July 3, 2021 at 3:51 amhappykiranSubscriber
Hi, I'm running a transient structure analysis for the impact of a cart.
Loading pattern-The cart was loaded with a point mass of 168kg and pushed the cart with a pusher for a distance of 100 mm against obstruction of 1" bump.
This problem was solved in two loading steps -Step1- Settling time due to point mass and step 2- impact loading by pushing the pusher in the X direction (Displacement constraint)
COntacts - wheel to ground frictional with 0.1 as co-efficient of friction and pusher to cart structure frictional with co-efficient of friction as 0.1. The remaining contacts all are bonded
Results- I see that the back wheel of the cart is lifting off from the ground before the front wheel impacts. and after impact entire cart is flying. What could be the reason for this how can I control the cart to remains stay with the ground?July 3, 2021 at 4:07 ampeteroznewmanSubscriberPlease read this discussion, I think you have the same problem, you need to allow time for the cart be in equilibrium with the floor.
July 5, 2021 at 11:30 amhappykiranSubscriberHi, Peter, I have gone through this post. Few couple of things I would like to mention here.
In his video even though the wheel has bouncing action but it still remains in contact with the road. meanwhile in my case it is separated from the ground
I followed all the points like allow the cart to stabilize in the first step keeping y-direction as free.
also, I pulled the bump forward for enough gap to the wheel to rotate. an noticed the same effect.
help me how can I make the wheel remains in contact with the ground
July 5, 2021 at 12:28 pmpeteroznewmanSubscriberYou have an advantage over that other discussion, you are using Transient Structural and not Explicit Dynamics. In Transient Structural, you can turn off Time Integration during Step 1 to allow the structure to come fully into equilibrium with the ground.
Have you created small enough time increments for Step 2 to see the impact clearly?
I can take a look at your model if you attach a .wbpz archive file to your reply and say what version of ANSYS you are using.
July 5, 2021 at 1:08 pmhappykiranSubscriberPeter, Thanks for the option on time integration, and in the second loading step I have used initially as 250 minimum as 100 and maximum as 1e5
I will run one more iteration with time integration off if dint work I will share my wbpz file Ansys version 2020r2
July 6, 2021 at 10:56 amhappykiranSubscriberPeter, any updates on the results.
July 9, 2021 at 10:33 amhappykiranSubscriberPeter, I wanted to know that have you tried any methods?
Please let me know your recommandations
July 9, 2021 at 12:32 pmpeteroznewmanSubscriberI didn't find your post until just now. Sorry! If you put in your reply, then I get a notification of a reply and it is very easy to find your post as soon as you post it and I log on. I will look at your model now.
Also, please reply with the version of ANSYS you are using.
First mistake I found, Large Deflection is Off. This is a Large Deflection problem, turn that On.
Second mistake I found, the Contact with the bump is Far Open. That means it will not be used! You need to increase the Pinball radius until it is Near Open. Another mistake is the wheels are not touching the ground. I added an offset to get that.
I recommend you change the way the point mass connects to the structure. You had a Rigid connection, you should use a Deformable connection. It will be more efficient solving if you just pick 4 edges instead of 2 faces because there will be fewer nodes in the connection.
Another issue is meshing with linear elements and having only one element through the thickness such as the wheel holder. That makes that part stiffer than reality, but can probably remain.
July 9, 2021 at 8:58 pmpeteroznewmanSubscriberThe problem with the system above is there is an instantaneous 900 mm/s velocity imposed at the start of the transient step. This creates an infinite acceleration, which lifts the front wheels off the ground.
A more realistic load would apply a finite acceleration of say 9000 mm/s^2, which is a bit less than 1 G, that is still pretty high. If you apply that acceleration for 0.1 s you can get up to 900 mm/s velocity, then for the next time period, you can set the velocity to a constant 900 mm/s. The cart will travel 45 mm in 0.1 s while it is accelerating. There should be some considerably longer distance before the bump to travel at a constant velocity of 900 mm/s so vibrations in the cart die down before the front wheels hit the bump. That means some damping has to be defined for the transient structural solution.
July 11, 2021 at 6:44 pmpeteroznewmanSubscriberThe video above had the 168 kg point mass lowered below the handle and the velocity of the cart at impact was 3.4 m/s
The video below had the 168 kg point mass at the original height above the handle.
The velocity of the cart at impact was 0.9 m/s
As you can see, the simulation can end at 0.35 s the when you run it for yourself.
July 11, 2021 at 7:36 pmRameez_ul_HaqSubscriber,what should be the difference between the FAR OPEN contact (Yellow) and OPEN contact (Red)?
July 11, 2021 at 7:52 pmpeteroznewmanSubscriberFAR OPEN means those contact elements will be excluded and not used at all. Increase the Pinball Radius to change them to NEAR OPEN.
NEAR OPEN means the contact is open, but the gap is within the Pinball Radius so those contact elements will be tracked by the solver.
July 12, 2021 at 2:50 pmRobAnsys Employeeand I've just deleted a wbpz file from one of Peter's post of July 10th as per https://forum.ansys.com/discussion/29620/delete-post-and-attachment#latest Hopefully it was the correct one!
July 12, 2021 at 3:27 pmhappykiranSubscriber@Rob. Thanks a lot for your help. Can you please remove the videos from youtube which has been uploaded related to this post.
July 12, 2021 at 3:39 pmhappykiranSubscriber,it will be a great favour if you remove the entire post.
July 12, 2021 at 9:40 pmpeteroznewmanSubscriberVideos have been removed from YouTube. You might need to delete your browsing history to remove a locally cached copy on your computer to see that they no longer play from this site.
If you want help with your ANSYS models and can't put them on this site, you can leave me your email address and we can communicate privately.
It's fine by me if you remove the whole discussion.
July 13, 2021 at 3:17 amhappykiranSubscriberThank you for removing videos from youtube
As Peter mentioned it will be great if you delete whole post
July 13, 2021 at 10:40 amRobAnsys Employeeand I've removed the images so think that's anything incriminating gone from our side of the system. I will point out that Student is to be used for educational purposes only, so any and all materials are by definition public domain: read the terms of the licence. If you're working on a commercial project that is not public domain please contact us via the "contact us" button on ansys.com from an official email address to sort out licences etc. Similarly contact us if you're unsure: we can work things out very easily before you do anything in the licence grey areas, it's not easy if we find out during or afterwards.
July 14, 2021 at 11:38 amhappykiranSubscriberThank you for the favor. I understand completely your terms and conditions. this is an academic project. due to some confidential things I requested to remove the contents.
Viewing 18 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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
Top Rated Tags
© 2022 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.