December 12, 2019 at 1:37 pmmkosinSubscriber
I am a beginner in modal analysis. I'm trying to simulate a hammer impact test on a steel bar.
I did research with a modal hammer and now I want to try to do the same in Transient Structural. Acceleration results from Transient Structural analysis in places of accelerator gluing are very different from the results obtained in the tests. The test stand is shown in Fig. 1. The rod is attached to the steel plate with a neodymium manesque. Accelerometers are attached to the top of the rod.
In the Transient Structural analysis I added the load I received from the tests (Fig. 2), Δt = 0.00004 s. Rod attachment as a fixed support.
What am I doing wrong?
Thank you in advance for your help.
December 12, 2019 at 1:58 pmpeteroznewmanSubscriber
What direction are you hitting the rod? Axially?
Please show the results from the Transient Structural model.
Please show the measurements from the accelerometers.
You can attach .zip files on these posts, so you can put spreadsheets, Powerpoint files etc. inside zip files.
Please show the structure of the rod and attach the Workbench archive .wbpz file.
In your reply, please say what version of ANSYS you are using.
December 12, 2019 at 11:24 pm
December 12, 2019 at 11:24 pmsk_cheahSubscriber
December 13, 2019 at 2:50 pmmkosinSubscriber
Thank you all and sorry for the late reply.
How can I add a .wpbz file to the discussion. It is big after compression.
December 13, 2019 at 7:00 pmpeteroznewmanSubscriber
You can reduce the file size of the .wbpz file if you go into the Model and right click on the Mesh and Clear Generated Data. Then save the project, then create the Archive. If the file size is < 120 MB you can attach it here.
If the file size is > 120 MB and you have Gmail, attach it to an email. That will cause it to upload to your Google Drive and put a link to the file in the email body. Copy that link and paste it in your reply.
December 13, 2019 at 7:54 pmpeteroznewmanSubscriber
You didn't answer the question about the direction of the hammer strike. Building on the comment by sk_cheah, the natural frequencies in the rod are probably much higher in the axial direction than the bending direction. Also, the flexibility of the accelerometer mount could be higher for axial vibrations because of the tipping moment on the accelerometer compared with bending vibrations of the rod where the accelerometer mount is seeing axial forces in its connection to the rod.
The rod mounted to a magnetic mount has its own flexibility, especially in bending modes. You may get much better correlation between measurement and model if you lay the rod on a very soft pillow or a pair of foam wedges and hit it in the center to excite a bending mode. In the Modal analysis, have no support and ignore the first six zero frequency modes.
December 14, 2019 at 9:22 ammkosinSubscriber
Mr. peteroznewman, I attached the test data and the Ansys file to the Excel file. I use answer 18.1. The direction of the hammer was axial to the bar. I tested a steel bar.
Thanks again for your interest.
December 14, 2019 at 3:10 pmpeteroznewmanSubscriber
@mkosin, this site has a short list of allowable file extensions that can be attached. One of the allowed types is .zip file. That means you can put anything in the .zip file and attach that. The file size limit is 120 MB.
Also, this site will automatically put some posts into an approval queue so you won't see it posted until staff or a moderator approves the post in the queue. It doesn't help to post it again and again. They just pile up in the queue.
December 15, 2019 at 4:36 ampeteroznewmanSubscriber
ANSYS Modal Analysis
You should always run a Modal analysis when doing any kind of Dynamics study. The Modal analysis shows the frequency of the axial vibration mode is 6,333 Hz. To capture that frequency in a Transient Structural analysis requires 20 times that frequency for computing the response, which means a time step of about 8e-6 seconds. In your Transient Dynamics model, the Time Step is 4e-5 seconds, which is about 5 times too large.
On the other hand, if you physically support the bar on a pillow or foam wedges and hit it in the center, the first natural frequency with no fixed support is Mode 7 at 3,191 Hz, and 20 times that makes a time step of 1.5e-5 seconds, which is more reasonable.
I only see one channel of data for each accelerometer. I expect that is because those are single-axis accelerometers, which is fine, but that means they are recording accelerations perpendicular to their mount and are not directly measuring axial vibrations. That means exciting axial vibrations by hitting the hammer axially on the end was not the best choice. It would be better to excite lateral or bending vibrations by hitting the hammer on the center of the rod.
The hammer impact force lasts 6e-4 seconds which tends to excite frequencies in the 833 Hz range. You should select a harder tip to install on the hammer to reduce the impact force duration to get it closer to the 3 kHz first bending mode of the unsupported rod.
December 15, 2019 at 10:15 ammkosinSubscriber
Thank you again for your reply. I will refer to the comments given. You can see I have to devote a lot of time to these issues.
I don't want to exaggerate but you're priceless.
- 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.
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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- 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
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.