Ansys Learning Forum Maintenance

NOTICE: We will be performing backend maintenance of our Learning Forum from April 5 to April 12, 2021. The result will be a new infrastructure but with little impact to user experience and design. Currently the forum is accessible in read-only mode as we complete our final migration. Thank you for your patience. For urgent issues please visit HERE.


How can a simply supported boundary condition be defined in a solid model? — Ansys Learning Forum

How can a simply supported boundary condition be defined in a solid model?

For example in the beam model, one can specify the following boundary condition at both the ends of a slender circular bar:

Ux = Uy = Uz = 0 ;

Rx = Ry = Rz = free

If a solid model is used instead of a beam model, applying Ux = Uy = Uz = 0 at the end faces would also arrest rotational degrees of freedom on those faces and it would act as a fixed boundary condition.

So how can a simply supported condition be applied in the solid model?

Answers

  • peteroznewmanpeteroznewman Member Posts: 11,369

    @ashansys

    Select the end face of the solid and select Remote Displacement from the Support category. You can fix three translations and leave the three rotations Free. Repeat on the other end except you cannot leave three rotations free at both ends. One end must have rotation about the axis along the beam length set to zero, otherwise the solver would see a zero pivot error. This is true for a beam model and a solid model with Remote Displacements.

  • ashansysashansys Member Posts: 3

    @peteroznewman@peteroznewman Thanks for the answer. I am aware of the option of applying remote displacements on remote points created with surfaces, however, I am looking for answers based on the physics of formulations of 1D and 3D elements.

  • peteroznewmanpeteroznewman Member Posts: 11,369
    edited March 18

    @ashansys

    The answer I gave is how to create a pinned connection on 3D solid elements meshed on a solid body. This gives the same boundary conditions as a 1D beam. I can only add that you should set the Behavior of the Remote Displacement as Rigid to fully match the 1D beam condition. What information is missing?

    Are you asking how to do that if you just have nodes and elements and no solid body?

  • ashansysashansys Member Posts: 3

    @peteroznewman

    In a way, yes!

    So I want to know whether the answer can be derived from the very basics, i.e. based on various elemental formulations? For example for Euler Bernoulli beam theory or Timoshenko beam theory for beam models vs solid models.

  • peteroznewmanpeteroznewman Member Posts: 11,369

    @ashansys

    ANSYS BEAM188 implements Timoshenko beam theory, which includes Shear Deformation, so will have the closest agreement with a solid model.

    ANSYS BEAM4 implements Euler-Bernoulli beam theory, which ignores Shear Deformation, so will differ from a solid model, especially for short beam lengths.

    Solid elements will need about 4 quadratic elements or 8 linear elements through the thickness of the beam to accurately capture the bending stress.

Sign In or Register to comment.