Shell slide on rigid body

Hallo.

I am quite new in ANSYS and have a problem with my model.

I have a part which is made of lot of shells. This part should slide on the rigid body, see figure 1.

The part should be able to move in the positive z-direction, but not step throug the rigid body (negativ z-direction).

In Figure2 you see the connection between the shells and the rigid body.

You see the details of the rigid body in figure3.

When I start my calculation i get the error "Not enough constraints..".

I want to get an fixed support on the rigid body. Can anyone tell my how to do this?


I also tried to use an "Compression Only Support" instead of the rigid body, but I can not choose my shells there fore.


Thank you

bokaJ

Best Answers

  • peteroznewmanpeteroznewman Posts: 12,000Member
    edited October 2020 Accepted Answer

    @bokaJ

    Delete the Fixed Joint, Body-Body.

    Insert a Fixed Joint, Body-Ground, and select only the Rigid Body.

    Insert a Contact between the Rigid Body and the 11 faces of the floor of the structure. The Rigid Body face must be on the Target side. Make the Contact type be Frictional or Rough. A rough contact will not slide on the rigid body, but can separate. You want to see the blue color on the opposite side to what you show in the image above. You do this by setting the Contact Side to Bottom instead of Top.

    Under the Connections folder, insert a Contact Tool and Generate Initial Contact Status. The Frictional or Rough contact must show as Closed.

    Under Analysis Settings, turn on Auto Time Stepping. Set the Initial Substeps to 100.

  • peteroznewmanpeteroznewman Posts: 12,000Member
    edited October 2020 Accepted Answer

    @bokaJ

    You can either put two surface bodies on the same plane and leave Shell Thickness Effect turned off, or

    you can put the two midsufaces 15 mm apart and turn on Shell Thickness effect.

    In either case, the thickness assigned to the surfaces is 7.5 mm.

    Contact algorithms allow a very small penetration to be used to compute the contact force needed to prevent large penetration. You can control the size of that very small penetration by altering the Normal Contact Stiffness Factor. The default value is 1, you can increase it by a factor of 10 or 100.

    You can insert a Contact Tool on the Solution branch and insert a Penetration plot on that tool. That will show the value of penetration as a contour plot. Note that the Deformation Result is often scaled to look 1000 times more that reality. Set the Result Deformation Scale to 1.0 (True Scale).

    https://forum.ansys.com/discussion/14332/deformation-scale

Answers

  • bokaJbokaJ Posts: 31Member

    @peteroznewman

    Thank you very much for your quick and very helpful answer.

    As you can see in the following picture, the deformation looks as expected.


    But there is a slight step through at some areas. In my opinion this should not be possible?

    On the picture below, you can see the details of the contact between the rigid body and the shell body.

    On the picture below you can see the initial information of the contact.

    For the hickness of the shell and the rigid body I choose 15mm. But I put the rigid body directly on the shell, or should I leave a gap of 15mm(=7,5+7,5) between the shell and the rigid body?

    Would you possibly so kind as to help me again with this problem?


    Thank you a lot,

    bokaJ

  • bokaJbokaJ Posts: 31Member

    thank you very much sir!

    the maximum penetration is about 0,001mm.

    I learned a lot from you!


    Best regards

    bokaJ

Sign In or Register to comment.