Learning Forum

[j.drozdowski]

Hello. I've got construction like this - two  UPN profiles connected with plate.


I would like to make a connection between bodies by RBE2 elements.
I define a Joint element but it is making spider curve connecting all edges in one point and then distributing it to nodes on the other body.

The effect which i would like to achieve should look like on picture below.
Does anyone know how to achieve that resultant ?
Thank you.

[peteroznewman]

I see you have selected Rigid as the connection between the four lines. You say RBE2 elements, but that is a NASTRAN term.  The ANSYS term is CERIG. Fixed Joints work by using Spiders from a node at the coordinate origin created for the joint. The joint is set to Rigid which is effectively making the entire rectangular pad rigid, adding stiffness to the model that you don't want. I see what you do want and in other software, that is easy to do. It's not so easy to do in Mechanical.

I assume you want to model these four edges being welded. I recommend you use Bonded Contact, Formulation = MPC to connect the four edges. This will connect the edges without adding stiffness.

If you want to add some stiffness to represent the weld bead, you can add a Bonded Contact, Formulation = Beam.
Note that you can define the Material, which could be a higher stiffness material, and the Radius of the circular beam section.

You will have also read my reply in the other thread.

[j.drozdowski]

Thank you Peter. I've tried it and it works.
If I understand well if I would like to use substitute of RBE2 element in this case I can always define fake material with very high Young modulus and this short beams would work as rigid. Am I right ?

[peteroznewman]

Yes, that is the idea. Also you can define higher beam radius cross-section to increase stiffness.

[Erik Kostson]

We do have rigid type of Element similar to RBE2.

We need a command snippet where we define loads and bc.

To convert the beam 188, we need to define them so say, et, 1000,mpc184. Then select the beams with esel, s, ename,, 188. Finally use the emodif command, emodif, all, type, 1000. This is on top of my head so check the command in our help manual.

[peteroznewman]

Good to know, thanks ekostson.

@jdrozdownski, you can read about MPC184 in Mechanical APDL section of the Help system in Chapter 7, Element library.  Look at MPC184-Link/Beam where you can define a Rigid Link.  Below is the URL

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_elem/Hlp_E_MPC184link.html

Follow these instructions to use that URL in the Student license.

From the help, I read the following:

If KEYOPT(1) = 0 (default), the element is a rigid link with two nodes and three degrees of freedom at each node (UX, UY, UZ). If KEYOPT(1) = 1, the element is a rigid beam with two nodes and six degrees of freedom at each node (UX, UY, UZ, ROTX, ROTY, ROTZ).

If KEYOPT(2) = 0 (default), then the constraints are implemented using the direct elimination method. If KEYOPT(2) = 1, then the Lagrange multiplier method is used to impose the constraints.

You will need to use KEYOP(1) = 1 because by default, there will only be 3 DOF and that parallel array of links will be a mechanism and the solver will have a zero pivot error.  You need 6 DOF at each end.

Later in the help, you can read this:

Direct Elimination Method (KEYOPT(2) = 0)

These additional restrictions apply to the direct elimination method:

• 
  

  This element cannot be used in a distributed solution when the direct elimination method is used.

  
  

You will need to use KEYOP(2) = 1 because by default, you can't use a distributed solution.  I always use a distributed solution and that is the default when ANSYS is installed.