mean contact pressure static structural

bokaJbokaJ Member Posts: 28
edited February 17 in Structural Mechanics

Hallo erveryone,

I want to find out the mean contact pressure of two bodies. Below you can see the contact pressure with the display option "averaged".


Below you can see the contact pressure with the display option "unaveraged".

These two solutions are nearly the same, so I think that my mesh is fine enough.

I want to find out the force at which the mean contact pressure is less than 50MPa. So I set Contact Misscellaneous and Nodal Forces to YES at the output controls.

I inserted a force reaction where I choose for Contact Region the contact I am intereseted in. I get following solution:

When I divide the Force reaction of 63809N throug the contact area of 782mm^2 I get 81,6N/mm^2. But when I look at the contact pressure above, I think that that can not be true. In my opinion this is way too high.

You can see my contact definition bellow:

You can see the contact area below:


Can anyone help my the get the mean pressure of my contact or has an idea what I have done wrong?


Thank you an best regards,

bokaJ

Best Answer

Answers

  • 1shan1shan Ansys Employee Posts: 109
    edited February 17

    Hello @bokaJ,

    Have you created multiple contacts with the same contact face? In the picture I see that 2 ribs are flushing with the red contact region but only one sleeve is selected as target face. If you have created multiple contact with the same contact face you may combine them in a single contact and see if the issue persists. Since the contact is asymmetric the values are computed at the contact face, so the force which you are seeing might be an addition from multiple contact pairs. You may also switch the behavior to symmetric and see if it makes any difference.

    Regards,

    Ishan.

  • bokaJbokaJ Member Posts: 28

    Hallo Ishan,

    Thank you for your quick answer.

    I am not sure what do you mean with multiple contact.

    I am just interested in the mean pressure on the first rib. So I made two contacts. The first contact was between the red area and the inner rib and the second one was between the outer rib and the red area. And then I plotted just the rraction force of the contact of the inner rib.


    Am I getting you wrigt that in your opinion it could be possible that I see the addition of the contact force of the inner and the outer rib, because they have the same contact body(the red one)?

    I am not sure how I can switch the behavior to symmetric. Or did you mean that I should use a symmetric boundary condition instead of the frictionless support?

    Thank you very much for your time.

    Best regards

    bokaJ

  • 1shan1shan Ansys Employee Posts: 109
    Accepted Answer

    Hello @bokaJ,

    That's correct, it might be an addition of the contact force of inner and outer rib(though I am not 100% sure). Create a single contact in which the inner and outer ribs are defined as target faces rather than 2 different contact. For symmetric contact, go to contact behavior>symmetric. You could read about this in the help documentation -

    Definition Settings (ansys.com)

    Regards,

    Ishan.

    https://forum.ansys.com/discussion/3978/how-to-access-the-ansys-online-help

  • bokaJbokaJ Member Posts: 28

    Thank you Ishan,


    it has worked. I splitted the red area into two areas. You can see my new contacts bellow:


    Now I get a mean pressure on the inner rib of about 10 N/mm^2 and if I look at the contact pressure this looks quiet logical.


    Thank you very much!!

    Best regards

    bokaJ

  • bokaJbokaJ Member Posts: 28

    If I sum up the reaction force of the two splitted areas, then I get the reaction force which I get before. So your guess was correct!

Sign In or Register to comment.