February 7, 2018 at 5:10 pmRana NasserSubscriber
I have some questions about the step controls in transient structural analysis sittings,
First, what is the difference between "time and substep" in the auto time stepping definition? and how this affect the solution of my model?
second, the transient load in my model is an acceleration time history produced from a passing train and measured by an accelorometer installed on the structure which take a reading every .002 seconds, so how good is the step controls that I used in the attached model?
*** The accelerometer that I'm taking about is ch(1) in the drawing pdf. The experiment was on a water structure (regulator), but the attached archive represent a 1 meter strip of the abutment.
February 7, 2018 at 6:54 pmpeteroznewmanSubscriber
I have used accelerometer data in a Transient Structural analysis. I opened your archive and pulled the data out of the acceleration load. There are a issues with your data.
Issue 1) There is a huge 10 second gap in the data.
Delete the first two lines and subtract 10 from the Time values unless you must specifically simulate the first 10 seconds, the acceleration history should begin at zero with no gaps.
Issue 2) The mean acceleration is 0.05 m/s^2 for 200 ms.
When I have acceleration data, it usually starts and ends at zero, and has some oscillation in between. Your data has a mean acceleration of 0.05 m/s^2. Are you trying to impart an impulse force on your structure or just vibrate your structure? If the latter, then subtract 0.05 from all the acceleration values in the Z column and you will be left with just the oscillations.
Issue 3) Your last data point has zero acceleration. If you were trying to impart an impulse force, then you want time to observe the response after the impulse ends at 0.2 seconds, so you will want zero acceleration for 0.8 seconds after that for a total simulation time of 1.0 seconds (or more!).
February 7, 2018 at 8:02 pmpeteroznewmanSubscriber
One more comment about acceleration. Ground motion tends to have displacement and return. That means when a ground impulse wave travels by, it should have negative, positive and negative acceleration, and at the end, the total displacement is zero.
To answer the question about Time Step controls, here is the appropriate time steps for such an event:
ANSYS will interpolate between the values in the acceleration table.
February 8, 2018 at 10:22 amRana NasserSubscriber
issue no. 1: I'm not trying to impart an impulse force on the structure it's just a vibration occurred due to passing trains which were close to the structure. the train takes about 30 seconds to pass and the available accelerometers were 500 Hz frequency, so I had more than 10000 reading for each acelerometer. To impart this acceleration to the model I decided to take a part of the readings which has the high peaks, so I inserted the readings from the second 10 to 10.2 as a trial, but now I after reading you comment I think I must subtract 10 from the part of readings that I have chosen to avoid changing the main function of the imparted data.
issue no. 2: I have already filtered the data coming from the accelerometer and subtracted the mean from it, I have done this for the whole 10000 point. I don't know if I have to do this again for the 100 points that I decided to impart to the model or that will affect my simulation negatively( make me far away from the real data)?
issue no 3: I think I need more explanation for you idea!
about the time step control:
1- The fist 2 rows of the acceleration data are always program controlled, I can't change or delete them!.. by the way what dose N/A in the tabular data steps cells mean?
2- If you wont think that I'm greedy, I want to know what's under the black box when I'm changing the step controls data?!
...And as usual I can't find words enough to thank you peter for your kindness and your continues help. I'm really looking forward to meet you some day I think you are really a good friend!!
February 8, 2018 at 10:58 amRana NasserSubscriber
one more question! what is the program that you used to visualize the acceleration - time history data in the first comment?
February 8, 2018 at 12:52 pmpeteroznewmanSubscriber
Please put your 30 second accelerometer data in a zip file and attach it to your post so I can see the whole record. Also, please describe where the accelerometer was placed.
The program I plotted your data with is JMP, but a very old copy, Version 5.
Consider two curves of acceleration data: red and green curves in the illustration below.
The green curve is the full record of the acceleration data. The red curve is cutting out a piece of the full record. The problem with applying the red data to a transient simulation is that the gradual ramp up to the peak value on the green curve is missing. The red curve is like a sudden impact and it excites higher frequencies in the structure that would not have been excited by the green curve. If you want to use just a portion of the data, you could multiply the data by a Hann window function to ramp up and down the amplitude.
