# How to incorporate moment release at beam end in FEM formulation?

I have a structure with a lot of interconnecting column and beam frame elements. I want to compute the displacement, member forces/moments via Finite Element Method.

The problem now is that I don't know how to properly incorporate moment release at beam end. I understand that moment release means that at the beam's end, the bending moment is $0$, but I don't know how I can incorporate this piece of information ( as a boundary condition? Or as a form of penalty function, or...?) into my FEM model.

I know how to incorporate support into my FEM model though; I can just make the relevant appropriate stiffness terms very big. But not moment release.

Any idea how moment release can be formulated in finite element terms to achieve the desired end results?

Note:

This question is different from the one that I asked here, because that one asked about mathematical formulation ( more on conceptual level), whereas this one asks about explicit FEM formulation. These two maybe related, but to go from previous question to this one is by no means trivial, and the connection not easy to see.

• – Wasabi
Oct 28 '16 at 10:08
• @Wasabi, I'm not sure whether they are exact duplicate-- this question explicitly ask about an explicit FEM formulation, but the another doesn't. Oct 28 '16 at 10:18
• Wouldn't the answer to this depend on the exact FEM program used? Or are you asking in general terms? If it is in general terms, I don't see how it is different than the mathematical question.
– hazzey
Oct 28 '16 at 12:55
• @hazzey, that's my point. What "exact FEM program" approach that you have in mind? If the answer is depending on the exact FEM program, then maybe you can outline some FEM program approaches and explain how they handle moment release? So it is very different from the conceptual mathematical question Oct 28 '16 at 13:59
• @Graviton Hazzey means that different commercial FE programs (Nastran, Abaqus, Ansys, etc) have different ways of specifying this in the input. For example in Nastran you can specify "pin flags" to "unpin" individual rotation variables at a grid point. You don't need to know how the math works at this level of detail to use the software correctly. Oct 28 '16 at 22:06

Conceptually, all you have to do is not assemble the "released" rotation variable to anything else in the system stiffness and mass matrices.

Apart from keeping track of the "extra" variables at some nodes in the model, everything else in the FE method "just works" without needing any special math.

Another way is to eliminate the "released" variable(s) from the element matrices before you assemble them into the global matrices. In that case, you need to keep track of what you did, so you can undo it when you want to recover the element stresses, etc.

In the general situation, you might also need to create a local coordinate system at the grid (node) point, so you have a single rotation variable in each orientation that you want to "release".

Note, the same technique is sometimes useful with translation variables as well as rotations - for example, if you are modeling a spline joint where the two parts can move relative to each other along the line of the joint, but the other two translations and all three rotations can transmit forces and moments across the joint.

• I am aware that at conceptual level, not assembling released rotation is the way to go. But practically, doing this might a) fraught with numerical difficulties, b) may not take care of the sparseness of the stiffness matrix, I'm interested in what are the numerical methods best for this scenario? Oct 29 '16 at 2:22
• btw, do you have any reference on such methods? Books or articles are welcome Oct 29 '16 at 2:23
• Another way is to eliminate the "released" variable(s) can you be more precise on how to do this? Oct 31 '16 at 8:01
• Not assembling the DOF can leave an unconstrained rotation if no other beams use that node. Either don't allocate space for that DOF in the global matrix, put an arbitrary stiffness on the diagonal, or use a more robust matrix solver that doesn't mind. Dec 28 '16 at 8:56

Make use of the DOF numbering as "indices" pertaining to the element stiffness coefficients in facilitating the aggregation of the global direct stiffness matrix.

Adding a moment release would make the rotational displacements of the connecting member distinct from each other right? So, define a node at the joint where you will apply a moment release, then assign a distinct DOF number for the rotational displacements of each of the connecting members.

The default type of connection in plane frame is RIGID that has 3 DOF's (1- Horizontal displacement; 2- Vertical displacement ; 3- Rotational displacement). If you apply moment release at the connection, then the DOF is increased by one, representing the distinction of the rotational displacements of each member. (1 & 2 translational displacements at the node; 3-rotational displacement of member 1 and 4 - rotational displacement of member 2). Then proceed with establishing the global direct stiffness matrix.