Learning Forum

[jfm418]

Hello,

I am trying to induce beam bending by applying a displacement on only one surface of the beam. (stretching one surface and expecting the opposite surface to compress.)

I am getting some deflection for small displacements but when I increase the displacement I do not see nice curvature and I am not sure why. I am applying a fixed support on one end of the beam and uniaxial displacement in one direction along the beam while leaving the other 2 directions free. I actually get some curvature but it is in the wrong direction (concave instead of convex). The bottom side is where the displacement is applied. (attached is the example but it is not showing a preview for some reason)

Any advice would be greatly appreciated.

Thanks a lot.

Jad

[peteroznewman]

Jad, you have the wrong idea about how the surface displaces to make a nice curvature. You should not use displacement, it doesn't give you want you want. It would be better to apply a different strain to the top half than the bottom half.  That will result in a surface displacement that starts at zero at the fixed end and is a maximum at the other end.

I suggest you slice the body into two bodies and put the bodies into a multibody part in DesignModeler to use Shared Topology. Duplicate the material you are using and call it Bottom, and edit the CTE on that material and make it 10 times larger and assign that material to the bottom body, while the original material is assigned to the top body.  Now use a Temperature Condition and raise the temperature by 10C. That will cause the material on the bottom to get larger and the beam will bend up. Use a higher temperature to get more bend.

Under Analysis Settings, you have to turn on Large Deflection.   You might also have to turn on Auto Time Stepping and set the Initial Substeps to 10.

[jfm418]

Brilliant! This worked really well. Thanks a lot.

I do get the following 2 warnings that I do not completely understand:

The maximum contact stiffness is too big. This may affect the accuracy of the results. You may need to scale the force unit in the model.

 

An iterative solver was used for this model. However, a direct solver may enhance performance. Consider specifying the use of a direct solver.

 

I was also wondering if I need to pay any particular attention to the meshing of the 2 slices. I currently have them both set at the same refinement element.

Sorry if any of these are trivial questions. I am new to ANSYS.

Thank you again so much for your help.

Jad

[peteroznewman]

Mechanical is configured to automatically add contacts to faces that are touching. I don't like that default and turn it off. In your case, you have Shared Topology holding the two bodies together. Your model doesn't need any contact, right?  Just delete that contact and the first warning will go away.

If you only waited a few seconds to solve, then you can ignore the second warning. But if you waited a few minutes, then under Analysis Settings, there is a line that says Solver and is Program Controlled. Change that to Direct and see if the solution takes less time.

As long as you have at least two elements through the thickness of each layer, that will be fine.  You could use SOLSHELL190 elements which are slightly better at thin solids that bend. You have to use a mesh control to sweep each body through its thickness, picking a Source Face as the top or bottom face.