The End Time in your Step Control has to be equal to or greater than the data in the Time column in your acceleration load. Any times greater than the End Time in your acceleration load is labeled N/A. Once your time starts at zero for the acceleration load, you won't have this problem.
February 13, 2018 at 10:15 amRana NasserSubscriber
did you fined the attached files which contains the accelerometer's reading & layout of the acceleorometer's distribution?
February 13, 2018 at 12:13 pmpeteroznewmanSubscriber
Sorry Rana, I only found them now because you added the post above, which gave this thread a new date.
When you edit an old post, or attach files to an old post, the thread doesn't get a new date so I don't know that there was a change. It's better to add a post to attach files so that I will know something changed.
I had a quick look and have attached a zip file for you. I will study this some more later. I'm a little concerned that the spreadsheet showed the units for the channel as µm/m. That is not a unit of acceleration, that is a unit of strain. Are you sure these sensors are accelerometers or are they strain gauges? This question is more important to get right than the choice of which section of time history to analyze.
I also didn't fully understand the pdf showing the location of the sensors relative to the structure. Please expand on the description of where Ch1 is located. Is it on the structure?
February 15, 2018 at 1:05 pmRana NasserSubscriber
sorry for being late, the sensors that we used can read different parameters and we use a compatible software on a laptop in the site to choose the parameter which we want it to read and adjust the units manually, but at the experiment time we set the program to take the acceleration readings and forgot to edit the units! so the reading are acceleration (m/sec^2).
the field test was held on a regulator ( a water head structure that is used to control the water flow in rivers) all the 6 sensors were distributed on the structural elements of the first bay of the regulator -except the raft-. So, yes accelerometer no. 1 was set on the abutment of the regulator vertically.
I have reviewed the attached files and I have taken your notes into consideration and there is no N/A cells any more, but could you please explain how did you extracted c1a file?, this is very useful for me by the way because that's my first field test too and if you don't mined I want to learn more from you, thank you peter for your dedication!!
** the attached file contains my trials to extract the time history sample according to your notes, but it was different from that in ca1 file.
February 16, 2018 at 3:47 ampeteroznewmanSubscriber
I'm glad to know that the data is as you said.
The only difference between your extraction and mine is that you picked your zero one time step away from mine. After deleting one cell, and shifting all cells up one, the two curves are aligned, and only off vertically by a constant of 9e-6 so I think you have done a good job isolating a section of data to use.
Location of Accelerometer on Cart
A cart with wheels rolls over bumps in the floor, which creates a transient vibration in the cart structure. The cart consists of a base where the wheels are attached, and a column with a component on top. One accelerometer is on the base and another accelerometer is under the component where it bolts to the column. The acceleration-time history is recorded as the wheels roll over bumps in the floor.
Take the wheels off the base and bolt the base to a servo-controlled shaker table. Play back the recorded acceleration-time history from the base accelerometer into the shaker table controller. The base, column and component will reproduce a similar transient vibration on the shaker table that was observed when the wheels rolled over the bumps in the floor.
Make an ANSYS model of the base, column and component structure but without wheels, and add a fixed support on the base where the accelerometer was mounted. Now use the base accelerometer data as an acceleration load on that model. The base, column and component will show a transient vibration like it had when the cart was on wheels.
But play back the acceleration-time history from the component accelerometer into the shaker table controller. It will not reproduce the transient vibrations that were observed in the base, column and component. Similarly, insert the acceleration data from the component accelerometer into the ANSYS model with the fixed support on the base, a similar transient will not be seen as was observed when the cart had wheels.
Now unbolt the component from the top of the column where the component accelerometer was mounted, and bolt that component onto the shaker table. Play back the acceleration-time history recorded by the component accelerometer and the component would experience a similar transient vibration that it saw when the cart rolled over the bumps in the floor.
But play back the acceleration-time history from the base accelerometer into to the shaker table and the component will not experience a similar transient as it saw when the wheels were rolling over bumps in the floor.
Make an ANSYS model of the component and add a fixed support to the component where it bolts to the column. Use the component accelerometer as the acceleration load for the ANSYS model of the component. The component model will show a similar transient that was obsvered as when the wheels rolled over the bumps.
