Learning Forum

[Aslinn]

 Hi, I am comparing different ways to connect the beam element and shell element. The example I used is to support a slab with beams. I used two ways to connect:

1. Set the beam and surface to share topology in SpaceClaim, and no connection setting in Mechanical;

2. No setting in Spaceclaim, but set the beams to be bonded with the surface in Mechanical.

It was found the deflection difference in beams is negligible, while the deflection different in the slab is about 6%.

Therefore, I wonder which is the most accurate way to simulate such a situation?

[Sandeep Medikonda]

You can also use define mesh Connections and define a Manual mesh Connection. You can also use Node Merge, but I often recommend against these 2 methods as it can cause extremely distorted meshes.

In your bonded contact definition, I would recommend you to double-check the constraint type and use MPC....This way you can couple your degrees of freedom accordingly and have more control.

To summarize, you can connect a Beam to Shell using the following ways:

• Multibody Part


• Mesh Connection


• Node Merge


• Bonded Contact

[Aslinn]

Hi SandeepMedikonda, thank you for your reply. One strange thing is that I don't see the 'target normal, couple U to ROT' option under constraint type. As shown below, the one more option it does show is 'program controlled'. I'm using 2019 R2 student version. Did I miss any step?

[Sandeep Medikonda]

That snapshot is from an older version and it is also possibly dependent on the scoping element type/analysis even. Please refer to the help on the options you have in 2019R2.

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v194/wb_sim/ds_Contact_Advanced.html

So, when you are trying to couple U to ROT, this is nothing but to use Distributed, All Directions, i.e., Rotational DOFs are bound to Translational DOFs

[Aslinn]

Hi, thank you very much for the clarification. To expand, connections between different elements, such as connection beam element to shell element, beam element to solid element, shell element to solid element, etc., are essentially bounding the mesh nodes. Different results from different connection approach is coming from different mesh option. Is my understanding correct?

[Sandeep Medikonda]

Yes, Shell and Beam elements have 6 degrees of freedom (3 translation + 3 rotational), whereas solid elements have only 3 (translational only) degrees of freedom. The coupling with add constraints to account for any mismatch.