

August 4, 2021 at 10:58 amRohit2215Subscriber
Hello Everyone..!!!
I am simulating a structure with a shock of 5g half sine shock wave for a given time like 13 milliseconds.
Is it correct to first analyze the structure in Static Structural Analysis for 5gs of acceleration before performing any transient analysis and is it correct to compare the results of static as well as transient analysis.
In static structural the maximum value of stress is 2465 Mpa and in Transient I am getting different values as I don't know the correct methodology of performing the transient analysis. I have attached some snapshots of what I have done. Please guide me. Thanks to everyone in advance...

August 16, 2021 at 5:51 pmDave LoomanAnsys EmployeeYour methodology is good. For efficiency it would be better to start the acceleration pulse at time = 0, but otherwise everything makes sense. You do a static analysis to determine the nondynamic response. This provides a good comparison with the dynamic response as you suggest. A modal analysis reveals the natural frequency of the structure. In your case it is relatively low compared to the duration of the excitation so a dynamic response less than the static is expected and the peak response occurs long after the peak acceleration. This is the classic response of a low frequency system to a shock loading.

February 17, 2022 at 4:36 amRohit2215SubscriberThanks a lot for your response.

February 17, 2022 at 4:42 amRohit2215Subscriber

February 17, 2022 at 4:44 amRohit2215SubscriberI have some basic queries
1) What should be the boundary conditions for a structure that is mounted on shock mounts. Is it better to simulate the shock mounts by using the springs in all the three directions with defined stiffness and damping rather than assuming the fixed supports, for dynamic analysis.
2) Is it always desirable to fulfill the CFL condition to calculate the minimum time step or number of sub steps.

February 17, 2022 at 10:38 amErik KostsonAnsys EmployeeHi
2) We use an implicit method in Transient Structural in Ansys workbench mechanical for full transient analysis (not mode superposition like you have) which is unconditionally stable,allowing the use of larger increment time steps. CFL is more related to explicit dynamics for instance in the Explicit Dynamics system and LSDyna (explicit solutions).
So for mode superposition transient like you do and for the full implicit (linear no nonlinearities) method in Transient Structural in Ansys workbench mechanical that you use we only need to have a time step that is fine enough to capture the highest frequency (smallest period since T=1/f) of interest. Say in your case from the modes the highest frequency is 30 Hz, then the time step should be one tenth of that smallest period. So the period is (1/30Hz) ~ 0.033s, and thus the time step is equal to 0.003 s . Also I would recommend our course in time integration and dynamics.
As for the boundary, I suppose the fixed supports might give the most conservative (so highest stress) at the base of the structure, but springs might be also possible if the connection stiffness at the base is know which is not always the case unless one e.g., measures it perhaps. So it is up to the user which approach to take, we can not advice exactly which one to use, but that is as we said up to the user and their experience in doing these calculations.
All the best
Erik

February 18, 2022 at 6:26 amRohit2215SubscriberThanks a lot Erik for your support. I will surely go through the suggested courses.

February 18, 2022 at 7:44 amErik KostsonAnsys EmployeeNo worries happy to help .
In your case except of the time step that should be one tenth of that smallest period of interest. So the smallest period is(1/30Hz) ~ 0.033s, and thus the time step is equal to 0.003 s we also need to have a time step that captures your shock, and again we should have a a time step that is say one tenth of the shock period.
In your case the pulse period seems to be about 0.08 s, so 0.003 s is more than enough to capture that schock.
Finally you seem to run the full transient (not mode superposition), so we use the implicit scheme. Have in mind though that if you have nonlinearities since the we need the NewtonRap. iterations for everytime tep, and we might then need a smaller time step than 0.003 to get convergence (so perhaps have substeps maximum say to 10  or define the minimum time step say as a start one tenth of the main time step of 0.003 s, so for the minimum 0.0003s.
All the best
Erik

February 18, 2022 at 9:34 amRohit2215SubscriberOk Got it.
Thanks again Erik.
To add to the discussion the above panel is designed to be mounted in a locomotive. Now a days we came across analysis of products related to defense as well. In which customer specifications provide us the value of shock in terms of Gs and its curve behavior along with the time. Like 57 Gs for 35 mili second full sine wave. Those structures are supported from the bottom as well as from top through the commercially available shock mounts. As per the results provided by our analysis team, our structures demands lot of support members to mitigate the generated stresses and to be within the yielding zone.
However I talked to other manufacturers also but their structure are pretty light weight as compared to ours for the same shock amount and period. I don't understand how but I want to know the correct methodology like selection of time step (solved as above), effect of shock mounts, weather base excitation to be considered or apply acceleration on all bodies, like such other factors which I may not know or our team may be missing to consider for the analysis and we are getting some incorrect results.
I request if you have any solve example of such a problem, please share as that will be a very great help for me.

 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.
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 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
 whether have the difference between using contact and target bodies
 User manual
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Colors and Mesh Display
 material damping and modal analysis

3930

2649

1863

1272

610
© 2023 Copyright ANSYS, Inc. All rights reserved.