General Mechanical

General Mechanical

Transient Structure | Impact Analysis

    • happykiran
      Subscriber

      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?

    • peteroznewman
      Subscriber
      Please read this discussion, I think you have the same problem, you need to allow time for the cart be in equilibrium with the floor.
    • happykiran
      Subscriber
      Hi, 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

    • peteroznewman
      Subscriber
      You 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.
    • happykiran
      Subscriber
      Peter, 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
    • happykiran
      Subscriber
      Peter, any updates on the results.
    • happykiran
      Subscriber
      Peter, I wanted to know that have you tried any methods?
      Please let me know your recommandations
    • peteroznewman
      Subscriber
      I 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.

    • peteroznewman
      Subscriber
      The 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.
    • peteroznewman
      Subscriber
      The 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.

    • Rameez_ul_Haq
      Subscriber
      ,what should be the difference between the FAR OPEN contact (Yellow) and OPEN contact (Red)?
    • peteroznewman
      Subscriber
      FAR 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.
    • Rob
      Ansys Employee
      and 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!
    • happykiran
      Subscriber
      @Rob. Thanks a lot for your help. Can you please remove the videos from youtube which has been uploaded related to this post.



    • happykiran
      Subscriber
      ,it will be a great favour if you remove the entire post.
    • peteroznewman
      Subscriber
      Videos 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.
    • happykiran
      Subscriber
      Thank you for removing videos from youtube

      As Peter mentioned it will be great if you delete whole post

    • Rob
      Ansys Employee
      and 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.
    • happykiran
      Subscriber
      Thank 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
  • You must be logged in to reply to this topic.