August 30, 2019 at 4:38 ampushkarkawaleSubscriber
August 30, 2019 at 11:08 ampeteroznewmanSubscriber
There is one error message, the second message is a warning.
I don't have ANSYS 19.0 installed, so I can't give you back a model you can open.
The shell model has a center vertex that is fixed. That is a very concentrated support for a dynamic model. A hole at the center would be more realistic.
The thickness of the shell is 200 mm and the part is 1000 mm square. That is a very thick piece of steel. It is more like a brick than a plate. Did you mean for it to be 200 mm thick?
I remeshed it with 20 mm element size to fit in the Student limits and you don't need it to be meshed with 5 mm elements, that is unnecessary and will slow down the solution time.
RULE 1: Always run a Modal analysis to learn about the natural frequency of your structure before you run a Transient Structural. If you do that, you will find that the first natural frequency of this structure is 17 Hz while the second is 158 Hz. The period for 17 Hz is 59 ms and the period for 158 Hz is 6 ms. Keep that in mind.
The acceleration load has a time-history using a 2 ms sample interval which is a sampling frequency of 500 Hz. Here is the first 0.1 seconds of that acceleration load.
It looks like a sinusoidal signal. If I do an FFT on this signal, I find out it is exactly 80 Hz (period 12.5 ms) with an amplitude of 252 m/s^2 or 25 g.
RULE 2: Use 20 samples per period for Transient Structural. That means the signal should be sampled at 20*80 = 1600 Hz (period 0.625 ms). What this means is that your input data is undersampled. It is sampled at 500 Hz (2 ms period), and should be sampled at 1600 Hz.
This rule applies to the time step for the simulation. If you want to see the effect of the second mode of vibration of the plate at 158 Hz, you need a time step that is 20 times higher or about 3 kHz. That means a time step of 3E-4 seconds. You have used a time step of 0.1 seconds. That is why your model doesn't converge. Here are the settings that will let the model run easily:
Here is the first 0.2 s of response of one corner of the brick. It is about 0.06 mm amplitude.
You have an end time of 20 seconds. That is a waste of time. Are you really interested in the startup transient of the vibration, or are you interested in the steady-state vibration response of the structure? In either case, you are missing a very important input to the model.
RULE 3: Use Damping. Under Analysis Settings, expand the Damping Controls category. You should never run a Transient Structural or a Harmonic Response analysis with zero damping.
So that has fixed your error. But there is a much more efficient way to get the maximum amplitude of the corner and that is to use a Harmonic Response analysis. The benefit of that analysis is it will take a tiny fraction of the time it took to solve the Transient Structural model. Let me know if you want to know more.
- 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.