Fixed Vs Pinned Boundary Condition

General Questions
1

Hi,
I have done the analysis of a circular beam element in PrePoMax both in pinned and fixed boundary condition for the same load also. But the displacement results are same. Could any one please help me to solve this. I am attaching the analysis file with this.
Thank You
Tomin Mathew

We Transfer File: WeTransfer - Send Large Files & Share Photos Online - Up to 2GB Free

2

Nodes of solid elements don’t have rotational degrees of freedom so there’s no difference when you release these DOFs. You have to use constraints like rigid body to control rotations. In this case, you can add these constraints at the ends of the bar and apply proper boundary conditions to the reference points.

1 Like
3

Did you mean, Whether I give fixed or pinned it will restrain all translation and rotation for solid.

4

Setting fixed will only fix translations for solid elements, boundary conditions on rotational DOFs will be ignored by the solver (often there’s a warning).

1 Like
5

How can we fix a solid element in rotation?

6

Via a rigid body constraint or coupling constraints (not yet supported in PrePoMax). It constrains the motion of nodes to the motion of a reference point which can also handle rotations. Check this tutorial, for example: PrePoMax (CalculiX FEA) - Tutorial 2 - Torsion of an elliptical bar - YouTube

7

I have made some changes as per you said, but the results are same as the
Fixed.pmx (2.3 MB)
earlier. Could you please check the analysis file.

8

They will be the same for the fixed case but should be different for the pinned one, when you release rotation.

9

Can I conclude that it’s not possible to assign fixed support to solid elements?

10

It actually depends on how you want to apply such support. Let’s consider 3 possible scenarios:

  1. Fixed support applied to a face - blocking all translations of solid elements’ nodes will be sufficient - the model won’t move
  2. Fixed support applied to an edge - blocking all translations of solid elements’ nodes won’t be sufficient - the model will be able to rotate about that edge so it won’t be a truly fixed support. In the case of elements supporting rotational DOFs at nodes (shells or beams), you can also constrain rotations and the model won’t be able to rotate about the edge and thus you will have true fixed support.
  3. Fixed support applied to a point - as above but the model will be able to rotate about the point. In the case of shells and beams, you can fix it preventing rotation. Another thing is that applying a fixed constraint to just a single node of a shell is not a good idea.
1 Like
11

It is important to understand how the FEM works. The basis is the finite element mesh that consists of nodes and elements. The nodes of the mesh are the only items where loads and supports are applied, and elements are only used to connect the nodes. So when you select a surface and apply a load or a boundary condition what happens is that your are actually selecting all nodes of the surface.

If you consider the analytical support shown in the image (top image), it is rotational support. Now you would like to have the same support type on your solid model, so you selected the left surface in your component and applied the translational constraints x = y = z = 0. But you left the rotational constraints (DOF) free and thought the component would rotate. But it cannot rotate since you applied the translational constraint to all nodes of the selected surface. So all three red nodes in the image (middle image) are fixed. They cannot move. So the component cannot rotate.

What you need to do is to create a single point in the middle of the surface you selected and then apply the boundary conditions only to that single point (bottom image). Only that will work in the same way as in the analytical model. When the rotations are unconstrained, the point can rotate.

image

3 Likes
12

Thank you so much for the explanation.