I'm new to FEMAP. I would like to represent a component with rigid material. How do I do it?
Does it have a rigid material so that I can assign it to the part? Please help me.
In Finite Element Method we can say that something is rigid only in a relative sense, depends of the comparison. For instance, in the material sense if you use a YOUNG module material property value that is 100 times bigger than the other material properties in your FE model, then this is a rigid material.
But if you are looking for a rigid joint to connect different portions of your FE model, then I suggest to use the RBE2 rigid element. The RBE2 provides a very convenient tool for rigidly connecting the same components of several grid points together.
For instance, RBE2 Rigid Elements can be used to transmit rotations between Solids and Shells and Solids and Beams by coupling the nodal rotations on the plate/beam elements to the nodal translations.
Please note that if you use adjacent elements whose stiffness differ by several orders of magnitude can produce an ill-conditioned stiffness matrix, which leads to problems when solving the model. For example, if you were to use a CBEAM element with extremely large moment inertia values to simulate a rigid connection, an ill-conditioned stiffness matrix would likely arise.
The RBE2 element uses constraint equations internally to couple the motion of the dependent degrees of freedom to the motion of the independent degrees of freedom. Consequently, RBE2 elements do not contribute directly to the stiffness matrix of the structure and ill-conditioning is avoided, OK?. Then you can use RBE2 elements riskless, instead to use extremely rigid material properties, not all is valid in FEA!!.
Thanks Blas for your reply.
Can I create rigid connection region using surfaces of a component (3D model) to represent it as a rigid body?
Lets assume there are 2 plates on top of each other. Can I create 2 rigid connection regions using the surfaces of these plates and create a connection between them? If this works, we need not mesh those 2 plates right?
You can connect rigidly two surfaces using RBE2 rigid elements, yes, you have available the macro under CUSTOM TOOLS > MESHING > CONNECT NODES ON SURFACES USING RIGID ELEMENTS, yes.
Also, you can use GLUE surface-to-surface connection and GLUE EDGE-TO-SURFACE, and GLUE EDGE-TO-EDGE as well, this is my favourite connecting method when I have to define a rigid joint between components, the reason is because RBE2 can produce local stress concentrations that are difficult to explain to others because the discrete nature of the joint; instead GLUE is more natural and
GLUE is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in an accurate strain and stress condition at the interface. The grid points on glued edges and surfaces do not need to be coincident. Glue creates stiff springs or a weld like connection to prevent relative motion in all directions.
To learn more about GLUE contact take a look to my blog in the following address:
To understand better your connection problem, post a picture or an sketch (or a FEMAP model) to help us to form a correct idea, OK?.