Do you see how the location of the accelerometer determines what can be in the ANSYS model if you want to use that accelerometer time-history as an acceleration load to the model?
It seems to me that you want an accelerometer mounted to a stake in the ground to record the ground motion in order to use that data as an acceleration load to a structure that is mounted to the ground. The accelerometer mounted to the top of the structure is seeing the response of the struture to the ground motion, so it not ideal to use as an acceleration load for the ground motion.
A Seismograph instrument may be more appropriate than an accelerometer, since you are trying to record the seismic vibrations in the ground and use that to simulate vibrations in a structure that is built on the ground.
February 17, 2018 at 11:03 pmRana NasserSubscriber
thank you so much for this illustration, I have discussed this issue before with my professor (the discussion was after the filed test so I couldn't do the 2 scenarios) and his opinion was that we are interested in the load which affect the structure directly so we will take the readings of the accelorometer no. 1 (ch1) as an input and verify the model by comparing the acceleration on the structural elements at the same positions of the acceleromrters in the field test with the data comes from the test, so he thought that the dissipation of the load due to the soil between the railway and the regulator will not affect my model because we are taking the readings which represent the real vibration that hit the structure directly
February 17, 2018 at 11:17 pmpeteroznewmanSubscriber
I don't have a clear picture of where ch1 accelerometer was mounted. Do you have any photographs from the field test?
February 18, 2018 at 9:18 amRana NasserSubscriber
The attached file contains pictures for the ch1 accelerometer location, I hope they can illustrate the location clearly!
February 18, 2018 at 11:05 pmpeteroznewmanSubscriber
Thank you Rana, that is a great help.
April 8, 2020 at 10:31 ampsh1988Subscriber
Regarding this topic, I have a query..I am going to do a Transient Structural anlysis on a soil slope..but before that I have done Modal analysis to get its mode shapes and calculate the correct integration time step(here=1/(20*f)=0.003sec). As I am going to apply a real earthquake component(from Peer website), its time steps for acceleration is 0.02sec. Is it ok?(comparing 0.003sec for integration time step and 0.02sec for acceleration time history steps?)
April 8, 2020 at 1:58 pmpeteroznewmanSubscriber
ANSYS will use linear interpolation to obtain an acceleration value for time values between the data in the table. If you fit a spline through the points in the acceleration table, you could resample the acceleration data and provide slightly smoother input data, but that is not required.
April 10, 2020 at 4:15 pmpsh1988Subscriber
1.Could you please elaborate a bit more? I am confused...In acceleration time history data(tabular)-->I used time steps 0.01 for my harmonic loading....In analysis settings,i set initial and max time step equal to what??.....it is written in the manual that it should no more than than 1/(20*f)-->what is f in here? I know that i should do modal analysis, but which natural frequency to consider? As I have to do numerous sensitivity analysis, small time steps will not be efficient....could you please help me to choose the best integration time step?
2. Is the integration step size(time step in transient structural analysis setting) dependant upon the load step size in acceleration time history tabular data?
It is worth mentioning that my loading is of harmonic type(0.005g,0.333Hz)....I have attached my slope geometry here for you..
April 10, 2020 at 9:47 pmpeteroznewmanSubscriber
I pulled the earthquake acceleration data from your project archive, subtracted 10 from the time, and plotted a small snip.
The red dots are the tabular data, the blue lines are the linear interpolation values for times between the tabulated data.
The earthquake was sampled at 0.02 seconds or 50 Hz, which are the red dots.
The simulation has an integration time step of 0.003 sec or 333 Hz. So as the solver steps through those tiny time steps, it will use an acceleration value on the blue line.
I mentioned it is possible to smooth out that data by using a spline fit and resampling. In the plot below, that was done at a sample rate of 333 Hz. Again, this is not required.
Divide 333 Hz by 20 to get 17 Hz. This is the 20 time steps per cycle rule to get good resolution of the motion at 17 Hz.
Since the earthquake was sampled at 50 Hz, there is not going to be any content above 25 Hz. You can see that in the FFT.
There is not much energy in the earthquake above 10 Hz so .003 s is a reasonable time step.
The Modal analysis provides you with the Participation Factor Summary. If you wanted to link the solution of the Modal into the Setup cell of the Transient Structural model to do a MSUP Transient analysis, you would look at that table in the X direction, which is what the earthquake is exciting.
