November 20, 2020 at 12:15 pmdardhruvSubscriber
hello,November 21, 2020 at 4:50 ampeteroznewmanSubscriberArray
I haven't opened your model, but looking at the images, I don't see any load applied in the Harmonic Analysis. I don't know what is in the Command object.
The loads applied in the static analysis are only for computing the pre-tension stress and are not harmonic.
November 22, 2020 at 8:18 pmdardhruvSubscriber.
I have used large signal analysis in static and want to use small signal for harmonic.
I have applied load using apdl command
apdl command which I have used.
If its possible then please check my file.
Thanks in advance sir
DhruvNovember 23, 2020 at 3:48 amBenjaminStarlingSubscriber.
You do not need to create the TRANS elements again using the EMTGEN command, in fact this is not possible as it is a linear perturbation analysis of the static structural. In your solver files directory of the static structural, find the ds.dat file. In this file you will see where the EMTGEN command is input.
I have highlighted all you need for your harmonic response. I took those highlighted commands, and placed them in a command snippet, changing 400 to 10. the result I got is shown below at 2.5e6 MHz. I supressed your original command snippet.
.November 23, 2020 at 1:25 pmdardhruvSubscriber.
Hello Mr. BenjaminStarling,
I got same result using your code. But I don't why it is showing distortion in geometry.
I am planning to understand one research paper
Could you please suggest me? Am I going in right direction according to this paper?
First I have to apply large signal (DC) in static then small signal (AC) in harmonic. for that, should I delete degree-of-freedom constraints suing DDELE command??
Thanks and Regards,
Dhruvin.November 24, 2020 at 12:41 amBenjaminStarlingSubscriberHi Dhruvin,
I do not have access to that article so I am unable to understand their modelling methods.
Your question is not clear regarding distortion. Are you referring to the non uniform displacement field? This is due to the very small displacements of this model and the parabolic elements being used. If you swith to linear elements and mesh much finer this displacement field will appear much smoother.
The reason the parabolic elements are doing this is the corner nodes of a parabolic element actually have negative stiffness. This along with uniform reduced integration, and a non uniform mesh, results in this random-esque appearance of the displacement field.
Also to remember is that the displacement field is being applied to the undeformed geometry in the Mechanical application. This is not what is actually happening, the harmonic response is using the deformed shape from the static structural analysis. You can confirm this by viewing the result file in MAPDL.
November 25, 2020 at 12:34 amdardhruvSubscriberThank you so much Benjamin. I will simulate using fine mesh size.
January 12, 2021 at 11:07 pmSean HarveyAnsys Employee.
We noticed your questions in the Ansys Learning channel on YouTube. You asked a few questions. Let's see if this helps.
To perform a pre-stressed harmonic analysis you can do a pre-stressed modal followed by harmonic. This video details the pre-stress modal method.
If you are going to use the full method, you can connect static structural to harmonic as shown below and this will be a pre-stress harmonic using the full method.
-Solve for the modes once, then the solution of the harmonic equations is quick and you can experiment with different loads without having to rerun the modal analysis. In full you will have to resolve all the equations and this can take increased time
-You can use modal damping where the damping ratio is a function of frequency, and this can help in correlating simulation with test
-MSUP harmonic solves fewer uncoupled equations
-If you extract too few modes, you will get inaccurate results, so take care that sufficient modes are extracted
Finally, you had asked about damping and you will also find a newly release damping course on the platform, and in that course we discuss some general guidlines on damping values, but also, how to experimentally compute damping ratios.
I hope this helps. Please let us know. Thank you.
Sean Harvey.May 14, 2021 at 11:25 pmhhuskerSubscriber.
I noticed how you coupled static to harmonic. I am trying to run a harmonic analysis to retrieve frequency response while the structure is prestressed. But I am unable to apply any load in Harmonic analysis when I couple the static structural for pre-stressing. What am I missing?
Haafiz Husker.May 18, 2021 at 4:25 pmMay 18, 2021 at 5:27 pmhhuskerSubscriber.
I was pointing to the fact that I cant apply a unit force in harmonic analysis to the prestressed structure. I was able to do so when using MSUP, but full method is returning much more accurate when not prestressed. So i would prefer to use full method to get the results AM I going fundamentally wrong somewhere in my approach?
Haafiz Husker.May 18, 2021 at 6:15 pmSean HarveyAnsys Employee.
Thanks, just so I understand, you are not able to use a nodal force scoped to a named selection of nodes which can be any region of your model? Maybe I am missing something, and if so, my apologies. Regarding Full and MSUP not matching, have you extracted sufficient modes, and If your unit force is concentrated, you may wish to turn on residual vectors. There is a good video on that topic here https://courses.ansys.com/index.php/courses/topics-in-harmonic-response-analysis/lessons/how-to-utilize-the-residual-vector-method-lesson-2/
Sean.Viewing 11 reply threads
Ansys Innovation Space
- The topic ‘prestressed harmonic analysis’ is closed to new replies.
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.
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.Trending discussions
- 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
- 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
- Defining rigid body and contact
- Colors and Mesh Display
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.