds of earthquake xyz data or 42,000 rows and paste that into a Workbench Acceleration load. It took a long time for the paste to finish, like more than an hour. Afterward, I extracted the code created, stored it in a text file and used a command object to read that text file into the solver at run time. This sped up the Workbench user interface dramatically for all future model building.
I'm confused about having 310 steps, each 1 second long, and taking 100 seconds of data to paste into step 1. I thought you might have 3 steps, each 100 seconds long. That would make sense.
Data Sample Rate for Transient Analysis
Here is a good article to read.
If you want to do frequency analysis of a signal, then you can use a minimum sampling rate of 2.4 times the highest frequency of interest and if you have the proper antialiasing filter on the signal prior to sampling, then you will have all the frequency content of the original filtered signal in the sampled data. The sampled data and the original filtered signal will have the same frequency spectrum.
But you are not doing frequency analysis, you are using Transient Structural, where the transient signal is recreated in the time domain. That means ANSYS will draw a straight line between point in the table. If those points are spread out with only 2.4 samples/cycle, that will be a very choppy waveform for the solver to integrate, not at all like the smooth original filtered data. That is why 20 samples/cycle is recommended, with 10 as a minimum. You have a 128 Hz sampling rate and have a 19 Hz frequency of interest, so you have 6.7 samples/cycle. That may introduce some noise into the simulation.
Below is a 19 Hz sine wave sampled at 20*19 Hz as recommended. It looks like a sine wave.
Below is the data sampled at the minimum 2.4 samples/cycle, which is adequate for frequency analysis. Transient Structural can take smaller time steps than the sampled data and uses linear interpolation. The graph below is clearly NOT what you want driving your structure.
Here is your 128 Hz sampling rate. Not nearly as bad as the 2.4, but not as good at the 20 samples/cycle.

December 27, 2019 at 4:37 amsmehboobSubscriber
The problem resolved... I am now able to copy paste all my data in once step, yes based on data points it takes some time to show the pasted data in the tabular area while defining the acceleration history.
Secondly, your shared article "Sampling and TimeDomain Analysis" is helpful.
Once again thanks.
Stay safe

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
Ansys Blog
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.
 Solver Pivot Warning in Beam Element Model
 Saving & sharing of Working project files in .wbpz format
 Understanding Force Convergence Solution Output
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 User manual
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 whether have the difference between using contact and target bodies
 material damping and modal analysis
 Colors and Mesh Display

5346

3345

2471

1310

1018
© 2023 Copyright ANSYS, Inc. All rights reserved.