I've never done a Plane Strain Transient Structural. Since the bodies are considered infinite, Workbench does not compute a mass for them, but Modal prints the Participation Factor Summary. The sum of the effective mass at Mode 14 at 24 Hz has accounted for 95% of the mass so 14 modes is plenty for a Linear analysis.
However, you want to use a nonlinear material, so you can't use MSUP Transient Structural, but it is good to know that the cumulative effective mass up to Mode 8 at 17 Hz is 86%.
To answer question 2, no, the integration time step size is independent of the load step size.
It seems that the choice of 0.003 s is a reasonable choice for this model for efficiency.
The inefficiency in the model is that it spends 10 seconds simulating a static gravity load before the earthquake starts. The efficient way to do that is to have Step 1 be 10 seconds but turn off integration and it will become a simple Static Structural solution. You can get that to converge in 4 iterations.
Then step 2 can run with time integration on. There is not much going on after 35 s, do you need to go out to 70 s?
April 14, 2020 at 11:47 ampsh1988Subscriber
Many thanks for your helpful description...This is part of my sensitivity analysis in determining the length of the model(90m-...-180m-200m-220m-240m,...).
under the century city 90degree earthquake component.
So, lets see what i have understood...
As the 8th mode shape contribution in x direction is 86%(more or less sufficient) and its frequency is 17(Hz)--> so based on the relation 1/(20*f max) = 1/(20*17Hz)=0.003(sec), so 0.003 is considered as a reasonable initial and maximum time step. Am I right?(it is really important for me to understand this concept as it is the basis for my future analyses)
some more queries:
1. is only cumulative effective mass fraction in x direction important? when and how should we consider the very parameter in y direction?
2.How did you derive the acceleration-frequency graph from the acceleration time-history data?
April 14, 2020 at 11:51 ampsh1988Subscriber
3.What do you mean by "There is not much energy in the earthquake above 10 Hz so .003 s is a reasonable time step."? How do you conclude that 0.003sec is good by the little energy content above 10HZ? (I drew the fourier amplitude-frequency graph by seismosignal and observed that the vast majority of the seismic energy is below 10Hz).
4. How do you apply the 10sec-static gravity load in step one?(at t=0, acceleration(y)=0 or 9.8066m/s2?)
5. I ran the analysis(it took 12 hours!!), but it did not converge...I need its results to verify my geometry. what should I do?Could you please help me?
In this regard, I have attached my model to benefit from your kind guidance(please consider the ansys file attached to my first post in this topic as I can not attach files anymore....).
April 14, 2020 at 5:50 pmpeteroznewmanSubscriber
Yes, I agree that .003 s is a good step size based on it being adequate to resolve 17 Hz motion in the time history results.
1. Since the earthquake data is only applied in the horizontal X direction, I only looked at that. Also, since the geometry is large in the X direction and small in the vertical Y direction, there was very little Mass Participation in the Y direction.
2. I did an FFT on the acceleration-time history and plotted the result in matlab. There is a nice set of scripts called vibrationdata.
3. A different acceleration load, sampled at a higher rate, say 2000 Hz, might show a large amount of energy at 50 Hz in the FFT. If there were some modes in the model that were near 50 Hz, then you would want to run the Transient structural simulation with time steps at 1000 Hz or 0.001 s time step.
4. Under Analysis Settings, with Current Step 1, change Time Integration from On to Off.
5. Under the Solution Information folder, look at the Solution Output. You can search the text for the word ERROR. Look at what it says there and look above there at the convergence and look for information on why it stopped converging. You can search this site using the details of the error.
The website is a bit broken now so you can't Insert Image or Attach files to replies. Sorry.
April 16, 2020 at 10:43 pmpsh1988Subscriber
Words are not enough to express you how grateful I am for the helpful answers you gave me. I am running my model. If any doubt arise, I will come back to you.
April 22, 2020 at 11:46 ampsh1988Subscriber
April 22, 2020 at 5:24 pmpeteroznewmanSubscriber
Yes, that will be good enough.
April 25, 2020 at 11:22 pmsaifaliSubscriber
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.