March 29, 2020 at 5:32 amVelocimetrySubscriber
I am working on a transient simulation, where I have the remote force applied as following image. It is changing from zer to 17000 Newtons, every 1/30 th of a second. Basically the 17000 N, force is being applied at 30 Hz in an impact manner.
When I run the transient analysis, after around 0.5 second, my result seems to be flattening out. There is no damping included in the model.(Honestly i want to, however I could not find out the alpha and beta damping co-efficients for steel. How would one get those?)
Any suggestions on what is happening, and why the result is this way?
I have 60 load steps. Each load step's deltaT = 1.6667E-3 seconds, and each load step has 2 sub steps (min), and 5 sub steps (max)
March 29, 2020 at 1:02 pmpeteroznewmanSubscriber
Please show your mesh, support face, load face, remote point and your Modal analysis results.
Proper resolution of a 30 Hz frequency in a Transient analysis requires 20 time steps per cycle. That means the maximum time step should be 1/600 or 1.667e-3 seconds, and you say that is what you intended, but why does the result graph below only shows only 8 points between 0 and 0.125 s which implies a delta T of 1.7e-2? The actual time step is 10 times too large.
March 29, 2020 at 6:23 pmVelocimetrySubscriber
Please find attached mesh, load conditions and the Modal analysis. The remote force is acting on remote point EngineMass.
I realized, I typed an error in the question regarding deltaT. It is actually 1.6667E-2. However, your answer reminded me that my time step should be 1/(f*20). Where f would be 30 Hz for me.
I will re-do the work, with the suggested time step.
These are my questions regarding your comment.
1. What help would modal analysis give me in a situation of transient simulation? I performed Modal + Harmonic before this simulation. Then I realized my forcing frequency is not sinusoidal. So I am just doing Transient, where I am inputting my Force vs Time in a table.
2. Your damping post, was helpful. I also took the liberty to read about damping more. So I realized that there are four types of dampings - viscous, Material, coloumb, artificial damping. Obviously since we are talking about the first two types of damping here. My question would be, I do not have any fluid in my system, or a spring. Can I say viscous damping is zero? ( Also I do not have any spring in the system as well)
3. Are viscous damping and material damping independent of each other?
4. Regarding the Material damping, the post mentions an experiment needed to be conducted, to get the actual damping frequency and its log decrement graph. With no resources for the same, would I be able to get a damping ratio from Modal analysis? Or am I at mercy of various online resources. Even if I chose, online resources damping ratio is a function of frequency.
March 30, 2020 at 1:00 ampeteroznewmanSubscriber
1. The Modal analysis provides the first natural frequency of the structure. You use that information to decide the time step to use in Transient Structural. For example, if the first natural frequency was 500 Hz, you would not waste your time with a time step of 0.01 seconds (100 Hz). At the other end, if the first natural frequency was 5 Hz, you would not waste your time with a time step of 0.001 second (1000 Hz). If you have no idea what the first natural frequency is, how do you choose a time step for Transient Structural?
2. Yes, you can have any one of the four types and they are all additive. Damping applied to the material in Engineering Data is additive with damping applied under the Analysis Settings in the Damping Controls. You can have zero damping for any of those types applied from the material or the analysis.
3. Each type of damping is independent and additive.
4. If you can't obtain experimental data, do a sensitivity study to see how much the response changes for a range of possible damping values.
March 30, 2020 at 1:40 amVelocimetrySubscriber
1. In my case, the first natural frequency is at 11 hz. However, that is not of important to me. Should I still chose 1/(20*11) as my time step? Or should I use 26 hz, which is close to my forcing frequency? I actually ran the case with 1.667E-3, and I noticed a huge difference (see attached). In fact, I tried other time steps and results changed significantly.
2 & 3 - I spent all my sunday reading about damping. I am still lost, with so many resources out there and mixed answers between Structural and material damping. I also went through ANSYS damping pdf.
Is there any article you can suggest, that talks basics about damping, and directly related to terminology of ANSYS? I see you mentioned they are additive, but how are they different though? how is analysis damping different from material damping?
There is an option for damping in Modal analysis and also in Transient structural. Should I write damping values in both locations?
March 30, 2020 at 2:52 ampeteroznewmanSubscriber
1. You should use a sampling frequency of at least 20 times 26 Hz. What is the frequency of mode 2? If the sampling frequency is too low, you can have errors. When the sampling frequency is higher than necessary, you are only wasting time. You should increase the sampling frequency until the results stop changing. This is like the Mesh Refinement Study concept. Make the elements smaller until the stress result stops changing.
2. Yes damping is very complicated. It is further complicated because some types of damping are available in one analysis type and not in another type: for example MSUP Transient vs. Full Transient.
How are different damping coefficients different? That goes back to the equations of motion being formulated by the solver and where the damping term appears in those equations. The ANSYS Damping pdf is helpful, but not completely clear.
If you are doing Full Transient, there is no Modal. If you are doing MSUP Transient, the Modal should be undamped. The damping is applied in the MSUP Transient either as Material Damping or under the Damping Controls in the Analysis settings.
- 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.